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Geometry

Table Of Contents
Geometry: Overview ...................................................................................... 1 What's New? ................................................................................................. 3 New Functionalities...................................................................................... 3 Enhanced Functionalities .............................................................................. 3 Getting Started ........................................................................................ 4 Basic Tasks.............................................................................................. 4 Creating Wireframe Geometry .................................................................... 4 Creating Surfaces ..................................................................................... 4 Performing Operations on Shape Geometry .................................................. 4 Editing Surfaces and Wireframe Geometry ................................................... 5 Using Tools.............................................................................................. 5 Advanced Tasks Managing Geometrical Sets and Ordered Geometrical Sets ...... 5 Customizing Settings ................................................................................... 5 Generative Shape Design ................................................................................ 7 Generative Shape Design: Overview .............................................................. 7 Generative Shape Design in a Nutshell......................................................... 7 Before Reading this Guide.......................................................................... 7 Getting the Most Out of this Guide .............................................................. 8 Accessing Sample Documents..................................................................... 8 Getting Started ........................................................................................... 8 Getting Started ........................................................................................ 8 Lofting, Offsetting and Intersecting ............................................................. 9 Splitting, Lofting and Filleting ....................................................................11

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geometry Sweeping and Filleting..............................................................................14 Transforming the Part ..............................................................................18 Entering the Generative Shape Design Workbench .......................................19 Basic Tasks ...............................................................................................21 Basic Tasks.............................................................................................21 Creating Wireframe Geometry ...................................................................22 Creating Surfaces ..................................................................................133 Performing Operations on Shape Geometry ...............................................216 Editing Surfaces and Wireframe Geometry ................................................315

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Geometry: Overview
The Geometry workbench allows the designer to create the underlying geometry of a form, including points, lines, planes, and 2d profiles that combine in various ways to form wire frames, surfaces, and solids. This workbench allows designers to quickly model both simple and complex shapes using wire frame and surface features, providing a large set of tools for creating and editing shape designs. Since this feature is integrated into Geometry, it meets the requirements of solid-based hybrid modeling. The geometry of the part is incorporated in the Project workbench either when the part is included (bottom-up design) or later specified (top-down design) in the Geometry workbench. The Geometry workbench includes one other workbench:

Sketcher workbench enables designers to sketch precise The affiliated and rapid 2D profiles. These profiles can then be used singly or in combination to create solids and surfaces.

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What's New?
New Functionalities
Working with a 3D Support The Work On Support 3D capability allows you to automatically reference surfaces or planes as supporting elements whenever required. Creating Associative Isoparametric Curves This new command allows you to create associative isoparametric curves, any modification of the support associated with the curve modifies the curve. Extracting Multiple Elements This new functionality allows you to extract sub-elements (curves, points, surfaces, solids, volumes and so forth) that are joined into one element Instantiating a Power Copy Using a VB Macro This new functionality allows you to instantiate a Power Copy using a VB macro Creating Developable Surfaces This new functionality allows you to create developable surfaces from two curves

Enhanced Functionalities
Interruptions of computations when creating or editing all types of fillets or Boolean operations You can now interrupt geometry computations if needed, which lets you save time especially when working on complex parts. Boolean Operations You can now modify specifications for Boolean operations Previewing results prior to confirming operations is now possible for all Boolean features Shaft You can now select axes that are not included in the profile plane Rectangular Pattern A new parameter lets you assign distinct spacings between each instance Replace Face Replacing faces with other faces belonging to the same body is now possible, which in many cases simplifies geometry Deactivating Elements Two new options are now available: Delete all children and Deleted aggregated elements Rotations Two new rotation modes are now available: Axis-Two Elements and Three Points Point Coordinates: you can now specify a current local axis system On plane: if selecting an axis system as the plane, the reference point is automatically filled with the origin of the axis system On surface: you can now choose the dynamic positioning of the point: coarse (existing behavior) or fine Plane

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geometry Angle/Normal to plane: a new option enables you to project the rotation axis onto the reference plane. Equation: you can now specify a current local axis system

Getting Started
Entering the Workbench A new option is available in the New Part dialog box to insert an ordered geometrical set in the part to be created

Basic Tasks Creating Wireframe Geometry
Creating Points Coordinates: new Axis System field to specify a current local axis system On plane: if selecting an axis system as the plane, the reference point is automatically filled with the origin of the axis system On surface: you can now choose the dynamic positioning of the point: coarse (existing behavior) or fine Creating Planes Angle/Normal to plane: new Projecting the rotation axis on the reference plane option Equation: new Axis System field to specify a current local axis system Creating Circles Two point and radius type: you can now select a direction as Support Creating Parallel Curves New 3D smoothing option to enable a smoothing without selecting a surface Creating Projections New 3D smoothing option to enable a smoothing without selecting a surface

Creating Surfaces
Creating Extruded Surfaces You can now extrude up to a geometric element, that is a surface, a plane or a point Creating Blended Surfaces You can now specify a curve as spine

Performing Operations on Shape Geometry
Joining Geometry In case a check fails, elements in error are now highlighted in the 3D geometry Trimming Geometry New Pieces mode to let you select several curves to be trimmed Translating Geometry New Axis System field to specify a current local axis system Rotating Geometry New rotation modes: Axis-Two Elements and Three Points Extrapolating Surfaces New options: Constant extrapolation distance and Extend extrapolated edges

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What's New

Editing Surfaces and Wireframe Geometry
Editing Parameters When a feature's dimension is computed geodesically, parameters are displayed in the 3D geometry Deactivating Elements New Delete all children and Deleted aggregated elements options (as in Delete)

Using Tools
Stacking Commands All GSD commands can now be stacked New Axis System field to specify a current local axis system when editing the components' directions. You can now select the Compass Direction to create an infinite line corresponding to the Z axis of the current compass direction Selecting Using Multi-Output Selection of an element: it is highlighted in both the specification tree and 3D geometry New behavior when selecting one or several elements Managing Warnings You can now center the graph and reframe on the selected feature There is now a warning message when an optional element is deleted

Advanced Tasks Managing Geometrical Sets and Ordered Geometrical Sets
Managing Ordered Geometrical Sets Some features are grayed out at edition

Customizing Settings
Create a Geometrical Set Geometrical sets can now be located above Part Bodies in the specification tree. Create an Ordered Geometrical Set Available from the Part Document tab of the Options dialog box, the Create an Ordered Geometrical Set option lets you create ordered geometrical sets (OGSs) when creating a new part. Enable hybrid design inside part bodies and bodies If in the course of your CATIA session you deactivate the Enable hybrid design inside part bodies and bodies option, icons identifying existing bodies likely to include wireframe and surface elements turn yellow. This new behavior ensures that both types of bodies (bodies and solid bodies) can be quickly identified within the same document. Selection focus This new setting allows you to display a full cross cursor for the selection.

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Generative Shape Design
Generative Shape Design: Overview
Welcome to the Generative Shape Design User's Guide ! This guide is intended for users who need to become quickly familiar with the product. This overview provides the following information: • Generative Shape Design in a Nutshell • Before Reading this Guide • Getting the Most Out of this Guide • Accessing Sample Documents • Conventions Used in this Guide

Generative Shape Design in a Nutshell
The Generative Shape Design workbench allows you to quickly model both simple and complex shapes using wireframe and surface features. It provides a large set of tools for creating and editing shape designs and, when combined with other products such as Part Design, it meets the requirements of solid-based hybrid modeling. The feature-based approach offers a productive and intuitive design environment to capture and re-use design methodologies and specifications. This new application is intended for both the expert and the casual user. Its intuitive interface offers the possibility to produce precision shape designs with very few interactions. The dialog boxes are self explanatory and require practically no methodology, all defining steps being commutative. As a scalable product, Generative Shape Design can be used with other Version 5 products such as Part Design and FreeStyle Shaper and Optimizer. The widest application portfolio in the industry is also accessible through interoperability with CATIA Solutions Version 4 to enable support of the full product development process from initial concept to product in operation. This User's Guide has been designed to show you how to create and edit a surface design part. There are numerous techniques to reach the final result. This book aims at illustrating these various possibilities.

Before Reading this Guide
Before reading this guide, you should be familiar with basic Version 5 concepts such as document windows, standard and view toolbars. Therefore, we recommend that you read the Infrastructure User's Guide that describes generic capabilities common to all Version 5 products. It also describes the general layout of V5 and the interoperability between workbenches.

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geometry You may also like to read the following complementary product guides: • Part Design User's Guide

Getting the Most Out of this Guide
To get the most out of this guide, we suggest that you start reading and performing the step-by-step Getting Started tutorial. This tutorial will show you how create a basic shape design part. Once you have finished, you should move on to the Basic Tasks and Advanced Tasks sections, which deal with handling all the product functions. The Workbench Description section, which describes the Generative Shape Design workbench, and the Customizing section, which explains how to set up the options, will also certainly prove useful. Navigating in the Split View mode is recommended. This mode offers a framed layout allowing direct access from the table of contents to the information.

Accessing Sample Documents
To perform the scenarios, sample documents are provided all along this documentation. For more information on accessing sample documents, refer to Accessing Sample Documents in the Infrastructure User's Guide.

Getting Started
Getting Started
Before getting into the detailed instructions for using Generative Shape Design, the following tutorial aims at giving you a feel of what you can do with the product. It provides a step-by-step scenario showing you how to use key functionalities. The main tasks described in this section are:

This tutorial should take about 20 minutes to complete. You will use the construction elements of this part to build up the following shape design.

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What's New

Lofting, Offsetting and Intersecting
This task shows you how to create a multi-sections and an offset surfaces as well as an intersection. 1. Click the Multi-sections Surface icon .

The Multi-sections Surface Definition dialog box appears. 2. Select the two section curves. 3. Click within the Guides window then select the two guide curves.

4. Click OK to create the multi-sections surface.

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geometry

5. Click the Offset icon

.

6. Select the multi-sections surface. 7. Enter an offset value of 2mm. The offset surface is displayed normal to the multi-sections surface.

8. Click OK to create the offset surface.

9. Click the Intersection icon

.

The Intersection dialog box appears. 10. Select the offset surface then the first plane (Plane.2) to create the 10

What's New intersection between these two elements.

11. Click OK in the dialog box.

The created elements are added to the specification tree:

Splitting, Lofting and Filleting
This task shows how to split surfaces then create a multi-sections surface and two fillets.

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geometry

1. Click the Split icon

.

The Split Definition dialog box appears. 2. Select the offset surface by clicking on the portion that you want to keep after the split. 3. Select the first plane (Plane.2) as cutting element. 4. Click OK to split the surface.

5. Repeat the previous operations by selecting the multi-sections surface then the second plane (Plane.3) to define the intersection first, then to cut the surface. 6. Click OK to split the surface.

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What's New

7. Click the Multi-sections Surface icon

.

The Multi-sections Surface Definition dialog box appears. 8. Select the intersection edges of the two split surfaces as sections.

10. Click OK to create the multi-sections surface between the two split surfaces.

11. Click the Shape Fillet icon

.

The Fillet Definition dialog box appears. 12. Select the first split surface as the first support element (Split.3). 13. Select the multi-sections surface you just created as the second support element (Multi-sections Surface.3). 14. Enter a fillet radius of 3mm. The orientations of the surfaces are shown by means of arrows.

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geometry

15. Make sure that the surface orientations are correct (arrows pointing down) then click OK to create the first fillet surface. 16. Repeat the filleting operation, clicking the icon, then selecting the second split surface as the first support element. 17. Select the previously created filleted surface as the second support element. 18. Enter a fillet radius of 3mm. 19. Make sure that the surface orientations are correct (arrows pointing up) then click OK to create the second filleted surface.

The created elements are added to the specification tree:

Sweeping and Filleting
This task shows how to create swept surfaces and fillets on both sides of the part. You will use the profile element on the side of the part for this. In this task you 14

What's New will also create a symmetrical profile element on the opposite side of the part. 1. Click the Swept Surface icon 2. Click the Explicit sweep icon. 3. Select the profile element (Corner.1). 4. Select the guide curve (Guide.1). 5. Select the central curve (Spline.1) as the spine. .

The Swept Surface Definition dialog box appears.

6. Click OK to create the swept surface.

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geometry

7. Click the Symmetry icon

.

The Symmetry Definition dialog box appears. 8. Select the profile element to be transformed by symmetry. 9. Select the YZ plane as reference element.

10. Click OK to create the symmetrical profile element. 11. Click the Sweep icon again.

12. Select the profile (Symmetry.3) and the guide curve (Guide.2). 13. Select the central curve (Spline.1) as the spine. 14. Click OK to create the swept surface.

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What's New

15. To create a fillet between the side portion and the central part click the Shape Fillet icon .

16. Select the side sweep element and the central portion of the part, then enter a fillet radius of 1mm (make sure the arrows are pointing up). 17. Click Preview to preview the fillet, then OK to create it. 18. Repeat the filleting operation between the other sweep element and the central portion of the part, and entering a fillet radius of 1mm (make sure the arrows are pointing up). 19. Click OK to create the fillet.

The created elements are added to the specification tree:

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geometry

Transforming the Part
This task shows you how to modify the part by applying an affinity operation. 1. Click the Affinity icon .

The Affinity Definition dialog box appears.

2. Select the end section profile to be transformed by the affinity. 3. Specify the characteristics of the axis system to be used for the affinity operation: • • • point PT0 as the origin plane XY as reference plane X axis as the reference axis.

4. Specify the affinity ratios: X=1, Y=1 and Z=1.5.

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What's New

5. Click OK to create the new profile. 6. Edit the definition of the multi-sections surface (Multi-sections Surface.1), by double-clicking it, then select the second section, click the Replace button and select the new profile. 7. Click OK in the dialog box. 8. If needed, click the Update icon to update your design.

Multi-selection is available. Refer to Selecting Using Multi-Output to find out how to display and manage the list of selected elements.

Entering the Generative Shape Design Workbench
This first task shows you how to enter the Shape Design workbench and open a wireframe design part. Before starting this scenario, you should be familiar with the basic commands common to all workbenches. These are described in the Infrastructure User's Guide. 1. Select Shape -> Generative Shape Design from the Start menu. The Shape Design workbench is displayed.

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geometry

The New Part name dialog box may appear depending on the way you customized your session. It provides a field for entering the name you wish to assign to the part, an option that enables hybrid design an two other options to insert a geometrical set and/or an ordered geometrical set in the part to be created. If you select Enable hybrid design inside part bodies and bodies, the capability then applies to all the bodies you will create in your CATIA session (and not only to the new CATPart document you are opening). Consequently, if your session contains CATPart documents already including traditional bodies, the new bodies you will create subsequently in these documents will possibly include wireframe and surface elements. To facilitate your design, It is therefore recommended that you do not change this setting during your session. For more information, refer to the Part Document chapter in Customizing section of the Part Design documentation.

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What's New

2. Select File -> Open and navigate to the samples directory. 3. Select the GettingStartedShapeDesign.CATPart document. A wireframe design part is displayed.

You can add the Generative Shape Design workbench to your Favorites, using the Tools -> Customize item. For more information, refer to the Infrastructure User's Guide. If you wish to use the whole screen space for the geometry, remove the specification tree by selecting the View -> Specifications command or pressing F3.

Basic Tasks
Basic Tasks
The basic tasks you will perform in the Generative Shape Design workbench will involve creating and modifying wireframe and surface geometry that you will use in your part. The table below lists the information you will find in this section.

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When creating a geometric element, you often need to select other elements as inputs. When selecting a sketch as the input element, some restrictions apply, depending on the feature you are creating. You should avoid selecting self-intersecting sketches as well as sketches containing heterogeneous elements such as a curve and a point for example. However, the following elements accept sketches containing non connex elements (i.e. presenting gaps between two consecutive elements) as inputs, provided they are of the same type (homogeneous, i.e. two curves, or two points): • • • • • • • • • Intersections Projections Extruded surfaces Surfaces of revolution Joined surfaces Split geometry Trim geometry All transformations: translation, rotation, symmetry, scaling, affinity and axis to axis Developed wires (Developed Shapes)

Creating Wireframe Geometry
Creating Wireframe Geometry
Generative Shape Design allows you to create wireframe geometry such as points, lines, planes and curves. You can make use of this elementary geometry when you create more complex surfaces later on. Create points by coordinates: enter X, Y, Z coordinates. Create points on a curve: select a curve and possibly a reference point, and enter a length or ratio. Create points on a plane: select a plane and possibly a reference point, then click the plane. Create points on a surface: select a surface and possibly a reference point, an element to set the projection orientation, and a length. Create points as a circle center: select a circle. Create points at tangents: select a curve and a line. Create point between another two points: select two points

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What's New Create multiple points: select a curve or a point on a curve, and possibly a reference point, set the number of point instances, indicate the creation direction or indicate the spacing between points. Create extrema: select a curve and a direction into which the extremum point is detected. Create polar extrema: select a contour and its support, a computation mode, and a reference axis-system (origin and direction) . Create lines between two points: select two points. Create lines based on a point and a direction: select a point and a line, then specify the start and end points of the line. Create lines at an angle or normal to a curve: select a curve and its support, a point on the curve, then specify the angle value, the start and end points of the line. Create lines tangent to a curve: select a curve and a reference point, then specify the start and end points of the line. Create lines normal to a surface: select a surface and a reference point, then specify the start and end points of the line. Create bisecting lines: select two lines and a starting point, then choose a solution. Create an Axis: select a geometric element, a direction, then choose the axis type. Create polylines: select at least two points, then define a radius for a blending curve is needed. Create an offset plane: select an existing plane, and enter an offset value. Create a parallel plane through a point: select an existing plane and a point. The resulting plane is parallel to the reference plane and passes through the point. Create a plane at an angle: select an existing plane and a rotation axis, then enter an angle value (90° for a plane normal to the reference plane). Create a plane through three points: select any three points Create a plane through two lines: select any two lines Create a plane through a point and a line: select any point and line Create a plane through a planar curve: select any planar curve Create a plane normal to a curve: select any curve and a point Create a plane tangent to a surface: select any surface and a point Create a plane based on its equation: key in the values for the Ax + Bu + Cz = D equation

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Create a mean plane through several points: select any three, or more, points Create n planes between two planes: select two planes, and specify the number of planes to be created Create a circle based on a point and a radius: select a point as the circle center, a support plane or surface, and key in a radius value. For circular arcs, specify the start and end angles. Create a circle from two points: select a point as the circle center, a passing point, and a support plane or surface. For circular arcs, specify the start and end angles. Create a circle from two points and a radius: select the two passing points, a support plane or surface, and key in a radius value. For circular arcs, specify the arc based on the selected points. Create a circle from three points: select three points. For circular arcs, specify the arc based on the selected points. Create a circle tangent to two curves, at a point: select two curves, a passing point, a support plane or surface, and click where the circle should be created. For circular arcs, specify the arc based on the selected points. Create a circle tangent to two curves, with a radius: select two curves, a support surface, key in a radius value, and click where the circle should be created. For circular arcs, specify the arc based on the selected points. Create a circle tangent to three curves: select three curves. Create conics: select a support plane, start and end points, and any other three constraints (intermediate points or tangents). Create spirals: select a support plane, center point, and reference direction, then set the radius, angle, and pitch as needed. Create splines: select two or more points, if needed a support surface, set tangency conditions and close the spline if needed. Create a helix: select a starting point and a direction, and specify the helix pitch, height, orientation and taper angle. Create corners: select a first reference element (curve or point), select a curve, a support plane or surface, and enter a radius value. 2. Creating connect curves: select two sets of curve and point on the curve, set their continuity type and, if needed, tension value. Create parallel curves: select the reference curve, a support plane or surface, and specify the offset value from the reference. Create projections: select the element to be projected and its support, specify the projection direction, Create combined curves: select the curves, possibly directions, and specify the combine type.

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What's New

Create reflect lines: select the support and direction, and specify an angle. Create intersections: select the two elements to be intersected.

Creating Points, Lines and Planes
Creating Points
This task shows the various methods for creating points: • • • • • • • by coordinates on a curve on a plane on a surface at a circle/sphere center tangent point on a curve between

Open the Points3D1.CATPart document. 1. Click the Point icon .

The Point Definition dialog box appears. 2. Use the combo to choose the desired point type. Coordinates

• • •

Enter the X, Y, Z coordinates in the current axis-system. Optionally, select a Reference Point. When the command is launched at creation, the initial value in the Axis System field is the current local axis system. If no local axis system is current, the field is set to Default. 25

The corresponding point is displayed.

geometry Whenever you select a local axis system, the point's coordinates are changed with respect to the selected axis system so that the location of the point is not changed. This is not the case with points valuated by formulas: if you select an axis system, the defined formula remains unchanged. This option replaces the Coordinates in absolute axis-system option. If you create a point using the coordinates method and an axis system is already defined and set as current, the point's coordinates are defined according to current the axis system. As a consequence, the point's coordinates are not displayed in the specification tree. The current local axis system must be different from the absolute axis. On curve

• •

Select a curve Optionally, select a reference point.

If this point is not on the curve, it is projected onto the curve. If no point is selected, the curve's extremity is used as reference. • Select an option point to determine whether the new point is to be created: o at a given distance along the curve from the reference point o a given ratio between the reference point and the curve's extremity.

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What's New

•

Enter the distance or ratio value. If a distance is specified, it can be: o a geodesic distance: the distance is measured along the curve o an Euclidean distance: the distance is measured in relation to the reference point (absolute value). The corresponding point is displayed.

It is not possible to create a point with an euclidean distance if the distance or the ratio value is defined outside the curve. You can also: • • click the Nearest extremity button to display the point at the nearest extremity of the curve. click the Middle Point button to display the mid-point of the curve.

Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed) when using the Middle Point option. • use the Reverse Direction button to display: o the point on the other side of the reference point (if a point was selected originally) o the point from the other extremity (if no point was selected originally). • click the Repeat object after OK if you wish to create equidistant points on the curve, using the currently created point as the reference, as described in Creating Multiple Points in the Wireframe and Surface User's Guide.

You will also be able to create planes normal to the curve at these points, by checking the Create normal planes also button, and to create all instances in a new geometrical set by checking the Create in a new geometrical set button. If the button is not checked the instances are created in the current

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geometry geometrical set.

• •

If the curve is infinite and no reference point is explicitly given, by default, the reference point is the projection of the model's origin If the curve is a closed curve, either the system detects a vertex on the curve that can be used as a reference point, or it creates an extremum point, and highlights it (you can then select another one if you wish) or the system prompts you to manually select a reference point.

Extremum points created on a closed curve are aggregated under their parent command and put in no show in the specification tree.

On plane

•

Select a plane. o If you select one of the planes of any local axis system as the plane, the origin of this axis system is set as the reference point and featurized. If you modify the origin of the axis system, the reference point is modified accordingly. Optionally, select a point to define a reference for computing coordinates

•

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What's New in the plane. o If no point is selected, the projection of the model's origin on the plane is taken as reference. Optionally, select a surface on which the point is projected normally to the plane. o If no surface is selected, the behavior is the same.

•

Furthermore, the reference direction (H and V vectors) is computed as follows: With N the normal to the selected plane (reference plane), H results from the vectorial product of Z and N (H = Z^N). If the norm of H is strictly positive then V results from the vectorial product of N and H (V = N^H). Otherwise, V = N^X and H = V^N. Would the plane move, during an update for example, the reference direction would then be projected on the plane. • Click in the plane to display a point.

On surface

• •

Select the surface where the point is to be created. Optionally, select a reference point. By default, the surface's middle point is taken as reference. You can select an element to take its orientation as reference direction or 29

•

geometry a plane to take its normal as reference direction. You can also use the contextual menu to specify the X, Y, Z components of the reference direction. • • Enter a distance along the reference direction to display a point. Choose the dynamic positioning of the point: o Coarse (default behavior): the distance computed between the reference point and the mouse click is an euclidean distance. Therefore the created point may not be located at the location of the mouse click (see picture below). The manipulator (symbolized by a red cross) is continually updated as you move the mouse over the surface.

o

Fine: the distance computed between the reference point and the mouse click is a geodesic distance. Therefore the created point is located precisely at the location of the mouse click. The manipulator is not updated as you move the mouse over the surface, only when you click on the surface.

Sometimes, the geodesic distance computation fails. In this case, an euclidean distance might be used and the created point might not be located at the location of the mouse click. This is the case with closed surfaces or surfaces with holes. We advise you to split these surfaces before creating the point. Circle/Sphere center

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What's New

• •

Select a circle, circular arc, or ellipse, or Select a sphere or a portion of sphere.

A point is displayed at the center of the selected element.

Tangent on curve • Select a planar curve and a direction line.

A point is displayed at each tangent. The Multi-Result Management dialog box is displayed because several points are generated. Refer to the Managing Multi-Result Operations chapter.

Between

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geometry

•

Select any two points.

•

Enter the ratio, that is the percentage of the distance from the first selected point, at which the new point is to be. You can also click Middle Point button to create a point at the exact midpoint (ratio = 0.5).

Be careful that the arrow is orientated towards the inside of the curve (providing the curve is not closed) when using the Middle Point option. • Use the Reverse direction button to measure the ratio from the second selected point.

If the ratio value is greater than 1, the point is located on the virtual line beyond the selected points. 3. Click OK to create the point. The point (identified as Point.xxx) is added to the specification tree. • • Parameters can be edited in the 3D geometry. For more information, refer to the Editing Parameters chapter. You can isolate a point in order to cut the links it has with the geometry used to create it. To do so, use the Isolate contextual menu. For more information, refer to the Isolating Geometric Elements chapter.

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What's New

Creating Multiple Points and Planes
This task shows how to create several points, and planes, at a time: Open the MultiplePoints1.CATPart document. Display the Points toolbar by clicking and holding the arrow from the Point icon. 1. Click the Point & Planes Repetition icon 2. Select a curve or a Point on curve. The Points & Planes Repetition dialog box appears. .

3. Define the number or points to be created (instances field). Here we chose 5 instances. You can choose the side on which the points are to be created in relation to the initially selected point on a curve. Simply use the Reverse Direction button, or clicking on the arrow in the geometry.

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If you check the With end points option, the last and first instances are the curve end points. 4. Click OK to create the point instances, evenly spaced over the curve on the direction indicated by the arrow. The points (identified as Point.xxx as for any other type of point) are added to the specification tree.

•

If you selected a point on a curve, you can select a second point, thus defining the area of the curve where points should be created. Simply click the Second point field in the Multiple Points Creation dialog box, then select the limiting point. If you selected the Point2 created above as the limiting point, while keeping the same values, you would obtain the following:

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What's New

If the selected point on curve already has a Reference point (as described in Creating Points - on curve), this reference point is automatically taken as the second point. By default, the Second point is one of the endpoints of the curve. • When you select a point on a curve, the Instances & spacing option is available from the Parameters field. In this case, points will be created in the given direction and taking into account the Spacing value. For example, three instances spaced by 10mm.

•

Check the Create normal planes also to automatically generate planes at the point instances.

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geometry

•

Check the Create in a new Body if you want all object instances in a separate body. A new Geometrical Set or Ordered Geometrical Set will be created automatically, depending on the type of body the points or planes to be repeated belong to. In case an Ordered Geometrical Set is created, it is considered as private: it means that you cannot perform any modification on its elements (deleting, adding, reordering, etc., is forbidden). If the option is not checked the instances are created, in the current body.

Creating Extremum Elements

This task shows you to create extremum elements (points, edges, or faces), that is elements at the minimum or maximum distance on a curve, a surface, or a pad, according to given directions. Open the Extremum1.CATPart document. Display the Points toolbar by clicking and holding the arrow from the Point icon. 1. Click the Extremum icon . The Extremum Definition dialog box is displayed. 2. Set the correct options: • • Max: according to a given direction the highest point on the curve is created Min: according to the same direction the lowest point on the curve is created

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What's New

Extremum Points on a curve: 3. Select a curve.

4. Select the direction into which the extremum point must be identified.

5. Click OK. The point (identified as Extremum.xxx) is added to the specification tree.

Extremum on a surface:

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geometry

3. Select a surface.

4. Select the direction into which the extremum must be identified. If you click OK, the extremum face is created.

Giving only one direction is not always enough. You need to give a second, and possibly a third direction depending on the expected result (face, edge or point) to indicate to the system in which direction you want to create the extremum element. These directions must not be identical. 3. Select a second direction. If you click OK, the extremum edge is created.

4. Select a third direction.

38

What's New

5. Click OK. The point (identified as Extremum.xxx) is added to the specification tree.

Creating Polar Extremum Elements

This task shows how to create an element of extremum radius or angle, on a planar contour. Open the Extremum2.CATPart document. 1. Click the Polar Extremum icon .

The Polar Extremum Definition dialog box appears.

39

geometry

2. Select the contour, that is a connex planar sketch or curve on which the extremum element is to be created.

Non connex elements, such as the letter A in the sample, are not allowed. 3. Select the supporting surface of the contour.

4. Specify the axis origin and a reference direction, in order to determine the axis system in which the extremum element is to be created. 5. Click Preview:

40

What's New

Depending on the selected computation type, the results can be: • Min radius: the extremum element is detected based on the shortest distance from the axis-system origin

•

Max radius: the extremum element is detected based on the longest distance from the axis-system origin

•

Min angle: the extremum element is detected based on the smallest angle from the selected direction within the axis-system

•

Max angle: the extremum element is detected based on the greatest angle from the selected direction within the axis-system

41

geometry

The radius or angle value is displayed in the Polar Extremum Definition dialog box for information. 6. Click OK to create the extremum point. The element (identified as Polar extremum.xxx), a point in this case, is added to the specification tree.

Creating Lines
This task shows the various methods for creating lines: • • • • • • point to point point and direction angle or normal to curve tangent to curve normal to surface bisecting

It also shows you how to create a line up to an element, define the length type and automatically reselect the second point. Open the Lines1.CATPart document. 1. Click the Line icon .

The Line Definition dialog box is displayed. 2. Use the drop-down list to choose the desired line type. A line type will be proposed automatically in some cases depending on your first element selection.
Defining the line type

Point - Point This type is only available with the Generative Shape Design 2 product.

42

What's New

•

Select two points.

A line is displayed between the two points. Proposed Start and End points of the new line are shown.

•

If needed, select a support surface. In this case a geodesic line is created, i.e. going from one point to the other according to the shortest distance along the surface geometry (blue line in the illustration below). If no surface is selected, the line is created between the two points based on the shortest distance.

If you select two points on closed surface (a cylinder for example), the result may be unstable. Therefore, it is advised to split the surface and only keep the part on which the geodesic line will lie. The geodesic line is not available with the Wireframe and Surface workbench.

43

geometry

•

•

Specify the Start and End points of the new line, that is the line endpoint location in relation to the points initially selected. These Start and End points are necessarily beyond the selected points, meaning the line cannot be shorter than the distance between the initial points. Check the Mirrored extent option to create a line symmetrically in relation to the selected Start and End points.

The projections of the 3D point(s) must already exist on the selected support. Point - Direction

•

Select a reference Point and a Direction line. A vector parallel to the direction line is displayed at the reference point. Proposed Start and End points of the new line are shown.

44

What's New

•

Specify the Start and End points of the new line. The corresponding line is displayed.

The projections of the 3D point(s) must already exist on the selected support. Angle or Normal to curve

45

geometry

•

• •

Select a reference Curve and a Support surface containing that curve. o If the selected curve is planar, then the Support is set to Default (Plane). o If an explicit Support has been defined, a contextual menu is available to clear the selection. Select a Point on the curve. Enter an Angle value.

A line is displayed at the given angle with respect to the tangent to the reference curve at the selected point. These elements are displayed in the plane tangent to the surface at the selected point. You can click on the Normal to Curve button to specify an angle of 90 degrees.

46

What's New Proposed Start and End points of the line are shown. • Specify the Start and End points of the new line. The corresponding line is displayed. • Click the Repeat object after OK if you wish to create more lines with the same definition as the currently created line. In this case, the Object Repetition dialog box is displayed, and you key in the number of instances to be created before pressing OK.

As many lines as indicated in the dialog box are created, each separated from the initial line by a multiple of the angle value.

You can select the Geometry on Support check box if you want to create a geodesic line onto a support surface. The figure below illustrates this case.

47

geometry

Geometry on support option not checked

Geometry on support option checked

This line type enables to edit the line's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry. Tangent to curve

•

Select a reference Curve and a point or another Curve to define the tangency. o if a point is selected (mono-tangent mode): a vector tangent to the curve is displayed at the selected point. o If a second curve is selected (or a point in bi-tangent mode), you

48

What's New need to select a support plane. The line will be tangent to both curves. If the selected curve is a line, then the Support is set to Default (Plane). If an explicit Support has been defined, a contextual menu is available to clear the selection. When several solutions are possible, you can choose one (displayed in red) directly in the geometry, or using the Next Solution button.

Line tangent to curve at a given point •

Line tangent to two curves

Specify Start and End points to define the new line. The corresponding line is displayed.

Normal to surface

49

geometry

•

Select a reference Surface and a Point. A vector normal to the surface is displayed at the reference point. Proposed Start and End points of the new line are shown.

If the point does not lie on the support surface, the minimum distance between the point and the surface is computed, and the vector normal to the surface is displayed at the resulted reference point. • Specify Start and End points to define the new line. The corresponding line is displayed.

50

What's New

Bisecting

• • • • •

Select two lines. Their bisecting line is the line splitting in two equals parts the angle between these two lines. Select a point as the starting point for the line. By default it is the intersection of the bisecting line and the first selected line. Select the support surface onto which the bisecting line is to be projected, if needed. Specify the line's length by defining Start and End values (these values are based onto the default start and end points of the line). The corresponding bisecting line, is displayed. You can choose between two solutions, using the Next Solution button, or directly clicking the numbered arrows in the geometry.

51

geometry

3. Click OK to create the line. The line (identified as Line.xxx) is added to the specification tree. • • • • • • • Regardless of the line type, Start and End values are specified by entering distance values or by using the graphic manipulators. Start and End values should not be the same. Check the Mirrored extent option to create a line symmetrically in relation to the selected Start point. It is only available with the Length Length type. In most cases, you can select a support on which the line is to be created. In this case, the selected point(s) is projected onto this support. You can reverse the direction of the line by either clicking the displayed vector or selecting the Reverse Direction button (not available with the point-point line type). Parameters can be edited in the 3D geometry. For more information, refer to the Editing Parameters chapter. You can isolate a line in order to cut the links it has with the geometry used to create it. To do so, use the Isolate contextual menu. For more information, refer to the Isolating Geometric Elements chapter.

Creating a line up to an element

This capability allows you to create a line up to a point, a curve, or a surface. • It is available with all line types, but the Tangent to curve type. Up to a point • Select a point in the Up-to 1 and/or Up-to 2 fields. Here is an example with the Bisecting line type, the Length Length type, and a point as Up-to 2 element.

52

What's New

Up to a curve • Select a curve in the Up-to 1 and/or Up-to 2 fields. Here is an example with the Point-Point line type, the Infinite End Length type, and a curve as the Up-to 1 element.

Up to a surface • Select a surface in the Up-to 1 and/or Up-to 2 fields. Here is an example with the Point-Direction line type, the Length Length type, and the surface as the Up-to 2 element.

53

geometry

•

• • •

If the selected Up-to element does not intersect with the line being created, then an extrapolation is performed. It is only possible if the element is linear and lies on the same plane as the line being created. However, no extrapolation is performed if the Up-to element is a curve or a surface. The Up-to 1 and Up-to 2 fields are grayed out with the Infinite Length type, the Up-to 1 field is grayed out with the Infinite Start Length type, the Up-to 2 field is grayed out with the Infinite End Length type. The Up-to 1 field is grayed out if the Mirrored extent option is checked. In the case of the Point-Point line type, Start and End values cannot be negative.

Defining the length type

•

Select the Length Type: o Length: the line will be defined according to the Start and End points values o Infinite: the line will be infinite o Infinite Start Point: the line will be infinite from the Start point o Infinite End Point: the line will be infinite from the End point

Reselecting automatically a second point

By default, the Length type is selected. The Start and/or the End points values will be grayed out when one of the Infinite options is chosen.

This capability is only available with the Point-Point line method. 1. Double-click the Line icon 2. Create the first point. The Reselect Second Point at next start option appears in the Line dialog box. 3. Check it to be able to later reuse the second point. 4. Create the second point. 5. Click OK to create the first line. .

The Line dialog box is displayed.

54

What's New

The Line dialog box opens again with the first point initialized with the second point of the first line. 6. Click OK to create the second line.

To stop the repeat action, simply uncheck the option or click Cancel in the Line Definition dialog box.

Creating an Axis
This task shows you how to create an axis feature. Open the Axis1.CATPart document. 1. Click the Axis icon .

The Axis Definition dialog box appears. 2. Select an Element where to create the axis.

55

geometry This element can be: • • • • a circle or a portion of circle an ellipse or a portion of ellipse an oblong curve a revolution surface or a portion of revolution surface

Circle • Select the direction (here we chose the yz plane), when not normal to the surface. • Select the axis type: o Aligned with reference direction o Normal to reference direction o Normal to circle

Aligned with reference direction Ellipse • Select o o o

Normal to reference direction

Normal to circle

the axis type: Major axis Minor axis Normal to ellipse

56

What's New

Major axis Oblong Curve • Select the axis type: o Major axis o Minor axis o Normal to oblong

Minor axis

Normal to ellipse

Major axis Revolution Surface

Minor axis

Normal to oblong

57

geometry

The revolution surface's axis is used, therefore the axis type combo list is disabled.

The axis can be displayed in the 3D geometry, either infinite or limited to the geometry block of the input element. This option is to be parameterized in Tools -> Options -> Shape -> Generative Shape Design -> General. To have further information, please refer to the General Settings chapter in the Customizing section. 3. Click OK to create the axis. The element (identified as Axis.xxx) is added to the specification tree.

Creating Planes
This task shows the various methods for creating planes: • • • • • • offset from a plane parallel through point angle/normal to a plane through three points through two lines through a point and a line • • • • • • through a planar curve normal to a curve tangent to a surface from its equation equation mean through points

Open the Planes1.CATPart document. 1. Click the Plane icon .

The Plane Definition dialog box appears.

58

What's New 2. Use the combo to choose the desired Plane type. Once you have defined the plane, it is represented by a red square symbol, which you can move using the graphic manipulator. Offset from plane

• Select a reference Plane then enter an Offset value. A plane is displayed offset from the reference plane.

Use the Reverse Direction button to reverse the change the offset direction, or simply click on the arrow in the geometry.

•

Click the Repeat object after OK if you wish to create more offset planes. In this case, the Object Repetition dialog box is displayed, and you key in the number of instances to be created before pressing OK.

As many planes as indicated in the dialog box are created (including the one you were currently creating), each separated from the initial plane by a multiple of the Offset value.

59

geometry

Parallel through point

• Select a reference Plane and a Point.

A plane is displayed parallel to the reference plane and passing through the selected point.

Angle or normal to plane

60

What's New

• Select a reference Plane and a Rotation axis. This axis can be any line or an implicit element, such as a cylinder axis for example. To select the latter press and hold the Shift key while moving the pointer over the element, then click it. • Enter an Angle value.

The plane is displayed such as its center corresponds to the projection of the center of the reference plane on the rotation axis. It is oriented at the specified angle to the reference plane.

•

Check the Project rotation axis on reference plane option if you wish to project the rotation axis onto the reference plane. If the reference plane is not parallel to the rotation axis, the created plane is rotated around the axis to have the appropriate angle with regard to reference plane. Check the Repeat object after OK option if you wish to create more planes at an angle from the initial plane. In this case, the Object Repetition dialog box is displayed, and you key in the number of instances to be created before pressing OK.

•

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geometry

As many planes as indicated in the dialog box are created (including the one you were currently creating), each separated from the initial plane by a multiple of the Angle value. Here we created five planes at an angle of 20 degrees.

This plane type enables to edit the plane's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry. Through three points

• Select three points.

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What's New

The plane passing through the three points is displayed. You can move it simply by dragging it to the desired location.

Through two lines • Select two lines.

The plane passing through the two line directions is displayed. When these two lines are not coplanar, the vector of the second line is moved to the first line location to define the plane's second direction.

Check the Forbid non coplanar lines button to specify that both lines be in the same plane.

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geometry

Through point and line

• Select a Point and a Line.

The plane passing through the point and the line is displayed.

Through planar curve

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What's New

• Select a planar Curve.

The plane containing the curve is displayed.

Normal to curve

• Select a reference Curve. • You can select a Point. By default, the curve's middle point is selected. It can be selected outside the curve.

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geometry

A plane is displayed normal to the curve with its origin at the specified point. The normal is computed at the point on the curve that is the nearest to the selected point.

Tangent to surface

• Select a reference Surface and a Point.

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What's New

A plane is displayed tangent to the surface at the specified point.

Equation

67

geometry

• Enter the A, B, C, D components of the Ax + By + Cz = D plane equation. • Select a point to position the plane through this point, you are able to modify A, B, and C components, the D component becomes grayed. • When the command is launched at creation, the initial value in the Axis System field is the current local axis system. If no local axis system is current, the field is set to Default. Whenever you select a local axis system, A, B, C, and D values are changed with respect to the selected axis system so that the location of the plane is not changed. This is not the case with values valuated by formulas: if you select an axis system, the defined formula remains unchanged. This option replaces the Coordinates in absolute axis-system option. Use the Normal to compass button to position the plane perpendicular to the compass direction.

Use the Parallel to screen button to parallel to the screen current view.

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What's New

Mean through points

• Select three or more points to display the mean plane through these points.

It is possible to edit the plane by first selecting a point in the dialog box list then choosing an option to either: • Remove the selected point • Replace the selected point by another point.

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geometry

3. Click OK to create the plane. The plane (identified as Plane.xxx) is added to the specification tree. • • Parameters can be edited in the 3D geometry. For more information, refer to the Editing Parameters chapter. You can isolate a plane in order to cut the links it has with the geometry used to create it. To do so, use the Isolate contextual menu. For more information, refer to the Isolating Geometric Elements chapter.

Creating Planes Between Other Planes
This task shows how to create any number of planes between two existing planes, in only one operation. Open the Planes1.CATPart document. 1. Click the Planes Repetition icon The Planes Between dialog box appears. .

2. Select the two planes between which the new planes must be created.

3. Specify the number of planes to be created between the two selected planes. 4. Click OK to create the planes. The planes (identified as Plane.xxx) are added to the specification tree.

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What's New

You can check the Create in a new Body button to create a new geometrical set containing only the repeated planes.

Creating Polylines, Splines, and Curves
Creating Polylines
This task shows you how to create a polyline, that is a broken line made of several connected segments. These linear segments may be connected by a blending radii. Polylines may be useful to create cylindrical shapes such as pipes, for example. Open the Spline1.CATPart document. 1. Click the Polyline icon.

The Polyline Definition dialog box appears.

2. Select several points in a row. Here we selected Point.1, Point.5, Point.3 and Point.2 in this order. The resulting polyline would look like this:

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geometry

3. From the dialog box, select Point.5, click the Add After button and select Point.6. 4. Select Point.3 and click the Remove button. The resulting polyline now looks like this:

5. Still from the dialog box select Point.5, click the Replace button, and select Point.4 in the geometry. The added point automatically becomes the current point in the dialog box. 6. Click OK in the dialog box to create the polyline. The element (identified as Polyline.xxx) is added to the specification tree.

7. Double-click the polyline from the specification tree. The Polyline Definition dialog box is displayed again. 8. Select Point.6 within the dialog box, enter a value in the Radius field, and click Preview.

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What's New

A curve, centered on Point.6, and which radius is the entered value (R=30 here) is created.

The Radius option is only available with the Generative Shape Design 2 product. • • • You can define a radius for each point, except end points. You can also define radii at creation time. The blending curve's center is located on the side of the smallest angle between the two connected line segments.

9. Click OK to accept the new definition of the polyline. • • • The polyline's orientation depends on the selection order of the points. You can re-order selected points using the Replace, Remove, Add, Add After, and Add Before buttons. You cannot select twice the same point to create a polyline. However, you can check the Close polyline button to generate a closed contour.

Creating Splines
This task shows the various methods for creating spline curves. Open the Spline1.CATPart document. 1. Click the Spline icon .

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geometry

The Spline Definition dialog box appears. 2. Select two or more points where the spline is to be created. An updated spline is visualized each time a point is selected.

3. It is possible to edit the spline by first selecting a point in the dialog box list then choosing a button to either: • • • • Add a point after the selected point Add a point before the selected point Remove the selected point Replace the selected point by another point

4. You can select the Geometry on support check box, and select a support (plane, surface), if you want the spline to be projected onto a support surface. It is better when the tangent directions belong to the support, that is when a projection is possible. In this case just select a surface or plane.

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What's New

In the figure above, the spline was created on a planar support grid. 5. Click on the Show parameters button to display further options. 6. To set tangency conditions onto any point of the spline, select the point and click on Tangent Dir.

There are two ways of imposing tangency and curvature constraints: 1. Explicit: select a line or plane to which the tangent on the spline is parallel at the selected point.

2. From curve: select a curve to which the spline is tangent at the selected point.

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geometry

Use the Remove Tgt., Reverse Tgt., or Remove Cur. to manage the different imposed tangency and curvature constraints.

Spline with a tangency constraint on endpoint (tension = 2)

Spline with reversed tangent

7. To specify a curvature constraint at any point of the spline, once a tangency constraint has been set, indicate a curvature direction and enter a radius value: The curvature direction is projected onto a plane normal to the tangent direction. If you use the Create line contextual menu, and want to select the same point as a point already used to define the tangent direction, you may have to select it from the specification tree, or use the pre-selection navigator.

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What's New

Spline with tangency constraint

Spline with tangency constraint and curvature constraint (radius = 50mm)

Spline with tangency constraint and curvature constraint (radius = 2mm) Note that there are prerequisites for the Points Specifications and you must enter your information in the following order: • • • • Tangent Dir. (tangent direction) Tangent Tension Curvature Dir. (curvature direction) Curvature Radius (to select it, just click in the field)

The fields become active as you select values. 8. Click OK to create the spline. The spline (identified as Spline.xxx) is added to the specification tree. To add a parameter to a point, select a line in the Points list. This list is highlighted. You have two possibilities: 1. extended parameters 2. select any line or plane for the direction. • Use the Close Spline option to create a closed curve, provided the

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geometry geometric configuration allows it.

Spline with Close Spline option unchecked

Spline with Close Spline option checked

Creating Circles
This task shows the various methods for creating circles and circular arcs: • • • • • • • • • center and radius center and point two points and radius three points center and axis bitangent and radius bitangent and point tritangent center and tangent

Open the Circles1.CATPart document. Please note that you need to put the desired geometrical set in show to be able to perform the corresponding scenario. 1. Click the Circle icon .

The Circle Definition dialog box appears. 2. Use the drop-down list to choose the desired circle type. Center and radius

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What's New

• • •

Select a point as circle Center. Select the Support plane or surface where the circle is to be created. Enter a Radius value.

Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. For a circular arc, you can specify the Start and End angles of the arc.

If a support surface is selected, the circle lies on the plane tangent to the surface at the selected point. • Start and End angles can be specified by entering values or by using the graphic manipulators. Center and point

•

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geometry

• • •

Select a point as Circle center. Select a Point where the circle is to be created. Select the Support plane or surface where the circle is to be created.

The circle, which center is the first selected point and passing through the second point or the projection of this second point on the plane tangent to the surface at the first point, is previewed. Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. For a circular arc, you can specify the Start and End angles of the arc.

Two points and radius

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What's New

• •

Select two points on a surface or in the same plane. Select the Support plane or surface.

You can now select a direction as the support. The support is calculated using this direction and the two input points. The plane passing through the two points and whose normal is closest to the given direction is computed as follows: • Let s take V1 as the vector P1P2, where P1 and P2 are the input points. • Let s take V2 as the user direction (which can be the compass direction). • Compute V3 = V1 X V2 (cross product). • Compute V4 = V3 X V1 (cross product). • The support plane is normal to V4 and passing through P1 and P2. • Note that if V2 is orthogonal to V1, V4 = V2 and the support plane is normal to V2 (user direction). • Enter a Radius value.

The circle, passing through the first selected point and the second point or the projection of this second point on the plane tangent to the surface at the first point, is previewed. Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. For a circular arc, you can specify the trimmed or complementary arc using the two selected points as end points. You can use the Second Solution button, to display the alternative arc.

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geometry

With a plane as Support Three points

With a direction as Support (the computed plane is shown in blue)

•

Select three points where the circle is to be created.

Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. For a circular arc, you can specify the trimmed or complementary arc using the two of the selected points as end points.

Center and axis

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What's New

• • • •

Select the axis/line. It can be any linear curve. Select a point. Enter a Radius value. Set the Project point on axis/line option: o checked (with projection): the circle is centered on the reference point and projected onto the input axis/line and lies in the plane normal to the axis/line passing through the reference point. The line will be extended to get the projection if required. o unchecked (without projection): the circle is centered on the reference point and lies in the plane normal to the axis/line passing though the reference point.

With projection Bi-tangent and radius

Without projection

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geometry

• •

Select two Elements (point or curve) to which the circle is to be tangent. Select a Support surface.

If one of the selected inputs is a planar curve, then the Support is set to Default (Plane). If an explicit Support needs to be defined, a contextual menu is available to clear the selection in order to select the desired support. This automatic support definition saves you from performing useless selections. • • Enter a Radius value. Several solutions may be possible, so click in the region where you want the circle to be.

Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. For a circular arc, you can specify the trimmed or complementary arc using the two tangent points as end points.

You can select the Trim Element 1 and Trim Element 2 check boxes to trim the first element or the second element, or both elements. Here is an example with Element 1 trimmed.

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What's New

These options are only available with the Trimmed Circle limitation. Bi-tangent and point

• • •

Select a point or a curve to which the circle is to be tangent. Select a Curve and a Point on this curve. Select a Support plane or planar surface.

The point will be projected onto the curve. If one of the selected inputs is a planar curve, then the Support is set to Default (Plane). If an explicit Support needs to be defined, a contextual menu is available to clear the selection in order to select the desired support. This automatic support definition saves you from performing useless selections. • Several solutions may be possible, so click in the region where you want the circle to be.

Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed.

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geometry

Complete circle For a circular arc, you can choose the trimmed or complementary arc using the two tangent points as end points.

Trimmed circle

Complementary trimmed circle

You can select the Trim Element 1 and Trim Element 2 check boxes to trim the first element or the second element, or both elements. Here is an example with both elements trimmed.

These options are only available with the Trimmed Circle limitation. Tritangent

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What's New

• •

Select three Elements to which the circle is to be tangent. Select a Support planar surface.

If one of the selected inputs is a planar curve, then the Support is set to Default (Plane). If an explicit Support needs to be defined, a contextual menu is available to clear the selection in order to select the desired support. This automatic support definition saves you from performing useless selections. • Several solutions may be possible, so select the arc of circle that you wish to create.

Depending on the active Circle Limitations icon, the corresponding circle or circular arc is displayed. The first and third elements define where the relimitation ends. For a circular arc, you can specify the trimmed or complementary arc using the two tangent points as end points.

You can select the Trim Element 1 and Trim Element 3 check boxes to trim the first element or the third element, or both elements. Here is an example with Element 3 trimmed.

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geometry

These options are only available with the Trimmed Circle limitation. You cannot create a tritangent circle if an input point lies on an input wire. We advise you to use the bi-tangent and point circle type. Center and tangent

There 1. • • •

are two ways to create a center and tangent circle: Center curve and radius Select a curve as the Center Element. Select a Tangent Curve. Enter a Radius value.

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What's New 2. Line tangent to curve definition • • Select a point as the Center Element. Select a Tangent Curve.

•

If one of the selected inputs is a planar curve, then the Support is set to Default (Plane). If an explicit Support needs to be defined, a contextual menu is available to clear the selection in order to select the desired support. This automatic support definition saves you from performing useless selections.

• •

The circle center will be located either on the center curve or point and will be tangent to tangent curve. Note that only full circles can be created.

4. Click OK to create the circle or circular arc. The circle (identified as Circle.xxx) is added to the specification tree. • You can click the Diameter button to switch to a Diameter value. Conversely, click the Radius button to switch back to the Radius value. This option is available with the Center and radius, Two point and radius, Bitangent and radius, Center and tangent, and Center and axis circle types.

Note that the value does not change when switching from Radius to Diameter and vice-versa. • You can select the Axis computation check box to automatically create axes while creating or modifying a circle. Once the option is checked, the Axis direction field is enabled. o o If you do not select a direction, an axis normal to the circle will be created. If you select a direction, two more axes features will be created: an axis aligned with the reference direction and an axis normal to the reference direction.

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geometry

In the specification tree, the axes are aggregated under the Circle feature. You can edit their directions but cannot modify them. If the datum mode is active, the axes are not aggregated under the Circle features, but one ore three datum lines are created.

Axis normal to the circle

Axis aligned with the reference direction (yz plane)

Axis normal to the reference direction (yz plane) • • If you select the Geometry on Support option and the selected support is not planar, then the Axis Computation is not possible. You can select the Geometry on Support check box if you want the circle to be projected onto a support surface. In this case just select a support surface. This option is available with the Center and radius, Center and point, Two point and radius, and Three points circle types. When several solutions are possible, click the Next Solution button to move to another arc of circle, or directly select the arc you want in the 3D geometry. A circle may have several points as center if the selected element is made of various circle arcs with different centers.

•

•

•

Parameters can be edited in the 3D geometry. For more information, refer to the

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What's New Editing Parameters chapter. You can isolate a plane in order to cut the links it has with the geometry used to create it. To do so, use the Isolate contextual menu. For more information, refer to the Isolating Features chapter.

•

Creating Conic Curves
This task shows the various methods for creating conics, that is curves defined by five constraints: start and end points, passing points or tangents. The resulting curves are arcs of either parabolas, hyperbolas or ellipses. The different elements necessary to define these curves are either: • • • • • • two points, start and end tangents, and a parameter two points, start and end tangents, and a passing point two points, a tangent intersection point, and a parameter two points, a tangent intersection point, and a passing point four points and a tangent five points.

Open the Conic1.CATPart document. 1. Click the Conic icon .

The Conic Definition dialog box opens.

2. Fill in the conic curve parameters, depending on the type of curve to be created by selecting geometric elements (points, lines, etc.): • Support: the plane on which the resulting curve will lie Constraint Limits:

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geometry • • • Start and End points: the curve is defined from the starting point to the end point Tangents Start and End: if necessary, the tangent at the starting or end point defined by selecting a line Tangent Intersection Point: a point used to define directly both tangents from the start and end point. These tangents are on the virtual lines passing through the start (end) point and the selected point.

a. Selecting the support plane and starting point

b. Selecting the ending point

c. Selecting the tangent at the starting point

d. Selecting the tangent at the ending point

Resulting conic curve If you check the Tgt Intersection Point option, and select a point, the tangents are created as passing through that point:

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Using a tangent intersection point

Resulting conic curve

Intermediate Constraints • Point 1, 2, 3: possible passing points for the curve. These points have to be selected in logical order, that is the curve will pass through the start point, then through Point 1, Point 2, Point 3 and the end point. Depending on the type of curve, not all three points have to be selected. You can define tangents on Point 1 and Point 2 (Tangent 1 or 2). • Parameter: ratio ranging from 0 to 1 (excluded), this value is used to define a passing point (M in the figure below) and corresponds to the OM distance/OT distance. If parameter = 0.5, the resulting curve is a parabola If 0 < parameter < 0.5, the resulting curve is an arc of ellipse, If 1 > parameter > 0.5, the resulting curve is a hyperbola.

3. Click OK to create the conic curve. The conic curve (identified as Conic.xxx) is added to the specification tree.

Creating Spirals
This task shows how to create curves in the shape of spirals, that is a in 2D plane, as opposed to the helical curves.

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geometry

Open the Spiral1.CATPart document. 1. Click the Spiral icon .

The Spiral Curve Definition dialog box appears.

2. Select a supporting plane and the Center point for the spiral.

3. Specify a Reference direction along which the Start radius value is measured and from which the angle is computed, when the spiral is defined by an angle. The spiral is previewed with the current options:

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4. Specify the Start radius value, that is the distance from the Center point, along the Reference direction, at which the spiral's first revolution starts. 5. Define the spiral's Orientation, that is the rotation direction: clockwise or counter clockwise 6. Specify the spiral creation mode, and fill in the corresponding values: • Angle & Radius: the spiral is defined by a given End angle from the Reference direction and the radius value, the radius being comprised between the Start and End radius, on the first and last revolutions respectively (i.e. the last revolution ends on a point which distance from the center point is the End radius value).

Ref. direction = Z, Start radius = 5mm, Angle = 45 End radius = 20mm, Revolutions = 5 •

,

Angle & Pitch: the spiral is defined by a given End angle from the Reference direction and the pitch, that is the distance between two revolutions of the spiral.

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geometry

Ref. direction = Z, Start radius = 5mm, Angle = 45 , Pitch = 4mm, Revolutions = 5 • Radius & Pitch: the spiral is defined by the End radius value and the pitch. The spiral ends when the distance from the center point to the spiral's last point equals the End radius value.

Ref. direction = Z, Start radius = 5mm, End radius = 20mm, Pitch = 4mm Depending on the selected creation mode, the End angle, End radius, Pitch, and Revolutions fields are available or not. 7. Click OK to create the spiral curve. The curve (identified as Spiral.xxx) is added to the specification tree.

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What's New

Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

Creating a Helix
This task shows the various methods for creating helical curves, such as coils and springs for example. These curves are 3D curves, as opposed to the spirals. Open the Helix1.CATPart document. 1. Click the Helix icon .

The Helix Curve Definition dialog box appears.

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geometry

2. Select a starting point and an axis.

3. Select a starting point and an axis.

3. Set the helix parameters: • Pitch: the distance between two revolutions of the curve

You can define the evolution of the pitch along the helix using a law. Defining Laws 1. Click the Law button to display the Law Definition dialog box.

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2. Choose type of law to be applied to the pitch: It can stay Constant, or evolve according to a S type law. For the S type pitch, you need to define a second pitch value. The pitch distance will vary between these two pitch values, over the specified number of revolutions. 3. The Law Viewer allows you to: - visualize the law evolution and the maximum and minimum values, - navigate into the viewer by panning and zooming (using to the mouse), - trace the law coordinates by using the manipulator, - change the viewer size by changing the panel size - reframe on by using the viewer contextual menu - change the law evaluation step by using the viewer contextual menu (from 0.1 (10 evaluations) to 0.001 (1000 evaluations)). 4. Click OK to return to the Helix Curve Definition dialog box. • • • Height: the global height of the helical curve, in the case of a constant pitch type helix Orientation: defines the rotation direction (clockwise or counter clockwise) Starting Angle: defines where the helical curve starts, in relation to the

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geometry starting point. This parameter can be set only for the Constant pitch only. Taper Angle: the radius variation from one revolution to the other. It ranges from -90 to 90 excluded. For a constant radius, set the taper angle to 0. Way: defines the taper angle orientation. Inward: the radius decreases Outward: the radius increases. Profile: the curve used to control the helical curve radius variation. The radius evolves according to the distance between the axis and the selected profile (here the orange curve). Note that the Starting point must be on the profile.

•

•

•

4. Click the Reverse Direction button to invert the curve direction. 5. Click OK to create the helix. The helical curve (identified as Helix.xxx) is added to the specification tree.

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What's New

Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

Creating New Elements from Existing Elements
Creating Corners
This task shows you how to create a corner between two curves or between a point and a curve. Open the Corner1.CATPart document. 1. Click the Corner icon .

The Corner Definition dialog box appears. The Corner On Vertex check box enables you to create a corner by selecting a point or a curve as Element 1 (Element 2 is grayed as well as the Trim Element 1 and 2 options). It is checked by default. 2. Choose the Corner Type: Corner on Support: the support can be a surface or a plane

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1. Select a curve or a point as first referen ce elemen t. 2. Select a curve as second referen ce elemen t. The corner will be created betwee n these two referen ces. 3. Select the Suppor t surface. Here we selecte d the zx plane.

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What's New

The result ing corne r is a curve seen as an arc of circle lying on a suppo rt place or surfa ce. The reference elements must lie on this support, as well as the center of the circle defining the corner. • You can edit the corner's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry.

Creating Connect Curves
This task shows how to create a connecting curve between two curves. Open the ConnectCurve1.CATPart document. 1. Click the Connect Curve icon . The Connect Curve Definition dialog box appears. 2. Select the Connect type. Normal

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geometry

1. Select a first Point on a curve then a second Point on a second curve. The Curve fields are automatically filled. Base Curve This option is only available with the Generative Shape Design 2 product.

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1. Select a base curve as the curve reference. The orientation of the connect curve will be the orientation of the base curve. 2. Select a first Point on a curve then a second Point on a second curve. • The support Curve is optional (it is set as Default) • The first point can be either on the base curve or on the support curve. • The Base Curve option is useful when creating several profiles or guides that have the same shape.

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geometry

Normal curve

Base Curve

3. Use the combos to specify the desired Continuity type: Point, Tangency or Curvature. 4. If needed, enter tension values. A graphic manipulator also allows you to modify the tension at the extremity of the connect curve, rather than in the dialog box. If the Base Curve type is selected, the Continuity and Tension options for the first and the second curve are grayed out and set to Tangency and 1 respectively. The connect curve is displayed between the two selected points according to the specified continuity and tension values.

Normal curve with point continuity at both points Both tensions = 1

Normal curve with point continuity at first point and tangent continuity at the second point Both tensions = 1

Normal curve with tangent continuity at first point and curvature continuity at the second point Both tensions = 1

Normal curve with tangent continuity at first point and curvature continuity at the second point First tension = 10 and second tension = 1

5. A red arrow is displayed at each extremity of the curve. You can click the

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What's New arrow to reverse the orientation of the curve at that extremity or click the Reverse Direction button. If the Base Curve type is selected, the Reverse Direction options are grayed out. 6. You can check the Trim elements option if you want to trim and assemble the two initial curves to the connect curve. If the Base Curve type is selected, you must select a support curve to access the Trim elements option. Otherwise, it is grayed out. 7. Click OK to create the connect curve. The curve (identified as Connect.xxx) is added to the specification tree.

Normal curve with tangent continuity at both points Both tensions = 1

Base Curve Trim elements option checked

Creating Projections
This task shows you how to create geometry by projecting one or more elements onto a support. The projection may be normal or along a direction. You can project: • • • a point onto a surface or wireframe support wireframe geometry onto a surface support any combination of points and wireframe onto a surface support.

Generally speaking, the projection operation has a derivative effect, meaning that there may be a continuity loss when projecting an element onto another. If the initial element presents a curvature continuity, the resulting projected element presents at least a tangency continuity. If the initial element presents a tangency continuity, the resulting projected element presents at least a point continuity. Open the Projection1.CATPart document. 1. Click the Projection icon .

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geometry

The Projection Definition dialog box appears as well as the Multi-Selection dialog box allowing to perform multi-selection.

2. Select the element to be Projected. You can select several elements to be projected. In this case, the Projected field indicates: x elements

3. Select the Support element. 4. Use the combo to specify the direction type for the projection: • Normal: the projection is done normal to the support element.

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What's New

•

Along a direction: you need to select a line to take its orientation as the translation direction or a plane to take its normal as the translation direction.

You can also specify the direction by means of X, Y, Z vector components by using the contextual menu on the Direction field.

•

Whenever several projections are possible, you can select the Nearest Solution check box to keep the nearest projection. The nearest solutions are sorted once the computation of all the possible solutions is performed.

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geometry • You can smooth the element to be projected by checking either:

o

None: deactivates the smoothing result

With support surface: the smoothing is performed according to the support. As a consequence, the resulting smoothed curve inherits support discontinuities. o o Tangency: enhances the current continuity to tangent continuity Curvature: enhances the current continuity to curvature continuity

You can specify the maximum deviation for G1 or G2 smoothing by entering a value or using the spinners. If the element cannot be smoothed correctly, a warning message is issued. Moreover, a topology simplification is automatically performed for G2 vertices: cells with a curvature continuity are merged. Without support surface: o 3D Smoothing: the smoothing is performed without specifying any support surface. As a consequence, the resulting smoothed curve has a better continuity quality and is not exactly laid down on the surface. As a consequence, you may need to activate the Tolerant laydown option. Refer to the Customizing General Settings chapter. This option is available if you previously select the Tangency or Curvature smoothing type.

With 3D smoothing option checked

With 3D smoothing option unchecked

Only small discontinuities are smoothed in order to keep the curve's sharp vertices. 5. Click OK to create the projection element. The projection (identified as Project.xxx) is added to the specification tree. The following capabilities are available: Stacking Commands and Selecting Using MultiOutput.

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Creating Combined Curves
This task shows you how to create combined curves, that is a curve resulting from the intersection of the extrusion of two curves. Open the Combine1.CATPart document. Display the Project-Combine toolbar by clicking and holding the arrow from the Projection icon. 1. Click the Combine icon .

The Combine Definition dialog box appears. 2. Choose the combine type: normal or along directions. • Normal: the virtual extrusion are computed as normal to the curve planes • Along directions: specify the extrusion direction for each curve (Direction1 and Direction2 respectively). Normal Type 3. Successively select the two curves to be combined.

Using the Normal type, the combine curve is the intersection curve between the extrusion of the selected curves in virtual perpendicular planes. This illustration represent the virtual extrusions, allowing the creation of the intersection curve that results in the combine curve.

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4. Click OK to create the element. The curve (identified as Combine.xxx) is added to the specification tree.

Along Directions Type 3. Successively select the two curves to be combined and a direction for each curve.

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What's New

Using the Along directions type, the combine curve is the intersection curve between the extrusion of the selected curves along the selected directions, as illustrated here:

4. Click OK to create the element. The curve (identified as Combine.xxx) is added to the specification tree.

The Nearest solution option, allows to automatically create the curve closest to the first selected curve, in case there are several possible combined curves.

Creating Reflect Lines
This task shows you how to create reflect lines, whether closed or open. Reflect lines are curves for which the normal to the surface in each point present the

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geometry same angle with a specified direction. Open the ReflectLine1.CATPart document. Display the Project-Combine toolbar by clicking and holding the arrow from the Projection icon. 1. Click the Reflect Lines icon .

The Reflect Line Definition dialog box appears.

2. Successively select the support surface and a direction. 3. Key in an angle, representing the value between the selected direction and the normal to the surface. Here we keyed in 15 .

You can also use the displayed manipulators to modify the angle value (ANG manipulator) or to reverse its direction (Support arrow). The Normal option lets you choose whether the angle should be computed: • between the normal to the support and the direction (option checked)

•

between the plane tangent to the support and the direction (option unchecked)

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4. Click OK to create the element. The Reflect Line (identified as ReflectLine.xxx) is added to the specification tree.

•

Use the Repeat object after OK checkbox to create several reflect lines, each separated from the initial line by a multiple of the Angle value. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK. When several reflect lines are created, as for example on a cylinder as illustrated here, you are prompted to choose to either keep both elements within the Reflect Line object, or to choose one as the reference, as described in Creating the Nearest Entity of a Multiple Element.

•

Do not use a null angle value on a closed surface issued from a circle for example. Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

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geometry

Creating Intersections
This task shows you how to create wireframe geometry by intersecting elements. You can intersect: • wireframe elements • surfaces • wireframe elements and a surface. Open the Intersection1.CATPart document. 1. Click the Intersection icon .

The Intersection Definition dialog box appears as well as the Multi-Selection dialog box allow perform multi-selection.

2. Select the two elements to be intersected. The intersection is displayed.

Multi-selection is available on the first and second selection, meaning you can select several eleme intersected as well as several intersecting elements. 3. Choose the type of intersection to be displayed. • A Curve (when intersecting two curves)

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What's New

•

Points (when intersecting two curves)

•

A Contour: when intersecting a solid element with a surface

•

A Face: when intersecting a solid element with a surface (we increased the transparency de pad and surface)

4. Click OK to create the intersection element.

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geometry

This element (identified as Intersect.xxx) is added to the specification tree.

The above example shows the line resulting from the intersection of a plane and a surface

The above example shows the curve resultin from the intersection of two surfaces

Several options can be defined to improve the preciseness of the intersection. Open the Intersection2.CATPart document. •

The Extend linear supports for intersection option enables you to extend the first, second or elements.

Both options are unchecked by default. Here is an example with the option checked for both elements.

•

The Extrapolate intersection on first element check box enables you to perform an extrapola first selected element, in the case of a surface-surface intersection. In all the other cases, th will be grayed.

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What's New

Intersection without the Extrapolation option checked Intersection with the Extrapolation option ch • The Intersect non coplanar line segments check box enables you to perform an intersection non-intersecting lines. In all the other cases, the option will be grayed. When checking this option, both Extend linear supports for intersection options are checked too.

Intersection between the light green line and the blue line: the intersection point is calculated after the blue line is extrapolated Avoid using input elements which are tangent to each the tangency zone.

Intersection between the pink line and the b the intersection is calculated as the mid-poin minimum distance between the two lines other since this may result in geometric insta

The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.

Creating Parallel Curves
This task shows you how to create a curve that is parallel to a reference curve. Open the ParallelCurves1.CATPart document.

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geometry

1. Click the Parallel Curve icon The Parallel Curve Definition dialog box appears.

.

2. Select the reference Curve to be offset. 3. Select the Support plane or surface on which the reference curve lies. 4. Specify the offset of the parallel curve either by:

a. entering a value or using the graphic manipulator in the Constant field.

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b. selecting a point in the Point field (in both Geodesic and Euclidean mode) In that case, the Constant field is grayed.

5. Choose the parallelism mode to create the parallel curve: • Euclidean: the distance between both curves will be the shortest possible one, regardless of the support.

If you select this mode, you can choose to offset the curve at a constant distance from the initial element, or according to a law. In this case, you need to select a law as defined in Creating Laws. Defining Laws The law can be negative, providing the curves are curvature continuous. Please note that: - it is advised to use curvature continuous laws, - it is advised not to use laws with a vertical tangency, - it is possible to create a parallel curve with a law that reverses (which means becoming either positive or negative) only on a curve that is tangency continuous. This option is only available with the Generative Shape Design 2 product. 1. Click the Law... button to display the Law Definition dialog box. The 2D viewer enables you to previsualize the law evolution before applying it. 2. Enter Start and End values. 3. Choose the law type to be applied to the pitch. Four law types are available: a. Constant: a regular law, only one value is needed. b. Linear: a linear progression law between the Start and End indicated values c. S type: an S-shaped law between the two indicated values d. Advanced: allowing to select a Law element as defined in Creating Laws.

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For the S type pitch, you need to define a second pitch value. The pitch distance will vary between these two pitch values, over the specified number of revolutions. 4. The Law Viewer allows you to: - visualize the law evolution and the maximum and minimum values, - navigate into the viewer by panning and zooming (using to the mouse), - trace the law coordinates by using the manipulator, - change the viewer size by changing the panel size - reframe on by using the viewer contextual menu - change the law evaluation step by using the viewer contextual menu (from 0.1 (10 evaluations) to 0.001 (1000 evaluations)). 5. Check the Inverse law button to reverse the law as defined using the above options. 6. Click OK to return to the Parallel Curve Definition dialog box.

•

Geodesic: the distance between both curves will be the shortest possible one, taking the support curvature into account. In this case, the offset always is constant in every points of the curves and you do not need to select a corner type.

This option is only available with the Generative Shape Design 2 product. 6. Select corner type (useful for curves presenting sharp angles): • Sharp: the parallel curve takes into account the angle in the initial curve • Round: the parallel curve is rounded off as in a corner In this case, the offset always is constant in every points of the curves and you do not need to select a corner type.

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The parallel curve is displayed on the support surface and normal to the reference curve. 7. Click OK to create the parallel curve.

Parallel curve defined by an constant offset value • You can smooth the curve by checking either: o None: deactivates the smoothing result o G1 : enhances the current continuity to tangent continuity o G2 : enhances the current continuity to curvature continuity

Parallel curve defined by a passing point

The curve (identified as Parallel.xxx) is added to the specification tree.

You can specify the maximum deviation for G1 or G2 smoothing by entering a value or using the spinners. If the curve cannot be smoothed correctly, a warning message is issued. Moreover, a topology simplification is automatically performed for G2 vertices: cells 123

geometry with a curvature continuity are merged. Please refer to the Customizing General Settings chapter. The Smoothing option is only available with the Generative Shape Design 2 product. • • • You can use the Reverse Direction button to display the parallel curve on the other side of the reference curve or click the arrow directly on the geometry. When the selected curve is a planar curve, its plane is selected by default. However, you can explicitly select any support. when you modify an input value through the dialog box, such as the offset value or the direction, the result is computed only when you click on the Preview or OK buttons. Would the value be inconsistent with the selected geometry, a warning message is displayed, along with a warning sign onto the geometry. If you move the pointer over this sign, a longer message is displayed to help you continue with the operation. Check the Both Sides button to create two parallel curves, symmetrically in relation to the selected curve, and provided it is compatible with the initial curve's curvature radius.

•

•

The second parallel curve has the same offset value as the first parallel curve. In that case it appears as aggregated under the first element. Therefore both parallel curves can only be edited together and the aggregated element alone cannot be deleted. If you use the Datum mode, the second parallel is not aggregated under the first one, but two datum elements are created. • Use the Repeat object after OK checkbox to create several parallel curves, each separated from the initial curve by a multiple of the offset value. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK. The options set in the dialog box are retained when exiting then returning to the Parallel curve function.

•

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What's New Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

Editing Surface and Wireframe Definitions
This task shows how to edit the definition of an already created geometric element. 1. Activate the Definition dialog box of the element that you want to edit in one of the following ways: • • • Select the element then choose the xxx.object -> Definition menu item from the contextual menu Select the element then choose the Edit -> xxx.object -> Definition command Double-click the element identifier in the specification tree

2. Modify the definition of the element by selecting new reference elements or by entering new values. 3. Click OK to save the new definition.

Creating Associative Isoparametric Curves
This task describes how to manage an isoparametric curve associated with a support. • • The association between the isoparametric curve and the support allows the application to update the curve according to the support modification in automatic update mode. This command is action/object only.

Open the FreeStyle_02.CATPart document.

1. Click the Isoparametric Curve icon: The Isoparametric curve dialog box appears. In the Selection page display, Support is highlighted.

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2. Select Surface.1 as curve support.

The Selection page display is updated in the Isoparametric Curve dialog box: Isoparameter is highlighted.

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What's New

The isoparametric curve is previewed on the surface when you move the cursor.

3. Click to indicate where to create the isoparametric curve. The isoparametric curve is pre-created, a manipulator is displayed. You can move the curve using the manipulator arrows.

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A contextual menu is available when you right-click the manipulator:

• • •

Edit: this command allows you to define the isoparametric curve according to its parameters. Keep this point: this command allows you to create the point where you clicked. Swap UV: this command allows you to swap U and V parameter values.

4. Select Swap UV from the contextual menu. The isoparametric curve parameters are swapped.

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5. Select Keep this point from the contextual menu. The point is created.

6. Select Edit from the contextual menu. The Tuner dialog box appears.

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7. Select Relative option in the Tuner dialog box. The relative origin of the curve is displayed on the curve support.

The Tuner dialog box is modified: • • True Length option is displayed. Reset Origin button is displayed.

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8. Click Reset Origin in the Tuner dialog box. The relative origin of the curve is reset from the curve point.

The Tuner dialog box displays the new origin values.

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9. Click Close in the Tuner dialog box. 10. Click OK in the Isoparametric curve dialog box. The isoparametric curve is created.

The Isoparameter.1 object is created in the specification tree.

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A point and line have been created: • • The point corresponds to the cursor location when you define the curve. The line corresponds to the curve orientation when you define the curve.

The Swap UV parameter contains the information indicating that the curve has been swapped.

About Editing Isoparametric Curve
You can edit an existing isoparametric curve using the contextual menu from the Isoparameter.n object command (specification tree or geometrical object), and selecting the Definition contextual command: • • You can change the curve support by selecting Support in the Selection page display of the Isoparametric Curve dialog box that appears. You can modify the curve parameters in the same way as during its creation.

Creating Surfaces
Creating Surfaces
Generative Shape Design allows you to model both simple and complex surfaces using techniques such as lofting, sweeping and filling. Create extruded surfaces: select a profile, specify the extrusion direction, and define the start and end limits of the extrusion Create revolution surfaces: select a profile, a rotation axis, and define the angular limits of the revolution surface Create spherical surfaces: select the center point of the sphere, the axis-system defining the meridian and parallel curves, and define the angular limits of the

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geometry spherical surface Create cylindrical surfaces: select the center point of the circle and specify the extrusion direction. Create offset surfaces: select the surface to be offset, enter the offset value and specify the offset direction Create swept surfaces: select one or more guiding curves, the profile to be swept, possibly a spine, reference surface, and start and end values Create fill surfaces: select curves, or surface edges, forming a closed boundary, and specify the continuity type Create multi-sections surfaces: select two or more planar section curves, possibly guide curves and a spine, and specify tangency conditions Create blend surfaces: select two curves, and possibly their support, specify the tension, continuity, closing point and coupling ratio, if needed

Creating Developable Surfaces
This task shows how to create a developable surface by selecting two curves. 1. Click the Developable Surface icon .

The Developable Surface dialog box appears.

2. Successively select any two curves or edges.

3. Click OK to create the developable surface. The surface (identified as Developable Surface.xxx) is added to the specification

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Creating Revolution Surfaces
This task shows how to create a surface by revolving a planar profile about an axis. Open the Revolution1.CATPart document.

1. Click the Revolve icon

.

The Revolution Surface Definition dialog box appears.

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2. Select the Profile and a line indicating the desired Revolution axis. 3. Enter angle values or use the graphic manipulators to define the angular limits of the revolution surface.

4. Click OK to create the surface. The surface (identified as Revolute.xxx) is added to the specification tree.

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What's New

• •

There must be no intersection between the axis and the profile. However, if the result is topologically consistent, the surface will still be created. If the profile is a sketch containing an axis, the latter is selected by default as the revolution axis. You can select another revolution axis simply by selecting a new line.

Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

Creating Spherical Surfaces
This task shows how to create surfaces in the shape of a sphere. The spherical surface is based on a center point, an axis-system defining the meridian & parallel curves orientation, and angular limits. Open the Sphere1.CATPart document. 1. Click the Sphere icon from the Extrude-Revolution toolbar.

The Sphere Surface Definition dialog box is displayed.

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2. Select the center point of the sphere. 3. Select an axis-system. This axis-system determines the orientation of the meridian and parallel curves, and therefore of the sphere. By default, if no axis-system has been previously created in the document, the axis-system is the document xyz axis-system. Otherwise the default axis-system is the current one. 4. Click Preview to preview the surface.

5. Modify the Sphere radius and the Angular Limits as required. Here we choose -90 and 0 and 90 for the parallel curves, and 240 for the meridian curves, and left the radius at 20 mm.

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Parallel angular limits are comprised within the -90 Meridian angular limits are comprised within the -360 6. Click OK to create the spherical surface.

and 90 and 360

range. range.

The spherical surface (identified as Sphere.xxx) is added to the specification tree.

You can also choose to create a whole sphere. In this case, simply click the icon from the dialog box to generate a complete sphere, based on the center point and the radius. The parallel and meridian angular values are then grayed.

Parameters can be edited in the 3D geometry. To have further information, please refer to the Editing Parameters chapter.

Creating Cylindrical Surfaces
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geometry

This task shows how to create a cylinder by extruding a circle along a given direction. Open the Cylinder1.CATPart document. 1. Click the Cylinder icon .

The Cylinder Surface Definition dialog box appears.

2. Select the Point that gives the center of the circle to be extruded and specify the desired Direction of the cylinder axis. You can select a line to take its orientation as the direction or a plane to take its normal as direction. You can also specify the direction by means of X, Y, Z vector components by using the contextual menu on the Direction area.

3. Select the Radius of the cylinder. 4. Enter values or use the graphic manipulators to define the start and end limits of the extrusion.

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5. You can click the Reverse Direction button to display the direction of the cylinder on the other side of the selected point or click the arrow in the 3D geometry. 6. Click OK to create the surface. The surface (identified as Cylinder.xxx) is added to the specification tree.

Creating Offset Surfaces
This task shows you how to create a surface, or a set of surfaces, by offsetting an existing surface, or a set of surfaces. It can be any type of surface, including multi-patch surfaces resulting from fill or any other operation. Open the Offset1.CATPart document. 1. Click the Offset icon .

The Offset Surface Definition dialog box appears.

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2. Select the Surface to be offset. An arrow indicates the proposed direction for the offset. In P1 mode, you can only select mono-element surfaces. 3. Specify 200mm as the Offset value.

4. Click Preview to preview the offset surface. The offset surface is displayed normal to the reference surface.

5. Click OK to create the surface. The surface (identified as Offset.xxx) is added to the specification tree. Depending on the geometry configuration and the offset value, an offset may not be allowed as it would result in a debased geometry. In this case, you need

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What's New to decrease the offset value or modify the initial geometry. The Parameters tab allows you to: • display the offset surface on the other side of the reference surface by clicking either the arrow or the Reverse Direction button.

•

define the smoothing: o None: the smoothing is constant o Automatic (you can use the Offset3.CATPart document): a local smoothing is applied only if the constant offset cannot be performed. It cleans the geometry of the surface and enables the offset. A warning panel is launched and the modified surface is shown in the 3D geometry. If a surface still cannot be offset, no smoothing is performed and a warning message is issued (as in the constant offset mode).

•

generate two offset surfaces, one on each side of the reference surface, by checking the Both sides option.

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geometry

•

create several offset surfaces, each separated from the initial surface by a multiple of the offset value, by checking the Repeat object after OK option. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK. Remember however, that when repeating the offset it may not be allowed to create all the offset surfaces, if it leads to debased geometry.

•

Would the value be inconsistent with the selected geometry, a warning message is displayed, along with a warning sign onto the geometry. If you move the pointer over this sign, a longer message is displayed to help you continue with the operation.

Furthermore, the manipulator is locked, and you need to modify the value within the dialog box and click Preview.

• •

The options set in the dialog box are retained when exiting then returning to the Offset function. When you modify an input value through the dialog box, such as the

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What's New offset value or the direction, the result is computed only when you click on the Preview or OK buttons.
Removing Sub-Elements

The Sub-Elements to remove tab helps you for the analysis in case the offset encounters a problem. Open the Offset2.CATPart document. 1. Perform steps 1 to 4. 2. Click Preview. The Warning dialog box appears, the geometry shows the erroneous subelements, and flag notes display sub-elements to remove.

3. Click Yes to accept the offset.

In the Offset Surface Definition dialog box, the Sub-Elements to remove tab lists the erroneous sub-elements and a preview of the offset is displayed.

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• •

If you move the mouse over a flag note, a longer message giving an accurate diagnosis is displayed. You can remove a sub-element by right-clicking it and choosing Clear Selection from the contextual menu.

The following modes are optional, you may use them if you need to add or remove a sub-element to create the offset. • Add Mode: when you click an unlisted element in the geometry, it is added to the list when you click a listed element, it remains in the list Remove Mode: when you click an unlisted element in the geometry, the list is unchanged when you click a listed element, it is removed from the list

•

If you double-click the Add Mode or Remove Mode button, the chosen mode is permanent, i.e. successively selecting elements will add/remove them. However, if you click only once, only the next selected element is added or removed. You only have to click the button again, or click another one, to deactivate the mode. The list of sub-elements to remove is updated each time an element is added. Note that if you modify an input in the Offset dialog box, the list is re-initialized. 4. Click Preview. The offset surface is displayed normal to the reference surface. 5. Click OK to create the surfaces. The surfaces (identified as Offset.xxx) are added to the specification tree.

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Performing a Temporary Analysis

While in the Offset command, you can perform a temporary analysis in order to check the connections between surfaces or curves. Open the Offset4.CATPart document. 1. Perform steps 1 to 4 (set 20mm as the Offset value). 2. Click Preview. The Temporary Analysis icon is available from the Tools toolbar. 3. Click the Temporary Analysis mode icon either the Connect checker icon . 5. Click OK in the Connect checker or Curve connect checker dialog box. You must activate the temporary analysis mode before running any analysis. Otherwise, a persistent analysis will be performed. The Temporary Analysis node is displayed in the specification tree and the associated analysis (here Curve Connection Analysis.1) appears below. .

4. Select the analysis to be performed in the Analysis toolbar by clicking or the Curve connect checker icon

The analysis is not persistent. Thus when you click OK in the Offset Definition dialog box to create the curve, the Temporary Analysis node disappears from the specification tree. An option is available from Tools -> Options to let you automatically set the analysis as temporary. Refer to the Customizing section. Parameters can be edited in the 3D geometry. To have further information, refer to the Editing Parameters chapter.

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Creating Swept Surfaces
Creating Swept Surfaces
You can create a swept surface by sweeping out a profile in planes normal to a spine curve while taking other user-defined parameters (such as guide curves and reference elements) into account. You can sweep an explicit profile: • • along one or two guide curves (in this case the first guide curve is used as the spine by default) along one or two guide curves while respecting a specified spine.

The profile is swept out in planes normal to the spine. In addition, you can control the positioning of the profile while it is being swept by means of a reference surface. The profile position may be fixed with respect to the guide curve (positioned profile) or user-defined in the first sweep plane. You can sweep an implicit linear profile along a spine. This profile is defined by: • • • • • • two guide curves and two length values for extrapolating the profile a guide curve and a middle curve a guide curve, a reference curve, an angle and two length values for extrapolating the profile a guide curve, a reference surface, an angle and two length values for extrapolating the profile a guide curve, and a reference surface to which the sweep is to be tangent a guide curve and a draft direction

You can sweep an implicit circular profile along a spine. This profile is defined by: • • • • three guide curves two guide curves and a radius value a center curve and two angle values defined from a reference curve (that also defines the radius) a center curve and a radius. • Generally speaking, the sweep operation has a derivative effect, meaning that there may be a continuity loss when sweeping a profile along a spine. If the spine presents a curvature continuity, the surface presents at least a tangency continuity. If the spine presents a tangency continuity, the surface presents at least a point continuity.

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What's New • Generally speaking, the spine must present a tangency continuity. However, in a few cases, even though the spine is not tangent continuous, the swept surface is computed: o when the spine is by default the guide curve and is planar, as the swept surface is extrapolated then trimmed to connect each of its segments. Note that if a spine is added by the user, the extrapolation and trim operations are not performed. o when consecutive segments of the resulting swept surface do not present any gap.

Tangency discontinuous spine with connex swept segments (the sweep is created)

Tangency discontinuous spine with non connex swept segments (the sweep is not created)

Defining Laws for Swept Surfaces Whatever the type of sweep, whenever a value is requested (angle or length) you can click the Law button to display the Law Definition dialog box. It allows you to define your own law to be applied rather than the absolute value.

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geometry The Law Viewer allows you to: - visualize the law evolution and the maximum and minimum values, - navigate into the viewer by panning and zooming (using to the mouse), - trace the law coordinates by using the manipulator, - change the viewer size by changing the panel size - reframe on by using the viewer contextual menu - change the law evaluation step by using the viewer contextual menu (from 0.1 (10 evaluations) to 0.001 (1000 evaluations)).

Four law types are available: a. Constant: a regular law, only one value is needed. b. Linear: a linear progression law between the Start and End indicated values c. S type: an S-shaped law between the two indicated values d. Advanced: allowing to select a Law element as defined in Creating Laws. Check the Inverse law button to reverse the law as defined using the above options. You can also apply laws created with the Knowledge Advisor workbench to swept surfaces. The law can be negative, providing the curves are curvature continuous.

Removing Twisted Areas During creation or edition, you can now generate swept surfaces that have a twisted area by delimiting the portions of the swept surface to be kept. The

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What's New generated surface is therefore composed of several unconnected parts. This capability is available with all types of swept surfaces, except for the With tangency surface and With two tangency surfaces subtypes of the linear profile, and the One guide and tangency surface and With two surfaces subtypes of the circular profile. Open the Sweep-Twist.CATPart document. Let's take an example by creating a swept surface with an implicit linear profile. 1. Click the Sweep icon . The Swept Surface Definition dialog box appears. 2. Click the Line profile icon and choose the With Reference surface subtype. 3. Select Curve.1 as the Guide Curve 1. 4. Select the xy plane as the reference surface. 5. Define a Length 1 of 30 mm and a Length 2 of 10 mm. 6. Click Preview. An error message displays asking you to use a guide with a smaller curvature. 7. Click OK in the dialog box.

Two manipulators ("cutters") appear for each untwisted zone. Their default positions are the maximal zone delimiters out of which they cannot be dragged. This maximal zone corresponds to the larger untwisted portion of the swept surface. 8. Use these manipulators to delimit the portions of the swept surface you want to keep.

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geometry curve is not closed. We advise you to cut a bit less than the maximal zone to delimit a safety area around the twisted portion. A contextual menu is available on the manipulators: • Reset to initial position: sets the manipulators back to their default positions, thqt is the position defined as the maximal zone. Remove twisted areas management: removes the manipulators and performs the swept surface generation again.

•

9. Click Preview again in the Swept Surface Definition dialog box. The swept surface is generated. 7.

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10. Click OK to create the swept surface.

•

If you modify the length value after clicking Preview, and the swept surface to be generated has no twisted area, the generated swept surface will still be cut. Use the Remove twisted areas management option to start the operation again. As the generated surface is composed of several unconnected part, the Multi-result management dialog box opens. For further information, refer to the Managing Multi-Result Operations chapter.

•

Creating Swept Surfaces Using an Explicit Profile
This task shows you how to create swept surfaces that use an explicit profile. These profiles must be T- or H-shaped profiles. The following sub-types are available: • • • With reference surface With two guide curves With pulling direction

You can use the wireframe elements shown in this figure. Open the Sweep1.CATPart document.

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1. Click the Swept Surface icon

.

The Swept Surface Definition dialog box appears. 2. Click the Explicit profile icon, then use the drop-down list to choose the subtype. With reference surface

• • •

Select the Profile to be swept out (DemoProfile1). Select a Guide curve (DemoGuide1). Select a surface (by default, the reference surface is the mean plane of the spine) in order

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control the position of the profile during the sweep. Note that in this case, the guiding curve must lie completely on this reference surface, exce if it is a plane. You can impose an Angle on this surface. Click the Law button if you want a specific law to be applied rather that the absolute angle value. See Defining Laws for Swept Surfaces.

With two guide curves

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• • •

Select the Profile to be swept out (DemoProfile1). Select a first Guide curve (DemoGuide1). Select a second Guide curve (DemoGuide2).

You can also specify anchor points for each guide. These anchor points are intersection points between the guides and the profile's plane or the profile itself, through which the guiding curves w pass.

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What's New There are two anchoring types: • •

Two points: select anchor points on the profile that will be matched respectively to Guide Curve 1 and 2. These points must belong to the sweeping plane of the profile. If the profile is open, these points are optional and the extremities of the profile are used. Point and direction: select an anchor point on the profile which will be matched onto Guide Curve 1 and an anchor direction. In each sweeping plane, the profile is rotated around the anchor point so that the anchor direction (linked to this profile) is aligned with the two guide curves, from Guide Curve 1 to Guide Curve 2.

Sweep without positioning Two points anchoring type

Sweep without positioning Point and direction anchoring type

If the profile is manually positioned defining anchor points will position the profile between the guides, matching the anchor points with guide intersection points, prior to performing the sweepin operation.

With pulling direction The With pulling Direction subtype is equivalent to the With reference surface subtype with a reference plane normal to the pulling direction.

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geometry

• • • •

Select the Profile to be swept out (DemoProfile2). Select a first Guide curve (DemoGuide1). Select a Direction (zx plane). Optionally, you can impose an Angle. Click the Law button if you want a specific law to be applied rather that the absolute angle value. See Defining Laws for Swept Surfaces.

(scenario continues for all sub-types) 3. If needed, select a Spine. If no spine is selected, the guide curve is implicitly used as the spine. Here is an example with DemoGuide2.

If the plane normal to the spine intersects one of the guiding curves at different points, it is advise to use the closest point to the spine point for coupling.

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4. Click OK to create the swept surface. The surface (identified as Sweep.xxx) is added to the specification tree. •

Check the Projection of the guide curve as spine option so that the projected spine is the projection of the guide curve onto the reference plane. This option is only available with the Pulling direction sub-type and with the Reference surface sub type providing the reference surface is a plane. • You can define spine relimiters (points or planes) in order to longitudinally reduce the doma of the sweep, if the swept surface is longer than necessary for example. Below is an example with a plane as Relimiter 1. When there is only one relimiter, you are able to choose the direction of the sweep by clicking the green arrow.

Relimiters can be selected on a closed curve (curve, spine, or default spine). In that case, you are advised to define points as relimiters, as plane selection may lead to unexpected

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geometry results due to multi-intersection. You can relimit the default spine, thus avoiding to split it to create the sweep. •

In the Smooth sweeping section, you can check: o the Angular correction option to smooth the sweeping motion along the reference surface. This may be necessary when small discontinuities are detected with regard the spine tangency or the reference surface's normal. The smoothing is done for any discontinuity which angular deviation is smaller than 0.5 degree, and therefore helps generating better quality for the resulting swept surface. o the Deviation from guide(s) option to smooth the sweeping motion by deviating from the guide curve(s).

•

If you want to manually position the profile, click the Position profile option. You can then directly manipulate the profile using the graphic manipulators in the geometry or access positioning parameters clicking on the Show Parameters>> button. These parameters allow you to position the profile in the first sweep plane.

o o o o o o

Specify a positioning point in the first sweep plane by either entering coordinates or selecting a point. Specify the x-axis of the positioning axis system by either selecting a line or specifyi a rotation angle. Select the X-axis inverted check box to invert the x-axis orientation (while keeping t y-axis unchanged). Select the Y-axis inverted check box to invert the y-axis orientation (while keeping t x-axis unchanged). Specify an anchor point on the profile by selecting a point. This anchor point is the origin of the axis system that is associated with the profile. Specify an axis direction on the profile by selection a direction. If no anchor direction was previously defined, the x-axis of the positioning axis system is used to join the extremities of the profile. The x-axis is aligned with the reference surface.

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Reference Surface

Two Guides

If you want to go back to the original profile, uncheck the Position profile option.

It is not mandatory that the profile be a sketch.

Creating Swept Surfaces Using a Linear Profile
This command is only available with the Generative Shape Design 2 product. This task shows how to create swept surfaces that use an implicit linear profile. The following subtypes are available: • Two limits • Limit and middle • With reference curve • With reference surface

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• • •

With tangency surface With draft direction With two tangency surfaces

Open the Sweep1.CATPart document. 1. Click the Sweep icon . The Swept Surface Definition dialog box appears. 2. Click the Line profile icon, then use the drop-down list to choose the subtype.
Two limits:

• •

Select two guide curves. You can enter one or two length values to define the width of the swept surface.

Limit and middle:

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• •

Select two guide curves. Select the Limit and middle option from the list to use the second guide curve as middle curve.

Checking the Second curve as middle curve button automatically selects this mode.
With reference surface:

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•

•

Select a guide curve, a reference surface, and key in an angle value. The guiding curve must lie completel y on this reference surface, except if the latter is a plane. You can enter one or two length values to define the width of the swept surface.

With reference curve:

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•

•

Select a guide curve, a reference curve, and key in an angle value. You can enter one or two length values to define the width of the swept surface.

With tangency surface:

•

•

Select a guide curve, and a reference surface to which the sweep is to be tangent. Depending on the geometry, there may be one or two solutions from which to choose, either by clicking on the

C

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solution displayed in red (inactive) or using the Next button. Check the Trim with tangency surface to perform a trim between the swept surface and the tangency surface. The part of the tangency surface that is kept is chosen so that the final result is tangent.
With two tangency surfaces:

Solu

Open the Sweep5.CATPart document.

•

Select a spine, and two tangency surfaces.

Swept surface with

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Check the Trim with tangency surface to perform a trim between the swept surface and the tangency surface. The part of the tangency surface that is kept is chosen so that the final result is tangent.

Trim with first tan surface

In any of the above cases, you can select a spine using the Spine field if you want to specify a spin If no spine is selected, the guide curve is implicitly used as the spine. Defining Relimiters You can define relimiters (points or planes) in order to longitudinally reduce the domain of the sweep, if the swept surface is longer than necessary for example. Besides is an example with a plane as Relimiter 1. When there is only one relimiter, you are able to choose the direction of the sweep by clicking the green arrow. • Relimiters can be selected on a closed curve (curve, spine, or default spine). In that case, you are advised to define points as relimiters, as plane selection may lead to unexpected results due to multiintersection. You can relimit the default spine, thus avoiding to split it to create the sweep. You can stack the creation of the elements by using the contextual menu available in either field

• •

This option is available with the Draft direction sweep type. • In the Smooth sweeping section, you can check: o the Angular correction option to smooth the sweeping motion along the reference surface. This may be necessary when small discontinuities are detected with regards to the spine

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o

tangency or the reference surface's normal. The smoothing is done for any discontinuity which angular deviation is smaller than 0.5 degree, and therefore helps generating better quality for the resulting swept surface the Deviation from guide(s) option to smooth the sweeping motion by deviating from the guide curve(s). A curve smooth is performed using correction default parameters in tangency and curvature. This option is not available for with tangency surface subtype.

3. Click OK to create the swept surface. The surface (identified as Sweep.xxx) is added to the specification tree. Click the Law button if you want a specific law to be applied rather that the absolute angle value.

Parameters can be edited in the 3D geometry. To have further information, please refer to the Edi

With draft direction:

Open the Sweep6.CATPart document.

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•

Select a guide curve and a draft direction (a line, a plane or components), o Select the draft computation mode: Square: equivalent to implicit linear profile swept surface with reference surface, using a plane normal to the draft direction as reference surface, and the projection of the guide curve onto this plane as spine Cone: envelop of cones defined along a given curve. In order to have swept start and end planes similar as the square mode, the guide curve needs to be extrapolated and the resulting surface split as explained in the following figure. o Choose the angular definition: Wholly defined: the angular value varies during the whole sweeping operation G1-Constant: a different draft value for every G1 section can be set; in this case, a relimiting plane is requested when defining lengths Location values: on given points on the curve, angular values can be

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defined. In the Wholly defined tab, you can click the Law... button to display the Law Definition dialog box. The 2D viewer enables you to previsualize the law evolution before applying it. 1. Enter Start and End values. 2. Choose the law type to be applied to the pitch. Four law types are available: a. Constant: a regular law, only one value is needed. b. Linear: a linear progression law between the Start and End indicated values c. S type: an S-shaped law between the two indicated values d. Advanced: allowing to select a Law element as defined in Creating Laws. For the S type pitch, you need to define a second pitch value. The pitch distance will vary between these two pitch values, over the specified number of revolutions. The Law Viewer allows you to: - visualize the law evolution and the maximum and minimum values, - navigate into the viewer by panning and zooming (using to the mouse), - trace the law coordinates by using the manipulator, - change the viewer size by changing the panel size - reframe on by using the viewer contextual menu - change the law evaluation step by using the viewer contextual menu (from 0.1 (10 evaluations) to 0.001 (1000 evaluations)). 3. Check the Inverse law button to reverse the law as defined using the above options. 4. Click Close to return to the Swept Surface Definition dialog

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box. This option is available with both Square and Cone computation mode. • Choose the length types: o From curve: the swept surface starts from the curve o Standard: the length is computed in sweeping planes o From/Up to: the length is computed by intersecting a plane or a surface; a point can be selected: a plane parallel to the draft plane would be computed o From extremum: the lengths are defined along the draft direction from an extremum plane; L1 corresponds to the "maximum plane" in the draft direction, L2 corresponds to the "minimum plane" in the draft direction o Along Surface: The boundary opposite to the guide curve is computed: it is the exact euclidean parallel curve of the guide curve.

The location value tab is only available for a square computation mode and will work only on G1 curves. The start (or end) section of the swept surface (in yellow) does not coincide with the expected relimiting plane (in green). As a consequence, the blue portion needed is missing. Here are the steps performed to create the swept surface: 1. The guide curve is extrapolated in curvature (pink curve) 2. The result is split by the green plane to obtain the green end section. As an information purpose, we put all the elements explaining the steps above in Open_body 2, so that you understand how the sweet surface is created.

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1. In the example above, we selected the 2. In the example above, we selected the following following values values Curve.1 as guide curve Curve.1 as guide curve Plane.1 as draft direction Plane.1 as draft direction Square as computation mode Square as computation mode 20deg as Wholly constant angle 35deg as Wholly constant angle Standard Length type From / Up To 50mm as Length 1 Point 1 as Relimiting element 1 20mm as Length 2

3. In the example above, we selected the following values Curve.1 as guide curve Plane.1 as draft direction Cone as computation mode 25deg as Wholly constant angle From Extremum type 50mm as Length 1

4. In the example above, we selected the following values Curve.1 as guide curve Plane.1 as draft direction Square as computation mode 20deg as Wholly constant angle Along surface type 30mm as Length 1

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Creating Swept Surfaces Using a Circular Profile

This task shows how to create swept surfaces that use an implicit circular profile. The following subtypes are available: • • • • • • Three guides Two guides and radius Center and two angles Center and radius Two guides and tangency surface One guide and tangency surface

You can use the wireframe elements shown in this figure.

Open the Sweep1.CATPart document. 1. Click the Swept Surface icon .

The Swept Surface Definition dialog box appears. 2. Click the Circle icon, then use the drop-down list to choose the subtype. The two following cases are possible using guide curves. Three guides:

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•

Select three guide curves.

Two guides and radius:

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•

Select two guide curves and enter a Radius value. You can then choose between four possible solutions by clicking the Other Solution button.

In the example above, the radius value is 45. The two following cases are possible using a center curve. Center and two angles:

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•

Select a Center Curve and a Reference angle curve. You can relimit the swept surface by entering two angle values.

In the example above, we selected the following values: Center curve: DemoGuide 1 Reference angle: DemoGuide 3 Angle 1: 50 deg Angle 2: 0 deg

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Center and radius:

•

Select a Center Curve and enter a Radius value.

In the example above, we selected the following values: Center curve: DemoGuide 3 Reference angle: DemoGuide 1 Angle 1: 0 deg Angle 2: 60 deg

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geometry The two following cases are possible using a reference surface to which the swept surface is to be tangent: Two guides and tangency surface:

• •

Select two guide curves, and a reference surface to which the sweep is to be tangent. Depending on the geometry, there may be one or two solutions from which to choose. The solution displayed in red shows the active sweep.

Choosing a solution One guide and tangency surface:

Resulting Sweep

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What's New

•

Select a guide curves, a reference surface to which the sweep is to be tangent, and enter a radius value.

Check the Trim with tangency surface to perform a trim between the swept surface and the tangency surface. The part of the tangency surface that is kept is chosen so that the final result is tangent.

Choosing a solution

Resulting Sweep

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Sweep 2 with Trim option (scenario continues for all sub-types) In any of the above cases, you can select a spine using the Spine field if you want to specify a spine different from the first guide curve or center curve. If the plane normal to the spine intersects one of the guiding curves at different points, it is advised to use the closest point to the spine point for coupling. Defining Relimiters You can define relimiters (points or planes) in order to longitudinally reduce the domain of the sweep, if the swept surface is longer than necessary for example. Below is an example with a plane as Relimiter 1. When there is only one relimiter, you are able to choose the direction of the sweep by clicking the green arrow.

• • •

Relimiters can be selected on a closed curve (curve, spine, or default spine). In that case, you are advised to define points as relimiters, as plane selection may lead to unexpected results due to multi-intersection. You can relimit the default spine, thus avoiding to split it to create the sweep. You can stack the creation of the elements by using the contextual menu available in either field. In the Smooth sweeping section, you can check: o the Angular correction option to smooth the sweeping motion along the reference surface. This may be necessary when small discontinuities are detected with regards to the spine tangency or the reference surface's normal. The smoothing is done for any discontinuity which angular deviation is smaller than 0.5 degree, and therefore helps generating better quality for the resulting swept surface. o the Deviation from guide(s) option to smooth the sweeping motion by deviating from the guide curve(s). A curve smooth is performed using correction default parameters

•

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What's New in tangency and curvature. This option is not available for One guide and tangency surface subtype.

3. Click OK to create the swept surface. The surface (identified as Sweep.xxx) is added to the specification tree. Click the Law button if you want a specific law to be applied rather that the absolute angle value. See Defining Laws for Swept Surfaces. This option is not available with the Three guides and Two guides and tangency surface sub-types.

Creating Swept Surfaces Using a Conical Profile

This command is only available with the Generative Shape Design 2 product. This task shows how to create swept surfaces that use an implicit conical profile, such as parabolas, hyperbolas or ellipses These swept surfaces are created based on guide curves and tangency directions. The latter can be defined either by the supporting surface or a curve giving the direction. The following sub-types are available: • • • • Two guides Three guides Four guides Five guides

Open the Sweep2.CATPart. 1. Click the Swept Surface icon .

The Swept Surface Definition dialog box appears. 2. Click the Conic icon, then use the drop-down to choose the subtype. Two guides

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• •

Select two guide curves and their tangency supports, indicating an angle value in relation to the support, if needed. Set the Parameter value. It is a ratio ranging from 0 to 1 (excluded), and is used to define a passing point as described in Creating Conic Curves and illustrated in the diagram.

Three guides

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•

Select three guide curves, and the tangency supports for the first and last guides. If needed, indicate an angle in relation to the support.

Four guides

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geometry

•

Select four guide curves and the tangency support for the first guide. If needed, indicate an angle in relation to the support.

Five guides

Open the Sweep3.CATPart.

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•

Select five guide curves.

(scenario continues for all sub-types) In any of the above cases, you can select a spine using the Spine field if you want to specify a spine different from the first guide curve or center curve. If the plane normal to the spine intersects one of the guiding curves at different points, it is advised to use the closest point to the spine point for coupling. Defining Relimiters You can define relimiters (points or places) in order to longitudinally reduce the domain of the sweep, if the swept surface is longer than necessary for instance. Below is an example with a plane as Relimiter 1.

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geometry When there is only one relimiter, you are able to choose the direction of the sweep by clicking the green arrow.

• • •

Relimiters can be selected on a closed curve (curve, spine, or default spine). In that case, you are advised to define points as relimiters, as plane selection may lead to unexpected results due to multi-intersection. You can relimit the default spine, thus avoiding to split it to create the sweep. You can stack the creation of the elements by using the contextual menu available in either field. Provided you are using two, three, or four guides, in the Smooth sweeping section, you can check: o the Angular correction option to smooth the sweeping motion along the reference surface. This may be necessary when small discontinuities are detected with regards to the spine tangency or the reference surface's normal. The smoothing is done for any discontinuity which angular deviation is smaller than 0.5 degree, and therefore helps generating better quality for the resulting swept surface. o the Deviation from guide(s) option to smooth the sweeping motion by deviating from the guide curve(s).

•

3. Click OK to create the swept surface. The surface (identified as Sweep.xxx) is added to the specification tree.

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What's New Click the Law button if you want a specific law to be applied rather that the absolute angle value. See Defining Laws for Swept Surfaces. This option is not available with the Five guides sub-type.

Creating Fill Surfaces
This task shows how to create fill surfaces between a number of boundary segments. Open the Fill1.CATPart document. 1. Click the Fill icon .

The Fill Surface Definition dialog box appears.

2. Select curves or surface edges to form a closed boundary. You can select a support surface for each curve or edge. In this case continuity will be assured between the fill surface and selected support surfaces. 3. Use the combo to specify the desired continuity type between any selected support surfaces and the fill surface: • • • Point Tangent, or Curvature continuity.

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geometry The fill surface is displayed within the boundary.

4. You can edit the boundary by first selecting an element in the dialog box list then choosing a button to either: • • • • • Add a new element after or before the selected one Remove the selected element Replace the selected element by another curve Replace the selected support element by another support surface Remove the selected support element.

5. Click in the Passing point field, and select a point. This point is a point through which the filling surface must pass, thus adding a constraint to its creation. However, you may need to alleviate the number of constraints by removing the supports. This point should lie within the area delimited by the selected curves. If not, the results may be inconsistent. The Planar Boundary Only check box allows you to fill only planar boundaries, when the boundary is defined by one curve on one surface. 6. Click OK to create the fill surface. The surface (identified as Fill.xxx) is added to the specification tree.

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What's New

Filling surface without specified supports

Filling surface with a passing point and no specified supports

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Filling surface with specified supports (Extrude 1 and Extrude 2) and a tangency continuity

Filling surface with a passing point, specified supports (Extrude 1 and Extrude 2) and a tangency continuity • The selected curves or surface edges can intersect. Therefore a relimitation of the intersecting boundaries is performed to allow the creation of the fill surface.

Two consecutive boundaries must have only one intersection. Selected curves cannot be closed curves.

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What's New

•

The selected curves or surfaces edges can have non-coincident boundaries. Therefore, an extrapolation is performed to allow the creation of the fill surface.

The distance between non-coincident boundaries must be smaller than 0.1mm.

A two-side fill surface cannot be created in the following ambiguous cases: • one intersection and two distances below 0.1 mm

•

no true intersection (therefore there may be several distances below 0.1 mm)

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geometry

Creating Multi-sections Surfaces
This task shows how to create a multi-sections surface and includes the following functionalities: • • • • • • Edit Smooth parameters Spine Relimitation Canonical Element Coupling

You can generate a multi-sections surface by sweeping two or more section curves along an autom computed or user-defined spine. The surface can be made to respect one or more guide curves. Open the Loft1.CATPart document. 1. Click the Multi-sections Surface icon .

The Multi-sections Surface Definition dialog box appears.

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What's New

2. Select two or more planar section curves. The curves must be continuous in point.

You can select tangent surfaces for the start and end section curves. These tangent surfaces mus not be parallel to the sections. A closing point can be selected for a closed section curves. Here is a multi-sections surface defined by three planar sections:

•

Sections can be 3D curves with following restrictions: o the intersection between one 3D profile and all guides must be coplanar (if three gui more are defined) o in case of a user-defined spine, this spine must be normal to the plane implicitly obta above.

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3. If needed, select one or more guide curves. Guide curves must intersect each section curve and must be continuous in point. The first guide curve will be a boundary of the multi-sections surface if it intersects the first extremity of each sections curve. Similarly, the last guide curve will be a boundary of the multi-sections surface if it intersects the extremity of each section curve. Here is a multi-sections surface defined by 2 planar sections and 2 guide curves:

You can make a multi-sections surface tangent to an adjacent surface by selecting an end section t the adjacent surface. In this case, the guides must also be tangent to the surface. In Figure 2 a multi-sections surface tangent to the existing surface has been created:

Figure 1

Figure 2

You can also impose tangency conditions by specifying a direction for the tangent vector (selecting take its normal, for example). This is useful for creating parts that are symmetrical with respect to Tangency conditions can be imposed on the two symmetrical halves. Similarly, you can impose a tangency onto each guide, by selection of a surface or a plane (the dir tangent to the plane's normal). In this case, the sections must also be tangent to the surface. 4. Click OK to create the multi-sections surface. The surface (identified as Multi-sections Surface.xxx) is added to the specification tree. Extremum points are now aggregated under the parent command that created them and put in no the specification tree.

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What's New

Editing a Multi-sections Surface

It is possible to edit the multi-sections surface reference elements by first selecting a curve in the d list, or by selecting the text on the figure, then choosing a button to either: • remove the selected curve • replace the selected curve by another curve • add another curve

More possibilities are available with the contextual menu and by right-clicking on the red text or on object. For example, it is possible to remove and replace tangent surfaces and closing points.

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geometry

The following example illustrates the result when the tangency condition is removed between the b sections surface and the adjacent surface.

Defining Smooth Parameters
In the Smooth parameters section, you can check: •

•

the Angular Correction option to smooth the lofting motion along the reference guide curves be necessary when small discontinuities are detected with regards to the spine tangency or reference guide curves' normal. The smoothing is done for any discontinuity which angular d smaller than 0.5 degree, and therefore helps generating better quality for the resulting mul surface. the Deviation option to smooth the lofting motion by deviating from the guide curve(s).

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What's New

If you are using a both Angular Correction and Deviation options, it is not guaranteed that the spin kept within the given tolerance area. The spine may first be approximated with the deviation tolera each moving plane may rotate within the angular correction tolerance.

Selecting a Spine

In the Spine tab page, select the Spine check box to use a spine that is automatically computed or curve to impose that curve as the spine. • • •

It is strongly recommended that the spine curve be normal to each section plane and must continuous in tangency. Otherwise, it may lead to an unpredictable shape. If the plane normal to the spine intersects one of the guiding curves at different points, it is use the closest point to the spine point for coupling. You can create multi-sections surfaces between closed section curves. These curves have po continuity at their closing point. This closing point is either a vertex or an extremum point automatically detected and highlig the system. By default, the closing points of each section are linked to each other.

The red arrows in the figures below represent the closing points of the closed section curves change the closing point by selecting any point on the curve.

The surface is twisted

A new closing point has been imposed to get a non-twisted surface

Relimitating the Multi-sections Surface
The Relimitation tab lets you specify the relimitation type. You can choose to limit the multi-sections surface only on the Start section, only on the End sectio or on none. Open the Loft3.CATPart document.

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geometry

a. when one or both are checked: the multi-sections surface is limited to corresponding section b. when one or both are when unchecked: the multi-sections surface is swept along the spine: o if the spine is a user spine, the multi-sections surface is limited by the spine extremi the first guide extremity met along the spine. o if the spine is an automatically computed spine, and no guide is selected: the multi-s surface is limited by the start and end sections o if the spine is an automatically computed spine, and one or two guides are selected: sections surface is limited by the guides extremities. o if the spine is an automatically computed spine, and more than two guides are select spine stops at a point corresponding to the barycenter of the guide extremities. In an the tangent to the spine extremity is the mean tangent to the guide extremities.

Multi-sections surface relimitation option checked on both Start and End section

Multi-sections surface relimitation option unchecked on End section only

After the multi-sections surface is relimited, the following constraint needs to be fulfilled: the plane the spine defined at the relimitation point must intersect the guide(s) and the point(s) resulting fro intersection must belong to the section.

Using a Canonical Element

Use the Canonical portion detection check button in the Canonical Element tab to automatically det surfaces to be used as planes for features needing one in their definition.

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What's New

Initial multi-sections surface with planar faces

Using a planar face as reference for a sketch

Resulting sketch

This task presents the two kinds of coupling during the creation of the multi-sections surface surfac • • coupling between two consecutive sections coupling between guides

These couplings compute the distribution of isoparameters on the surface. Open the Loft2.CATPart document.
Coupling between two consecutive sections

This coupling is based on the curvilinear abscissa. 1. Click the Multi-sections Surface icon .

The Multi-sections Surface Definition dialog box appears. 2. Select the two consecutive sections.

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geometry

3. Click OK to create the multi-sections surface.

If you want to create a coupling between particular points, you can add guides or define the coupli

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What's New

Coupling between guides

This coupling is performed by the spine. If a guide is the concatenation of several curves, the resulting multi-sections surface will contain as surfaces as curves within the guide.

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geometry

Several coupling types are available, depending on the section configuration: • Ratio: the curves are coupled according to the curvilinear abscissa ratio.

•

Tangency: the curves are coupled according to their tangency discontinuity points. If they d the same number of points, they cannot be coupled using this option.

• •

Tangency then curvature: the curves are coupled according to their tangency continuity firs curvature discontinuity points. If they do not have the same number of points, they cannot using this option. Vertices: the curves are coupled according to their vertices. If they do not have the same n vertices, they cannot be coupled using this option.

Manual Coupling

If the number of vertices differ from one section to another, you need to perform a manual couplin 1. Select the sections for the multi-sections surface, and check their orientations.

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What's New

2. In the Coupling tab, choose the Tangency option and click Apply. An error message is displayed as the number of discontinuity points on the first section is greate than on the other two sections.

The points that could not be coupled, are displayed in the geometry with specific symbol depending selected mode, along with coupling lines:

•

In Tangency mode: uncoupled tangency discontinuity points are represented by a square

•

In Tangency then curvature mode: o uncoupled tangency discontinuity points are represented by a square o uncoupled curvatures discontinuity points are represented by a empty circle

•

In Vertices mode: uncoupled vertices are represented by a full circle

3. Click in the coupling list, or choose Add coupling in the contextual menu, or using the Add b manually select a point on the first section. The Coupling dialog box is displayed.

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geometry

4. Select a corresponding coupling point on each section of the multi-sections surface. The Coupling dialog box is updated consequently, and the coupling curve is previewed, provided Display coupling curves option is active. When a coupling point has been defined on each section, this dialog box automatically disappear

5. Click OK. The multi-sections surface is created as defined with the coupling specifications.

The same multi-sections surface without coupling and with Ratio option would have looked like th

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What's New

Note the increased number of generated surfaces.

• •

You can create coupling point on the fly, using the Create coupling point contextual menu it on the document background to display the contextual menu) instead of selecting an existin To edit the coupling, simply double-click the coupling name in the list (Coupling tab) to disp Coupling dialog box. Then you select the point to be edited from the list and create/select a coupling point, then click OK. Use the contextual menu on the coupling list to edit defined couplings.

•

Creating Blended Surfaces
This task shows how to create a blended surface, that is a surface between two wireframe elements, taking a number of constraints into account, such as tension, continuity, and so forth. Several cases are worth surveying:

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geometry

• • •

blend between curves blend between closed contours coupling blend

Open the Blend1.CATPart document. 1. Click the Blend icon .

The Blend Surface Definition dialog box appears.

Blend between curves:

1. Successively select the first curve and its support, then the second curve and its support. These can be surface edges, or any curve.

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What's New

2. Set the continuity type using the Basic tab. It defines the continuity connection between the newly created surface and the curves on which it lies. The illustration above, shows the Tangency continuity, and the following illustrations show the Point and Curvature continuity types:

Point continuity on both limits

Curvature

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geometry

3. Activate the Trim first/second support option, on one or both support surfaces to trim them by the curve and assemble them to the blend surface: By default the blend surface borders are tangent to the support surface borders.

You can also specify whether and where the blend boundaries must be tangent to the supports boundaries: • Both extremities: the tangency constraint applies at both ends of the curve • None: the tangency constraint is disregarded • Start extremity: the tangency constraint applies at the start endpoint of the curve only • End extremity: the tangency constraint applies at the end endpoint of the curve only The Start and End extremities are defined according to the arrows in the blended surface's preview. 4. Set the tension type using the Tension tab. It defines the tension of the blend at its limits. It can be constant or linear, and can be set for each limit independently. A third tension type is available: S Type. It enables to set a variable tension.

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What's New

If you choose any of the tension types in the drop-down list, the Default option is deselected. 5. Click OK.
Blend between closed contours:

1. Successively select two contours.

2. Click Preview. The surface to be generated is twisted. To avoid this you need to define a closing point.

By default, the system detects and highlights a vertex on each curve that can be used as a closing point, or it creates an extremum point (you can also manually select another one if you wish). 3. Choose the Closing Points tab, and using the contextual menu, choose Create Projection on the First closing point.

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geometry

4. The Projection Definition dialog box is displayed. 5. Select the closing point on the second contour, then the first curve onto which the point is to be projected.

6. Click OK in the Projection Definition dialog box.

7. Click OK in the Blend Definition dialog box. The blend is correctly created.

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What's New

Coupling blend:

1. Select the elements to be blended and click Preview.

2. Select the Coupling / Spine tab and define the coupling type.

• • •

•

Ratio: the curves are coupled according to the curvilinear abscissa ratio. Tangency : the curves are coupled according to their tangency discontinuity points. If they do not have the same number of points, they cannot be coupled using this option. Tangency then curvature: the curves are coupled according to their tangency continuity first then curvature discontinuity points. If they do not have the same number of points, they cannot be coupled using this option. Vertices: the curves are coupled according to their vertices. If they do not have the same number of vertices, they cannot be coupled using this option.

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geometry

When using the above coupling types, the Spine field is disabled. • Spine: the curve are coupled using a spine curve. This curve can either be a new curve or one of the curves already specified. If no spine is explicitly selected, the first curve is used as the default one. Here is how the blended surface is computed using this coupling mode: at any given point on the spine, a plane normal to the spine is first computed then coupling points corresponding to the intersection of this plane with the limit curves are computed. The blended surface corresponds to the set of lines created with the coupled points. This construction is similar to the one used when creating swept surfaces using a linear profile and two guide curves. In the Spine field, select the spine curve. When using this option, the Display coupling curves option is disabled and any manual coupling is removed.

3. Click in the coupling list, or choose Add in the contextual menu, or using the Add button, and manually select a point on the first section. The Coupling dialog box is displayed.

4. Select a corresponding coupling point on each section. The Coupling dialog box is updated consequently, and the coupling curve is previewed, provided the Display coupling curves option is active. When a coupling point has been defined on each section, this dialog box automatically disappears.

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What's New

5. Click OK.

The surface (identified as Blend.xxx) is added to the specification tree. • • • • Selecting a support is not compulsory. You can create closing points using the contextual menu on the First or Second closing point fields in the dialog box, or using the contextual menu directly on one of the selected curves. Use the Replace, Remove, or Reverse buttons, to manage the selected elements (curves, support, closing and coupling points). You can also use the contextual menu on the texts displayed on the geometry to set the continuities, trim the supports or manage the curves and support in general.

Creating Extruded Surfaces
This task shows how to create a surface by extruding a profile along a given direction. Open the Extrude1.CATPart document. 1. Click the Extrude icon .

The Extruded Surface Definition dialog box appears. 2. Select the Profile to be extruded (Sketch.1). 3. Specify the desired extrusion Direction (xy plane). • • You can select a line to take its orientation as the extrusion direction or a plane to take its normal as extrusion direction. You can also specify the direction by means of X, Y, Z vector components by using the contextual menu on the Direction area.

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geometry

3. Define the Extrusion Limits for Limit 1 and Limit 2. • Dimension: enter length values or use the graphic manipulators to define the start and end limits of the extrusion. Here we defined a length of 30mm for Limit 1 and 80mm for Limit 2.

•

Up-to element: select a geometric element. It can be a point, a plane or a surface. If a point is specified, the up-to element is the plane normal to the extrusion direction passing through the given point.

Wires cannot be select as an up-to element. Here we selected Point.1 as Limit 1 and Plane.1 as Limit 2.

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What's New

You can also select different extrusion limits, for instance a Dimension for Limit 1 and an Up-to element for Limit 2:

•

•

The up-to element can intersect the profile and the surface to be extruded. In the latter case, it must completely cut the surface and there should not be any partial intersections of the up-to element with the surface. If you select two up-to elements, they must not cut each other within the surface to be extruded.

4. Click OK to create the surface. The surface (identified as Extrude.xxx) is added to the specification tree. You can click the Reverse Direction button to display the extrusion on the other side of the selected profile or click the arrow in the 3D geometry. Parameters can be edited in the 3D geometry. For further information, refer to the Editing Parameters chapter.

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geometry

Performing Operations on Shape Geometry
Performing Operations on Shape Geometry
Generative Shape Design allows you to modify your design using techniques such as trimming, extrapolating and filleting. Join geometry: select at least two curves or surfaces to be joined. Heal geometry: select at least two surfaces presenting a gap to be healed. Smooth a curve: select the curve to be smoothed and set the tangency threshold Restore an element: select a split element, and click the icon. Disassemble elements: select a multi-cell element, and choose the disassembling mode. Split geometry: select the element to be split and a cutting element. Trim geometry: select two elements to be trimmed and specify which side of element. Create boundary curves: select a surface's edge, set the propagation type, and re-define the curve limits if needed. Extract geometry: select an edge or the face of a geometric element, and set the propagation type. Extract multiple edges: select one or more element(s) of a sketch, and click OK. Reshape Corners: click either the Edge Fillet icon or the Variable Radius Fillet icon, select the edge to be filleted, click More>> and define the corner to reshape and the setback distance. Translate geometry: select an element, a translation direction (line, plane or vector), specify the translation distance. Rotate geometry: select an element, a line as the rotation axis, and specify the rotation angle. Perform symmetry on geometry: select an element, then a point, line, or plane as reference element. Transform geometry by scaling: select an element, then a point, plane, or planar surface as reference element, and specify the scaling ratio. Transform geometry by affinity: select an element to be transformed, specify the axis system characteristics, and the enter the affinity ratio values.

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What's New Transform geometry from an axis to another: select an element to be transformed, specify the axis system characteristics, and the enter the affinity ratio values. Extrapolate a surface: select a surface boundary then the surface itself, specify the extrapolation limit (value or limiting surface/plane), and specify the extremities constraints (tangent/normal). 5. Extrapolate a curve: select a curve endpoint then the curve itself, specify the extrapolation limit (length value or limiting surface/plane), and specify the continuity constraints (tangent/curvature). Invert geometry orientation: select the Insert -> Operations -> Invert Orientation menu item, then the surface or curve whose orientation is to be inverted, click the orientation arrow, and click Invert Orientation again to accept the inverted element. Create the nearest sub-element: select the Insert -> Operations -> Near menu item, the element made of several sub-elements, then a reference element whose position is close to the sub-element to be created. Create laws: select a reference line and a curve.

Surfaces and Curves
Joining Surfaces or Curves
This task shows how to join surfaces or curves. Open the Join1.CATPart document. 1. Click the Join icon .

The Join Definition dialog box appears.

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geometry

In Part Design workbench, the Join capability is available as a contextual command named 'Create Join' that you can access from Sketch-based features dialog boxes. 2. Select the surfaces or curves to be joined.

3. You can edit the list of elements to be joined: • by selecting elements in the geometry: o Standard selection (no button clicked): when you click an unlisted element, it is added to the list when you click a listed element, it is removed from the list o Add Mode: when you click an unlisted element, it is added to the list when you click a listed element, it remains in the list o Remove Mode: when you click an unlisted element, the list is unchanged when you click a listed element, it removed from the list by selecting an element in the list then using the Remove\Replace

•

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What's New contextual menu items. If you double-click the Add Mode or Remove Mode button, the chosen mode is permanent, i.e. successively selecting elements will add/remove them. However, if you click only once, only the next selected element is added or removed. You only have to click the button again, or click another one, to deactivate the mode. 4. Right-click the elements from the list and choose the Check Selection command. This lets you check whether an element to be joined presents any intersection (i.e. at least one common point) with other elements prior to creating the joined surface. If this command is not launched, possible intersections will not be detected.

The Checker dialog box is displayed, containing the list of domains (i.e. sets of connected cells) belonging to the selected elements from the Elements To Join list. 5. Click Preview.

•

An Information message is issued when no intersection is found.

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geometry

•

When an element is self-intersecting, or when several elements intersect, a text is displayed on the geometry, where the intersection is detected.

6. Click Cancel to return to the Join Definition dialog box. 7. Right-click the elements again and choose the Propagation options to allow the selection of elements of same dimension. • • G0 Propagate: the tolerance corresponds to the Merging distance value. G1 Propagate: the tolerance corresponds to the Angular Threshold value, if defined. Otherwise, it corresponds to the G1 tolerance value as defined in the part.

Each new element found by propagation of the selected element(s) is highlighted and added to the Elements To Join list. Note that: • • • The initial element to propagate cannot be a sub-element Forks stop the propagation Intersections are not detected

8. Click Preview in the Join Definition dialog box. The joined element is previewed, and its orientation displayed. Click the arrow to invert it if needed.

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What's New

The join is oriented according to the first element in the list. If you change this element, the join's orientation is automatically set to match the orientation of the new topmost element in the list. 9. Check the Check tangency option to find out whether the elements to be joined are tangent. If they are not, and the option is checked, an error message is issued. 10. Check the Check connexity option to find out whether the elements to be joined are connex. If they are not, and the button is checked, an error message is issued indicating the number of connex domains in the resulting join. When clicking Preview, the free boundaries are highlighted, and help you detect where the joined element is not connex. 11. Check the Check manifold option to find out whether the resulting join is manifold.

• •

The Check manifold option is only available with curves. Checking it automatically checks the Check connexity option. If two elements are not connex and the Check connexity option is deselected, the Multi-Result Management dialog box is displayed.

In case one of the above checks fails, an error message is issued and elements in error are highlighted in the 3D geometry. • The Simplify the result check option allows the system to automatically reduce the number of elements (faces or edges) in the resulting join whenever possible. • The Ignore erroneous elements option lets the system ignore surfaces and

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geometry edges that would not allow the join to be created. 12. You can also set the tolerance at which two elements are considered as being only one using the Merging distance. 13. Check the Angular Threshold option to specify the angle value below which the elements are to be joined. If the angle value on the edge between two elements is greater than the Angle Tolerance value, the elements are not joined. This is particularly useful to avoid joining overlapping elements. 14. Click the Federation tab to generate groups of elements belonging to the join that will be detected together with the pointer when selecting one of them. For further information, see Using the Federation Capability. 15. Click the Sub-Elements To Remove tab to display the list of sub-elements in the join. These sub-elements are elements making up the elements selected to create the join, such as separate faces of a surface for example, that are to be removed from the join currently being created. You can edit the sub-elements list as described above for the list of elements to be joined.

16. Check the Create join with sub-elements option to create a second join, made of all the sub-elements displayed in the list, i.e. those that are not to be joined in the first join. This option is active only when creating the first join, not when editing it. 17. Click OK to create the joined surface or curve. The surface or curve (identified as Join.xxx) is added to the specification tree. Sometimes elements are so close that it is not easy to see if they present a gap or not, even though they are joined. Check the Surfaces' boundaries option from the Tools -> Options menu item, General, Display, Visualization tab.

Using the Federation Capability

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What's New

This option is only available with the Generative Shape Design 2 product. The purpose of the federation is to regroup several elements making up the joined surface or curve. This is especially useful when modifying linked geometry to avoid re-specifying all the input elements. Open the Join2.CATPart document. 1. Create the join as usual, selecting all elements to be joined. (Make sure you do not select Sketch.1). 2. From the Join Definition dialog box click the Federation tab, then select one of the elements making up the elements federation. You can edit the list of elements taking part in the federation as described above for the list of elements to be joined. 3. Choose a propagation mode, the system automatically selects the elements making up the federation, taking this propagation mode into account.

• •

No federation: no element can be selected All: all elements belonging to the resulting joined curve/surface are part of the federation. Therefore, no element can be explicitly selected.

•

Point continuity: all elements that present a point continuity with the selected elements and the continuous elements are selected; i.e. only those that are separated from any selected element is not included in the federation

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geometry

•

Tangent continuity: all the elements that are tangent to the selected element, and the ones tangent to it, are part of the federation

Here, only the top faces of the joined surface are detected, not the lateral faces.

To federate a surface and its boundaries in tangency, you need to select the face as well as the edges: both face and edges will be federated. • No propagation: only the elements explicitly selected are part of the propagation

4. Choose the Tangency Propagation federation mode as shown above. 5. Move to the Part Design workbench, select the Sketch.1, and click the Pad

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icon to create an up to surface pad, using the joined surface as the limiting surface. 6. Select the front edge of the pad, and create a 2mm fillet using the Edge Fillet icon.

7. Double-click the Sketch.1 from the specification tree, then double-click the constraint on the sketch to change it to 10mm from the Constraint Definition dialog box.

Sketch prior to modification lying over two faces 8. Exit the sketcher .

Sketch after modification lying over one face only

The up to surface pas is automatically recomputed even though it does not lie over the same faces of the surface as before, because these two faces belong to the same federation. This would not be the case if the federation including all top faces would not have been created, as shown below. 9. Double-click the joined surface (Join.1) to edit it, and choose the No propagation federation mode. 10. Click OK in the Join Definition dialog box. A warning message is issued, informing you that an edge no longer is recognized on the pad. 11. Click OK.

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geometry

The Update Diagnosis dialog box is displayed, allowing you to re-enter the specifications for the edge, and its fillet.

You then need to edit the edge and re-do the fillet to obtain the previous pad up to the joined surface. 12. Select the Edge.1 line, click the Edit button, and re-select the pad's edge in the geometry. 13. Click OK in the Edit dialog box. The fillet is recomputed based on the correct edge.

Restoring a Surface
In this task you will learn how to restore the limits of a surface or a curve when it has been split using the Break Surface or Curve workbench) or the Split Surface workbenches). icon (FreeStyle

icon (Generative Shape Design and Wireframe &

Open the FreeStyle_06.CATPart document. 1. Click the Untrim Surface or Curve icon The Untrim dialog box is displayed. in the Operations toolbar.

2. Select the surface which limits should be restored. The dialog box is updated accordingly.

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3. Click OK in the dialog box. A progression bar is displayed, while the surface is restored. It automatically disappears once the operation is complete (progression at 100%).

The initial surface is automatically restored.

The restored surface or curve is identified as Surface Untrim.xxx or Curve Untrim.xxx. You can perform a local untrim on faces. Three modes of selection are available: • selection of the face: the initial surface is restored:

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geometry

•

selection of an inner loop: only this loop is restored:

•

selection of the outer loop: only this loop is restored:

• •

• • •

If the surface has been trimmed several times, it is the initial surface which is restored. To partially untrim the surface, you need to use the Undo command right after the trim. If the surface to be restored is closed (in the case of a cylinder) or infinite (in the case of an extrude), the limits of the untrim feature will be the bounding boxes of the initial surface. Therefore, the initial surface and the untrim surface may be identical. You can individually select a vertex or a boundary from the restored surface or curve. Multi-selection is available and allows to create several untrim features in one step. All untrim features will appear in the specification tree. The datum creation capability is available from the Dashboard.

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What's New

Smoothing Curves

This task shows how to smooth a curve, i.e. fill the gaps, and smooth tangency and curvature discontinuities, in order to generate better quality geometry when using this curve to create other elements, such as swept surfaces for example. Open the Smooth1.CATPart document. 1. Click the Curve Smooth icon .

The Curve Smooth Definition dialog box is displayed.

2. Select the curve to be smoothed. Texts are displayed on the curve indicating its discontinuities before smoothing, and type of discontinuity (point, curvature or tangency) and their values (In area). These values type are expressed in the following units: • • • for a point discontinuity: the unit is the document's distance unit (mm by default) for a tangency discontinuity: the unit is the document's angular unit (degree by default) for a curvature discontinuity: the value is a ratio between 0 and 1 which is defined as follows: if ||Rho1-Rho2|| / ||Rho2|| < (1-r)/r where Rho1 is the curvature vector on one side of the discontinuity, Rho2 the curvature vector on the other side, and r the ratio specified by

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geometry the user; then the discontinuity is smoothed. For example, r=1 corresponds to a continuous curvature and r=0.98 to the model tolerance (default value). A great discontinuity will require a low r to be smoothed.

3. Click Preview to display texts indicating the curve discontinuities that are still present after the smoothing operation, and whether they are within the threshold values (yellow box) or outside the set values (red box) (Out area). The following elements C0, C1 and C2 that are displayed before the discontinuity information indicate that the vertex is respectively point continuous (C0), tangent continuous (C1) and curvature continuous (C2). The value and location of the Maximum deviation between the curve to be smoothed and the smoothed curve are displayed in the 3D geometry.

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What's New

In the example, from top to bottom, once the curve is smoothed: • • • • the tangency discontinuity still is present there is no more discontinuity, the point discontinuity is corrected the curvature discontinuity still is present, even though it is slightly modified (different In and Out values) the curvature discontinuity still is present and not improved at all

Basically: • • • a red box indicates that the system could not find any solution to fix the discontinuity while complying with the specified parameters a yellow box indicates that some discontinuity has been improved, where there was a point discontinuity there now is a tangency discontinuity for example a green box indicates that the discontinuity no longer exists; it has been smoothed.

Defining tangency and curvature thresholds, the maximum deviation and the continuity 4. From the Parameters tab modify the Tangency threshold, that is the tangency discontinuity value above which the curve is smoothed. If the curve presents a tangency discontinuity greater than this threshold, it is not smoothed. If you increase the threshold value to 1.0 in our example, you notice that the Tangency discontinuity which value was below 1 changes to a curvature discontinuity.

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geometry

5. Similarly, you can check the Curvature threshold button to set curvature discontinuity value above which the curve is smoothed. 6. Define a Maximum deviation value to set the allowed deviation between the initial curve and the smoothed curve. Therefore, the resulting smoothed curve fits into a pipe which radius is the maximum deviation value and the center curve is defined by the selected curve. 7. Define the Continuity, that is the correction mode for the smoothing, by checking either: • Threshold: default mode. The tangency and curvature thresholds options are taken into account. • Point: no point discontinuity should remain. There is no point discontinuity in our example. • Tangency: no tangent discontinuity should remain. The tangency threshold option is not taken into account, it is grayed out and the defined value is ignored. You notice that the Tangency discontinuity changes to a curvature discontinuity.

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What's New

•

Curvature: no curvature discontinuity should remain. The curvature threshold option is not taken into account, it is grayed out and the defined value is ignored. You notice that there is no discontinuity any more.

In case tangent or curvature discontinuities remain, an error message is issued. Optionally, you can select a surface on which the curve lies. In this case the smoothing is performed so that the curve remains on the Support surface. From this ensues that the maximum degree of smoothing is limited by the support surface's level of discontinuity.

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geometry

Selecting Elements not to be smoothed 8. Click the Freeze tab. This tab enables you to select sub-elements of the curve that should not be smoothed. These sub-elements can either be vertices or edges. In case of a vertex, the local neighborhood remains unchanged, thus keeping the discontinuity. The Remove button enables to remove a single or a set of subelements.

External elements cannot be selected as sub-elements. Setting continuity conditions You now set continuity conditions on the resulting smoothed curve for each extremity with regards to the input curve. As a comparison basis, the continuity condition was previously always curvature: the output curve had the same extremity points, tangencies and curvatures as the input curve. 9. Click the Extremities tab and define the continuity conditions at each curve's extremity: • 234 Curvature (by default): extremity point, tangency and curvature are the

What's New same Tangency: extremity point and tangency are the same (curvature can be different) Point: extremity points are the same (tangency and curvature can be different)

• •

You can also right-click the icon at the curve's extremity and choose one of the following options:

Point and Tangency conditions can only be successfully applied if the Maximum Deviation is larger than 0.005mm. Note that these extremity conditions do not affect closed curves. You can also sequentially move from one conditions to the next one by clicking on the icons. Visualizing messages 10. Click the Visualization tab.

This tab lets you define the way the messages are displayed on the smoothed element. You can choose to see: • All the messages: those indicating where the discontinuity remains (red box) as well as those indicating where the discontinuity type has changed, or allows smoothing.

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geometry

•

only those messages indicating where the discontinuity is Not corrected and remains.

•

None of the messages.

You can also choose to: • Display information interactively: only the pointers in the geometry are displayed, above whichthe text appears when passing the pointer

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What's New

•

Display information sequentially: only one pointer and text are displayed in the geometry, and you can sequentially move from one pointer to the other using the backward/forward buttons

The Topology simplification check button automatically deletes vertices on the curves when the curve is curvature continuous at these vertices, thus reducing its number of segments. When this is the case, the displayed text indicates: Out: discontinuity erased to inform you that a simplification operation took place. This text is also displayed when two vertices are very close to each other and the system erases one to avoid the creation of very small edges (i.e. shorter than 10 times the model tolerance) between two close vertices. 11. Click OK. The smoothed curve (identified as Curve smooth.xxx) is added to the specification tree. When smoothing a curve on support that lies totally or partially on the boundary edge of a surface or on an internal edge, a message may be issued indicating that the application found no smoothing solution on the support. In this case, you must enter a Maximum deviation value smaller than or equal to the tolerance at which two elements are considered as being only one (0.001mm by default) to keep the result on the support.

Creating Boundary Curves
This task shows how to create the boundary curve of a surface. Open the Boundaries1.CATPart document. 1. Click the Boundary icon .

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geometry

The Boundary Definition dialog box appears.

2. Use the combo to choose the Propagation type: • • • • Complete boundary: the selected edge is propagated around the entire surface boundary. Point continuity: the selected edge is propagated around the surface boundary until a point discontinuity is met. Tangent continuity: the selected edge is propagated around the surface boundary until a tangent discontinuity is met. No propagation: no propagation or continuity condition is imposed, only the selected edge is kept.

You can select the propagation type before selecting an edge. 3. Select a Surface edge. The boundary curve is displayed according to the selected propagation type.

No propagation

Tangent continuity

Point continuity

Complete boundary

4. You can relimit the boundary curve by means of two elements.

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What's New If you relimit a closed curve by means of only one element, a point on curve curve for example, the closure vertex will be moved to the relimitation point, allowing this point to be used by other features. 5. Click OK to create the boundary curve. The curve (identified as Boundary.xxx) is added to the specification tree. • If you select the surface directly, the Propagation type no longer is available, as the complete boundary is automatically generated.

Provided the generated boundary curve is continuous, you can still select limiting point to limit the boundary.

Using the red arrow; you can then invert the limited boundary.

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geometry

If you select a curve which has an open contour, the Propagation type becomes available: choose the No Propagation type and select the curve again. The extremum points will define the boundary result.

You cannot copy/paste a boundary from a document to another. If you wish to do so, you need to copy/paste the surface first into the second document then create the boundary.

Healing Geometry
This task shows how to heal surfaces, that is how to fill any gap that may be appearing between two surfaces. This command can be used after having checked the connections between elements for example, or to fill slight gaps between joined surfaces. Open the Healing1.CATPart document from the Join Healing toolbar. 1. Click the Healing icon.

The Healing Definition dialog box appears.

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What's New

2. Select the surfaces to be healed.

3. You can edit the list of elements in the definition list: • by selecting elements in the geometry: o Standard selection (no button clicked): when you click an unlisted element, it is added to the list when you click a listed element, it is removed from the list Add Mode: when you click an unlisted element, it is added to the list when you click a listed element, it remains in the list Remove Mode: when you click an unlisted element, the list is unchanged when you click a listed element, it removed from the list

o

o

•

by selecting an element in the list then using the Remove\Replace contextual menu items.

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geometry If you double-click the Add Mode or Remove Mode button, the chosen mode is permanent, i.e. successively selecting elements will add/remove them. However, if you click only once, only the next selected element is added or removed. You only have to click the button again, or click another one, to deactivate the mode.
Parameters tab

4. Define the distance below which elements are to be healed, that is deformed so that there is no more gap, using the Merging distance. Elements between which the gap is larger than the indicated value are not processed. In our example, we increase it to 1mm. You can also set the Distance objective, i.e. the maximum gap allowed between two healed elements. By default it is set to 0.001 mm, and can be increased to 0.1 mm. 5. Change the continuity type to Tangent. In that case, the Tangency angle field becomes active, allowing you to key in the angle below which the tangency deviation should be corrected. The Tangency objective is, similarly to the Distance objective, the maximum allowed tangency deviation allowed between healed elements. The default value is 0.5 degree, but can range anywhere between 0.1 degree to 2 degrees. 6. Click Preview to visualize the maximum deviation value between the input surfaces and the result in the 3D geometry.

The value is displayed on the edge or the face onto which the deviation is maximal, not exactly where the maximum deviation is located.
Freeze tab

6. Click the Freeze tab.

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What's New

• • •

You can then define the list of frozen elements, that is the elements that should not be affected by the healing operation. You cannot freeze edges to be joined. If you want to do so, you first need to freeze the faces. You can edit the list as described above for the list of elements to be healed.

Similarly to the Elements to freeze list, when the Freeze Plane elements or Freeze Canonic elements options are checked, no selected plane/canonic element is affected by the healing operation. 7. Click OK to create the healed surfaces. The surface (identified as Heal.xxx) is added to the specification tree.

•

Check the Surfaces' boundaries option from the Tools -> Options menu item, General -> Display -> Visualization tab to display the boundaries. This may be especially useful when selecting, and also to identify gaps.

Sharpness tab

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geometry

•

Provided the Tangent mode is active, you can retain sharp edges, by clicking the Sharpness tab, and selecting one or more edges. You can edit the list of edges as described above for the list of elements to be healed. The Sharpness angle allows to redefine the limit between a sharp angle and a flat angle. This can be useful when offsetting the resulting healed geometry for example. By default this angle value is set to 0.5 degree. In some cases, depending on the geometry configuration and the set parameters, the Multi-Result Management dialog box is displayed. Click No or refer to the Managing Multi-Result Operations chapter for further information.

•

•

When the healing fail, an update error dialog is issued. Click OK to improve the geometry. The erroneous elements are displayed on the geometry.

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What's New

Visualization tab

The Visualization tab enables you to better understand the discontinuities in the model and the results of the healing action. It lets you define the way the messages are displayed on the smoothed element.

You can choose to see: • All the messages, that is to say the messages indicating where the discontinuity remains as well as those indicating where the discontinuity type has changed (in point (><) and tangency (^)).

•

only the messages indicating where the discontinuity is Not corrected

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geometry and still remains.

•

None of the messages.

You can also choose to see: • Display information interactively: only the pointers in the geometry are displayed, above which the text appears when passing the pointer

•

Display information sequentially: only one pointer and text are displayed in the geometry, and you can sequentially move from one pointer to another using the backward/forward buttons

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What's New

Disassembling Elements
In this task you will learn how to disassemble multi-cell bodies into mono-cell, or mono-domain bodies, whether curves or surfaces. Open the FreeStyle_07.CATPart document, or any document containing a multicell body. 1. Select the element to be disassembled. You can select only an edge of a surface, the system recognizes the whole element to be disassembled. Here we selected the join made of three elements, each made of several cells.

2. Click the Disassemble icon

in the Shape Modification toolbar.

The Disassemble dialog box is displayed.

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geometry

3. Choose the disassembling mode: • All Cells: all cells are disassembled, i.e. for all the selected element, a separate curve is created for each cell. • Domains Only: elements are partially disassembled, i.e. each element is kept as a whole if its cells are connex, but is not decomposed in separate cells. A resulting element can be made of several cells. The number selected elements, and the number of elements to be created according to the disassembling mode are displayed within the Disassemble dialog box. In the illustrations, we have colored the resulting curves for better identification.

Results when disassembling all cells (seven curves are created) 4. Click OK in the dialog box.

Results when disassembling domains only (three curves are created)

In case of a multi-selection, a progression bar is displayed, while the surface is being disassembled. It automatically disappears once the operation is complete (progression at 100%).

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What's New

The selected element is disassembled, that is to say independent elements are created, that can be manipulated independently. Multi-selection is available. FreeStyle workbench only: Capabilities available from the FreeStyle Dashboard are datum creation and insert in a new geometrical set.

Splitting/Trimming
Splitting Geometry

This task shows how to split a surface or wireframe element by means of a cutting element. You can split a wireframe element by a point, another wireframe element or a surface; or a surface wireframe element or another surface. • Keeping or Removing Elements • Intersecting and extrapolating • Splitting Wires • Splitting a surface by a curve or a surface by a surface • Splitting closed surfaces by two connex surfaces or curves • Splitting Volumes Open the Split1.CATPart document. 1. Click the Split icon .

The Split Definition dialog box appears.

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geometry

2. Select the element to be split. You should make your selection by clicking on the portion that you want to keep after the split.

You can select several elements to cut. In that case, click the Element to cut field again or click the

icon . The Elements to cut field opens. Select as many elements as needed. Click Close to return the Split Definition dialog box. The number of selected elements is displayed in the Element to cut

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What's New

Use the Remove and Replace buttons to modify the elements list. Use the Other side button to reverse the portion to be kept, element by element. 3. Select the cutting element. A preview of the split appears. You can change the portion to be kept by selecting that portion. You can also select the portion to be kept by clicking the Other side button. This option applies on all selected elements to cut.

•

You can select several cutting elements. In that case, note that the selection order is impor the area to be split is defined according to the side to be kept in relation to the current split element.

•

You can create a Join as the splitting element, by right-clicking in the Cutting Elements field choosing the Create Join item. If you split a surface and you keep both sides by joining the resulting splits, you cannot acc the internal sub-elements of the join: indeed, splits result from the same surface and the cu elements are common.

4. Click OK to split the element. The created element (identified as Split.xxx) is added to the specification tree.

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geometry

In the case several elements to cut were used, the created elements are aggregated under a Multi-Output.xxx feature.

In the illustrations below, the top-left line is the first splitting element. In the left illustration it defi area that intersects with the other three splitting curves, and in the illustration to the right, these t elements are useless to split the area defined by the first splitting element.

Would you need to remove, or replace, one of these cutting elements, select it from the list and cli Remove or Replace button. Keeping or Removing Elements

The Elements to remove and Elements to keep options allows to define the portions to be removed kept when performing the split operation. 1. Click in the field of your choice to be able to select the elements in the 3D geometry. 2. Right-click in the field either to clear the selection or display the list of selected elements.

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What's New

Only the selected element is removed. All other elements are kept. •

The selected elements are kept. All other elements are removed.

You must select sub-elements as elements to keep or to remove; otherwise, a warning mes is issued.

•

You can also select a point to define the portion to keep or to remove. A contextual menu is available on the Elements to remove and Elements to keep fields.

•

You do not need to select elements to keep if you already selected elements to remove and versa.

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geometry • Avoid splitting geometry when the intersection between the element to cut and the cutting element is merged with an edge of the element to cut. In that case, you can use the Elements to remove and Elements to keep options to remove positioning ambiguity.

•

Check the Keep both sides option to retain the other side of the split element after the oper In that case it appears as aggregated under the first element. Therefore both split elements can only be edited together and the aggregated element alon cannot be deleted.

If you use the Datum mode, the second split element is not aggregated under the first one, two datum surfaces are created.

In case there are several elements to cut, the Keep/Remove and Keep both sides options only app the first selected element. Intersections and extrapolations • Check the Intersections computation option to create an aggregated intersection when performing the splitting operation. This element will be added to the specification tree as Intersect.xxx.

In case there are several elements to cut, the Intersections computation option only applies on th selected element. • Uncheck the Automatic extrapolation option if do not you want the automatic extrapolation cutting curve. When a splitting curve is extrapolated, the extrapolation will performed on the original curv providing the underlying geometry (that is the curve) is long enough to be used for the extrapolation. If the Automatic extrapolation option is unchecked, an error message is issued when the cu element needs to be extrapolated, and the latter is highlighted in red in the 3D geometry. This option is available in the case of a split surface/curve or surface/surface.

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What's New

Splitting Wires •

When splitting a wire (curve, line, sketch and so forth) by another wire, you can select a su to define the area that will be kept after splitting the element. It is defined by the vectorial product of the normal to the support and the tangent to the splitting element. This is especially recommended when splitting a closed wire.

The non disconnected elements of the element to cut are kept in the result of the split.

Splitting with no support selected: first solution

Splitting with no support selected: second solution

Splitting with a selected support (xy plane): first solution

Splitting with a selected support (xy plane): second solution

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geometry Splitting a surface by a curve or a surface by a surface The following steps explain how split a surface by a curve or another surface. Split surface/curve 1. First, the cutting element (the curve) is laid down the surface.

2. Then, the result of step 1 is tangentially extrapolated in order to split the surface correctly (as shown in following figure). However, when this extrapolation leads to the intersection of the cutting element with itself prior to fully splitting the initial element, an error message is issued as there is an ambiguity about the area to be split.

If the cutting element does not reach the free edges of the element to cut, an extrapolation in tangency is performed using the part of the cutting element that lays down the surface. Split surface/surface Open the Split2.CATPart document. 1. First, an intersection (the green wire) is created between the two surface elements.

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What's New

2. Then, the result of the intersection is automatically extrapolated in tangency up to the closest free edges of the element to cut. The result of the extrapolation is used as the cutting element and the split is created.

Note that it is not the cutting element which is extrapolated but the result of the intersection. If the result of the split is not what was expected, it is also possible to manually extrapolate the cutting element with the extrapolate feature before creating the split. 1. Extrapolate the cutting element (the red surface) in order to fully intersect the element to cut.

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geometry

2. Then, use the extrapolated surface as the cutting element to split the surface.

Avoid using input elements which are tangent to each other since this may result in geometric instabilities in the tangency zone. In case surfaces are tangent or intersect face edges, please process as follow in order to avoid indeterminate positioning. Use the border edge of the cutting surface to split the element to cut: 1. Delimit the boundary of the cutting surface 2. Project this boundary onto the surface to split 3. Use this projection as the cutting element Steps 2 and 3 may be optional if the tangency constraint between the two surfaces has been clearly defined by the user during the surface creation.

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What's New

The following cases should be avoided when possible (especially when the tangency constraint between the two surfaces has not been clearly defined by the user during the surface creation), as the result of the positioning is likely to be indeterminate and the result of the intersection to be unstable.

Splitting Closed Surfaces by Two Connex Surfaces or Curves When splitting a closed surface or a curve by connex elements, an error message is issued. You need to create a join feature of non connex elements and cut the closed surface or curve with this join feature. Open the Split3.CATPart document.

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geometry

1. Click the Join icon

.

The Join Definition dialog box appears. 2. Select Split.1 and Inverse.1 as the surfaces to be joined. Be careful that both surfaces or curves to join have coherent orientations. If it is not the case, use the Invert command to invert the orientation of one of the two surfaces or curves. 3. Uncheck the Check connexity option. 4. Click OK to create the joined surface. 5. Click the Split icon .

The Split Definition dialog box is displayed. 6. Select Surface.1 as the Element to cut and Join.1 as the Cutting element. 7. Click OK to split the closed surface.

If the orientation of the elements composing the joined surface or curve is incoherent, an error message is issued when creating the split surface. Splitting Volumes This capability is only available with Generative Shape Optimizer. Providing the element to be cut is a volume and the cutting element is a volume or a surface, you can choose whether you want the result of the split to be a surface or a volume. To do so, switch to either Surface or Volume option. This switch only concerns volumes since the transformation of a surface can only be a surface. Note that the switch between surface and volume is grayed out when editing the feature. If the result of the split is a volume, the split is a modification feature. If the result of the split is a surface, the split is a creation feature. To have further information about volumes, please refer to the Creating Volumes chapter.

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What's New

The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.

Trimming Geometry
This task shows you how to trim two or more surface or wireframe elements. Open the Trim1.CATPart document. 1. Click the Trim icon .

The Trim Definition dialog box appears. 2. Select the trim mode: o o
Standard

Standard Pieces

With this mode, one portion of the selected element (surface or wire) is kept and the list of trimmed elements is ordered. The following options are explained hereafter: • • • • Selecting a Support Keeping or Removing Elements Simplifying the result Intersecting and extrapolating

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geometry

1. Select the two surfaces or two wireframe elements to be trimmed.

A preview of the trimmed elements appears and the list of trimmed elements is updated:

You can change the portion to be kept by selecting that portion.

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What's New

2. Click OK to trim the surfaces or wireframe elements. The trimmed feature (identified as Trim.xxx) is added to the specification tree.

You can also select the portions to be kept by clicking the Other side / next element and Other side / previous element buttons.

Clicking the Other side / next element button Selecting a Support •

Clicking the Other side / previous element button

When trimming wires (curve, line, sketch and so forth) by another wire, you can select a support to define the area that will be kept after trimming the element. It is defined by the vectorial product of the normal to the 263

geometry support and the tangent to the trimming element. This is especially recommended when trimming a closed wire. In our example, the Sketch composed of two lines (Sketch.11) is trimmed by the circle (Sketch.10).

Resulting trimmed element without support selection Keeping or Removing Elements

Resulting trimmed element with support selection

The Elements to remove and Elements to keep options allows to define the portions to be removed or kept when performing the trim operation. 1. Click in the field of your choice to be able to select the elements in the 3D geometry. 2. Right-click in the field either to clear the selection or display the list of selected elements.

Only the selected portion is removed. All other elements are kept.

Only the selected portion is kept. All other elements are

264

What's New removed. • You can also select a point to define the portion to keep or to remove. A contextual menu is available on the Elements to remove and Elements to keep fields.

•

You do not need to select elements to keep if you already selected elements to remove and vice-versa. Avoid trimming geometry when the intersection between the trimmed elements is merged with an edge of one of the elements. In that case, you can use the Elements to remove and Elements to keep options to remove the position ambiguity.

•

Simplifying the Result • Check the Result simplification button to allow the system to automatically reduce the number of faces in the resulting trim whenever possible.

Intersecting and extrapolating • Check the Intersections computation button to create an aggregated intersection when performing the trimming operation. This element will be added to the specification tree as Intersect.xxx.

Refer to the Splitting Geometry chapter in the case surfaces are tangent or intersect face edges. • Uncheck the Automatic extrapolation option if you do not want the automatic extrapolation of the elements to trim. If the Automatic extrapolation button is unchecked, an error message is issued when the elements to trim need to be extrapolated, and the latter

265

geometry are highlighted in red in the 3D geometry.

To be able to trim the two surfaces or wireframe elements, check the Automatic extrapolation option.

The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.
Pieces

With this mode, all trimmed curves are split together, all selected portions are kept and the list of trimmed curves is unordered. This mode is only available with curves.

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What's New

1. Select the elements to be trimmed, as shown below:

A preview of the trimmed elements appears and the list of trimmed curves is updated:

You can deselect a sub-element by selecting it again. 2. Click OK to trim the curves. The trimmed feature (identified as Trim.xxx) is added to the specification tree.

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geometry

•

• •

Check the Check connexity option to find out whether the curves to be trimmed are connex. If they are not, and the option is checked, an error message is issued indicating the number of connex domains in the resulting trimmed feature. The resulting feature is highlighted, and help you detect where the trimmed feature is not connex. Check the Check manifold option to find out whether the resulting trimmed feature is manifold. Use the Remove and Replace buttons to modify the elements list.

The following capability is available: Stacking Commands. For both modes: • • At creation, when you switch from one mode to the other, the list of selected elements is automatically reinitialized. You cannot modify the mode at edition.

Extracting Geometry
This task shows how to perform an extract from elements (curves, points, solids, volumes and so forth). This may be especially useful when a generated element is composed of several non-connex sub-elements. Using the extract capability you can generate separate elements from these sub-elements, without deleting the initial element. Open the Extract1.CATPart document. 1. Select an edge or the face of an element. The selected element is highlighted.

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What's New

2. Click the Extract icon The Extract Definition dialog box is displayed.

.

In Part Design workbench, the Extract capability is available as a contextual command named Create Extract that you can access from Sketch-based features dialog boxes. 3. Choose the Propagation type:

•

Point continuity: the extracted element will not have a hole.

•

Tangent continuity: the extracted element will be created according to tangency conditions.

•

Curvature continuity: the extracted element will be created according to curvature conditions. Define a Curvature Threshold value. For a curvature discontinuity: the value is a ratio between 0 and 1 which is defined as follows: if ||Rho1-Rho2|| / ||Rho2|| < (1-r)/r where Rho1 is the curvature vector on one side of the 269

geometry then the discontinuity is smoothed. For example, r=1 corresponds to a continuous curvature and r=0.98 to the model tolerance (default value). A great discontinuity will require a low r to be taken into account.

The extracted element must be a wire.

•

No propagation: only the selected element will be created.

4. Click OK to extract the element. The extracted element (identified as Extract.xxx) is added to the specification tree. • If you extract an edge that you want to propagate, and there is an ambiguity about the propagation side, a warning is issued and you are prompted to select a support face. In this case, the dialog box dynamically updates and the Support field is added.

•

The Complementary mode option, once checked, highlights, and therefore selects, the elements that were not previously selected, while deselecting the elements that were explicitly selected.

270

What's New You can select a volume as the element to be extracted. To do so, you can either: 1. select the volume in the specification tree, or 2. use the User Selection Filter toolbar and select the Volume Filter mode. For further information, refer to the Selecting Using A Filter chapter in the CATIA Infrastructure User's Guide. In both cases, the result of the extraction is the same whatever the chosen propagation type. • In a .CATProduct document containing several parts, you can use the extract capability in the current part from the selection of an element in another part, provided the propagation type is set to No Propagation. In this case, a curve (respectively a surface or point) is created in the current part if the selected element is a curve (respectively a surface or point); the Extract parent therefore being the created curve (respectively the surface or point). Note: o if another propagation type is selected, the extraction is impossible and an error message is issued. o when editing the extract, you can change the propagation type as the parent belongs to the current part. In the current model, if you select an element using the Tangent or Point continuity as the Propagation type, a warning is issued and you have to select No propagation instead. If the selected element has a support face and is not a surface, even though the Complementary mode option is checked, the Complementary mode will not be taken into account for the extraction and the option will therefore be inactive. After the extraction, the option will be available again. When the result of an extract is not connex (during creation or edition) due to naming ambiguity, you can now select the part to keep to solve the ambiguity. You cannot copy/paste an extracted element from a document to another. If you wish to do so, you need to copy/paste the initial element first into the second document then perform the extraction.

• •

• •

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geometry

Extracting Multiple Elements
This task shows how to extract sub-elements (curves, points, surfaces, solids, volumes and so forth) that are joined into one element. Open the MultipleExtract1.CATPart document.

1. Click the Multiple Extract icon

from the Extracts toolbar.

The Multiple Extract Definition dialog box is displayed.

2. Select the elements to be extracted. If the first selected element is a curve (or a point, a surface, a volume), the next selected element is necessarily a curve (or a point, a surface, a volume).

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What's New

3. Choose the Propagation type: • Point continuity: the extracted element will not have a hole.

•

Tangent continuity: the extracted element will be created according to tangency conditions.

•

Curvature continuity: the extracted element (necessarily a curve) will be created according to curvature conditions. Define a Curvature Threshold value. For a curvature discontinuity: the value is a ratio between 0 and 1 which is defined as follows: if ||Rho1-Rho2|| / ||Rho2|| < (1-r)/r 273

geometry where Rho1 is the curvature vector on one side of the discontinuity, Rho2 the curvature vector on the other side, and r the ratio specified by the user; then the discontinuity is smoothed. For example, r=1 corresponds to a continuous curvature and r=0.98 to the model tolerance (default value). A great discontinuity will require a low r to be taken into account.

•

No propagation: only the selected element will be created.

4. Click OK to extract the elements. Only one feature (identified as Multiple Extract.xxx) is added to the specification tree. • Providing several elements are selected and can be joined into one element after the propagation (if needed), this is automatically done within the Multiple Extract command. Otherwise, the result is not connex, you are prompted to solve the ambiguity and keep only one sub-element or all the sub-elements. Refer to Managing Multi-Result Operations for further information. The Complementary mode option, once checked, highlights, and therefore selects, the elements that were not previously selected, while deselecting the elements that were explicitly selected.

•

This option is disabled if the extracted element is a point or a volume. • Check the Federation option to generate groups of elements belonging to the resulting extracted element that will be detected together with the pointer when selecting one of its sub-elements. For further information, see Using the Federation Capability.

274

What's New • In a .CATProduct document containing several parts, you can use the multiple extract capability in the current part from the selection of an element in another part, provided the propagation type is set to No Propagation. In this case, a curve (respectively a surface or point) is created in the current part if the selected element is a curve (respectively a surface or point); the Extract parent therefore being the created curve (respectively the surface or point). Note: o if another propagation type is selected, the extraction is impossible and an error message is issued. o when editing the extract, you can change the propagation type providing the parent belongs to the current part. o in the current part, if you select an element using the Tangent, Point or Curvature continuity as the Propagation type, a warning is issued and you have to select No propagation instead. If the selected element is not tangent continuous and the propagation type is set to Tangent continuity, an error message is issued. If the selected element is a wire that is not curvature continuous and the propagation type is set to Curvature continuity, an error message is issued. If the selected element has a support face and is not a surface, even though the Complementary mode option is checked, the Complementary mode will not be taken into account for the extraction and the option will therefore be inactive. After the extraction, the option will be available again. When the result of an extract is not connex (during creation or edition) due to naming ambiguity, you can now select the part to keep to solve the ambiguity. You cannot copy/paste an extracted element from a document to another. If you wish to do so, you need to copy/paste the initial element first into the second document then perform the extraction.

• • •

• •

In case you are using the old multiple edge extract command:

Open the MultipleEdgeExtract1.CATPart document. 1. Double-click the extracted element. A warning message is issued...

... as well as the Sketch Extract dialog box:

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geometry

Only the Cancel button is available, all other fields and options are grayed out.

Transformations
Translating Geometry
This task shows you how to translate one, or more, point, line or surface element. Open the Translate1.CATPart document. 1. Click the Translate icon .

The Translate Definition dialog box appears as well as the Tools Palette. 2. Select the Element to be translated. 3. Select the Vector Definition. Direction, distance

1. Select a line to take its orientation as the translation direction or a plane to take its normal as the translation direction.

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What's New

You can also specify the direction by means of X, Y, Z vector components by using the contextual menu on the Direction field. 2. Specify the translation Distance by entering a value or using the spinners.

Point to Point

1. Select the Start point. 2. Select the End point.

Coordinates

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geometry

1. Define the X, Y, and Z coordinates. In the example besides, we chose 50mm as X, 0mm as Y, and 100 as Z. 2. When the command is launched at creation, the initial value in the Axis System field is the current local axis system. If no local axis system is current, the field is set to Default. Whenever you select a local axis system, the translated element's coordinates are changed with respect to the selected axis system so that the location of the translated element is not changed. This is not the case with coordinates valuated by formulas: if you select an axis system, the defined formula remains unchanged. This option replaces the Coordinates in absolute axis-system option.

4. Click OK to create the translated element. The element (identified as Translate.xxx) is added to the specification tree. The original element is unchanged. • Use the Hide/Show initial element button to hide or show the original element for the translation. • 278 Choose whether you want the result of the transformation to be a

What's New surface or a volume by switching to either Surface or Volume option. This capability is only available with Generative Shape Optimizer. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature. To have further information about volumes, please refer to the corresponding chapter. • Use the Repeat object after OK checkbox to create several translated surfaces, each separated from the initial surface by a multiple of the Distance value. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK.

The selection of the feature prevails over the selection of the sub-element. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. The elements to be translated are kept next time you enter the command and you change the vector definition. You can select an axis system as the Element to be translated, providing it was previously created. The element is identified as Translate.xxx in the specification tree, however the . associated icon is the axis system's You can edit the translated element's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry. The following capabilities are available: Stacking Commands, Selecting Using Multi-Output, Measure Between and Measure Item.

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geometry

Rotating Geometry
This task shows you how to rotate geometry about an axis. Open the Transform1.CATPart document. 1. Click the Rotate icon .

The Rotate Definition dialog box appears as well as the Tools Palette.

2. Define the rotation type: • Axis-Angle (default mode): the rotation axis is defined by a linear element and the angle is defined by a value that can be modified in the dialog box or in the 3D geometry (by using the manipulators). Axis-Two Elements: the rotation axis is defined by a linear element and the angle is defined by two geometric elements (point, line or plane) o Axis/point/point: the angle between the vectors is defined by the selected points and their orthogonal projection onto the rotation axis.

•

o

Axis/point/line: the angle between the vector is defined by the selected point and its orthogonal projection onto the rotation axis

280

What's New and the selected line.

o

Axis/point/plane: the angle between the vector is defined by the selected point and its orthogonal projection onto the rotation axis and the normal to the selected plane.

o

Axis/line/line: the angle between the direction vectors of the projection is defined by the two selected lines in the plane normal to the rotation axis. In case both lines are parallel to the rotation axis, the angle is defined by the intersection points of the plane normal to the rotation axis and these lines.

281

geometry

o

Axis/line/plane: the angle is defined between the selected line and the normal to the plane.

o

Axis/plane/plane: the angle is defined between the normals to the two selected planes.

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What's New

•

Three Points: the rotation is defined by three points. o The rotation axis is defined by the normal of the plane created by the three points passing through the second point. o The rotation angle is defined by the two vectors created by the three points (between vector Point2-Point1 and vector Point2Point3):

The orientation of the elements (lines or planes) is visualized in the 3D geometry by a red arrow. You can click the arrow to invert the orientation and the angle is automatically recomputed. By default, the arrow is displayed in the direction normal to the feature (line or plane). For instance, in the plane/plane mode, the arrow is displayed on each plane:

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geometry

3. Select the Element to be rotated. 4. Select the inputs depending on the chosen rotation type. 5. Click OK to create the rotated element. The element (identified as Rotate.xxx) is added to the specification tree. • Use the Hide/Show initial element button to hide or show the original element for the translation. Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option.

•

This capability is only available with Generative Shape Optimizer. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature. To have further information about volumes, please refer to the corresponding chapter. • Use the Repeat object after OK checkbox to create several rotated surfaces, each separated from the initial surface by a multiple of the Angle value. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK.

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What's New

The Repeat object after OK capability is not available with the Axis-Two Elements and Three Points rotation types. You can select an axis system as the Element to be rotated, providing it was previously created. The element is identified as Rotate.xxx in the specification tree, however the associated icon is the axis system's .

You can edit the rotated element's parameters. Refer to Editing Parameters to find out how to display these parameters in the 3D geometry. Note that the selection of the feature prevails over the selection of the subelement. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting Using A Filter chapter in the CATIA Infrastructure User's Guide. The following capabilities are available: Stacking Commands, Selecting Using Multi-Output, Measure Between and Measure Item.

Performing a Symmetry on Geometry
This functionality is P2 for FreeStyle Shaper, Optimizer, and Profiler. This task shows you how to transform geometry by means of a symmetry operation. Open the Transform1.CATPart document. 1. Click the Symmetry icon .

The Symmetry Definition dialog box appears as well as the Tools Palette.

285

geometry

2. Select the Element to be transformed by symmetry. 3. Select a point, line or plane as Reference element. The figure below illustrates the resulting symmetry when the line is used as reference element The figure below illustrates the resulting symmetry when the point is used as reference element

4. Click OK to create the symmetrical element. The element (identified as Symmetry.xxx) is added to the specification tree. • Use the Hide/Show initial element button to hide or show the original element for the translation. • Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option.

This capability is only available with Generative Shape Optimizer. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature.

286

What's New To have further information about volumes, please refer to the corresponding chapter. You can select an axis system as the Element to be transformed, providing it was previously created. The element is identified as Symmetry.xxx in the specification tree, however the associated icon is the axis system's . Note that the selection of the feature prevails over the selection of the subelement. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.

Transforming Geometry by Scaling
This task shows you how to transform geometry by means of a scaling operation. Open the Transform1.CATPart document. 1. Click the Scaling icon .

The Scaling Definition dialog box appears as well as the Tools Palette.

2. Select the Element to be transformed by scaling. 3. Select the scaling Reference point, plane or planar surface. 4. Specify the scaling Ratio by entering a value or using the drag manipulator. The figure below illustrates the resulting The figure below illustrates the resulting scaled element when the

287

geometry scaled element when the plane is used as reference element (ratio = 2). point is used as reference element (ratio = 2).

5. Click OK to create the scaled element. The element (identified as Scaling.xxx) is added to the specification tree. • Use the Hide/Show initial element button to hide or show the original element for the translation. • Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option.

This capability is only available with Generative Shape Optimizer. • Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature. This capability is only available with Generative Shape Optimizer. To have further information about volumes, please refer to the corresponding chapter. Use the Repeat object after OK checkbox to create several scaled surfaces, each separated from the initial surface by a multiple of the initial Ratio value. Simply indicate in the Object Repetition dialog box the number of instances that should be created and click OK.

•

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What's New

The selection of the feature prevails over the selection of the sub-element. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.

Transforming Geometry by Affinity
This task shows you how to transform geometry by means of an affinity operation. Open the Transform1.CATPart document. 1. Click the Affinity icon .

The Affinity Definition dialog box appears as well as the Tools Palette.

289

geometry

2. Select the Element to be transformed by affinity. 3. Specify the characteristics of the Axis system to be used for the affinity operation: • • • the Origin (Point.1 in the figures below) the XY plane (the XY plane in the figures below) the X axis (Line.1 in the figures below).

4. Specify the affinity Ratios by entering the desired X, Y, Z values. The figure below illustrates the resulting affinity with ratios X = 2, Y =1 and Z=1.

The figure below illustrates the resulting affinity with ratios X = 2, Y =1 and Z=2.

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What's New

The figure below illustrates the resulting affinity with ratios X = 2, Y =2.5 and Z=2

5. Click OK to create the affinity element. The element (identified as Affinity.xxx) is added to the specification tree. • Use the Hide/Show initial element button to hide or show the original element for the translation. • Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option.

This capability is only available with Generative Shape Optimizer. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature. To have further information about volumes, refer to the corresponding chapter.

291

geometry The selection of the feature prevails over the selection of the sub-element. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. The following capabilities are available: Stacking Commands and Selecting Using Multi-Output.

Transforming Elements From an Axis to Another
This task shows you how to transform geometry positioned according to a given axis system into a new axis system. The geometry is duplicated and positioned according to the new axis system. One or more elements can be transformed at a time, using the standard multi-selection capabilities. See also Defining an Axis System. Open the Transform2.CATPart document. 1. Click the Axis To Axis icon .

The Axis to Axis Definition dialog box appears as well as the Tools Palette.

2. Select the Element to be transformed into a new axis system.

292

What's New

3. Select the initial (Reference) axis system, that is the current one.

4. Select the Target axis system, that is the one into the element should be positioned.

5. Click OK to create the transformed element. New geometry is now positioned into the new axis system.

293

geometry

The element (identified as Axis to axis transformation.xxx) is added to the specification tree.

•

Use the Hide/Show initial element button to hide or show the original element for the translation. Choose whether you want the result of the transformation to be a surface or a volume by switching to either Surface or Volume option.

•

This capability is only available with Generative Shape Optimizer. This switch only concerns volumes since the transformation of a surface can only be a surface. Thus in case of multi-selection of volumes and surfaces, the switch only affect volumes. Note that the switch between surface and volume is grayed out when editing the feature. This capability is only available with Generative Shape Optimizer. To have further information about volumes, refer to the corresponding chapter. You can select an axis system as the Element to be transformed, providing it was previously created. The element is identified as Axis to axis transformation.xxx in the specification . tree, however the associated icon is the axis system's The selection of the feature prevails over the selection of the sub-element. To select a sub-element, you need to apply the ''Geometrical Element'' filter in the User Selection Filter toolbar. For further information, refer to the Selecting using a Filter chapter in the CATIA Infrastructure User's Guide. The following capabilities are also available: Stacking Commands and Selecting Using Multi-Output.

Inverting the Orientation of Geometry

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What's New

This task shows you how to easily invert the orientation of a surface or curve. Open any document containing wireframe or surface type element. 1. Select the Insert -> Operations -> Invert Orientation... command.

The Invert Definition dialog box is displayed.

2. Select the surface or curve whose orientation is to be inverted. An arrow is displayed on the geometry indicating the inverted orientation of the element. 3. Click the arrow to invert the orientation of the element.

4. Click OK to accept the inverted element. The element (identified as Inverse.xxx) is added to the specification tree. Once the orientation is inverted, the Reset Initial button changes to Click to Invert whether you changed the orientation using the button itself, or the arrow.

Patterns
Patterning

Create rectangular patterns: select the element to be duplicated, define the creation directions, choose the parameters you wish to define and set these parameters Create circular patterns: select the element to be duplicated, define the axial reference, the creation direction, choose the parameters you wish to define and set these parameters

Creating Rectangular Patterns

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geometry

This task shows how to use create rectangular patterns, that is to duplicate an original wireframe o type element at the location of your choice according to a rectangular arrangement. This means that you will need to define a 2-axis system using two directions. Open the Pattern1.CATPart document. 1. Click the Rectangular Pattern icon.

2. Select the element you wish to replicate as a pattern.

The Rectangular Pattern Definition dialog box is displayed. Each tab is dedicated to a directi use to define the location of the duplicated element.

3. Click the Reference element field and select a direction to specify the first direction of creat

To define a direction, you may select a line, a planar face or surface edge. You can reverse this direction by clicking the Reverse button. 4. Set the duplication parameters by choosing the number of instances, the spacing between i the total length of the zone filled with instances. Three options are available:

1. Instances & Length: the spacing between instances is automatically computed based on t number of instances and the specified total length 2. Instances & Spacing: the total length is automatically computed based on the number of 296

What's New instances and the specified spacing value

3. Spacing & Length: the number of instances is automatically computed to fit the other two parameters. For each of these cases only two fields are active, allowing you to define the correct value.

If you set Instances & Length or Spacing & Length parameters, note that you cannot define the len using formulas.

5. Click the Second Direction tab to define the same parameters along the other direction of th

You can delete instances of your choice when creating or editing a pattern. To do so, just select the materializing instances in the pattern preview. The instance is deleted, but the point remains, as you may wish to click it again to add the instanc pattern definition again.

6. Click the More>> button to display further options. These options let you position the instances in relation to the first selected element.

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geometry

7. Increase the Row in direction 2 to 2. You notice that the first selected pattern now is the second instance in the vertical direction the second selected direction.

The Simplified representation option lets you lighten the pattern geometry, when more than 15 ins generated. What you need to do is just check the option, and click Preview. The system automatica simplifies the geometry:

Previewed simplified geometry

Simplified geometry

You can also specify the instances you do not want to see by double-clicking them. These instances represented in dashed lines during the pattern definition and then are no longer visible after valida pattern creation. The specifications remain unchanged, whatever the number of instances you view option is particularly useful for patterns including a large number of instances.

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What's New

8. Click OK to create the pattern. The pattern (identified as RectPattern.xxx) is added to the specification tree.

Patterning User Features (UDFs) is not allowed.

Patterning Volumes This capability is only available with Generative Shape Optimizer. Open the PatterningVolumes1.CATPart document. 1. Click the Rectangular Pattern icon.

2. Select the element you wish to replicate as a pattern. The Rectangular Pattern Definition dialog box is displayed. 4. Set the duplication parameters by choosing the number of instances, the spacing between i the total length of the zone filled with instances.

3. Click the Reference element field and select a direction to specify the first direction of creat

5. Click OK to create the pattern.

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geometry

Creating Circular Patterns

This task shows how to use create circular patterns, that is to duplicate an original wireframe or surface-type element at the location of your choice according to a circular arrangement. Open the Pattern2.CATPart document. 1. Click the Circular Pattern icon.

2. Select the element to replicate as a pattern. Here we selected the multi-sections surface. The Circular Pattern Definition dialog box is displayed.

3. Click the Reference element field and select a direction to specify the first direction of creation, that is the rotation axis (Line.2). • • To define a direction, you can select a line, an edge or a planar face. Should you select a face, the rotation axis would be normal to that face. You can click the Reverse button to inverse the rotation direction.

4. Define the Axial Reference by choosing the Parameters type: • Instance(s) & total angle: the number of patterns as specified in the instances field are created, in the specified direction, and evenly spread

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What's New out over the total angle.

•

Instance(s) & angular spacing: the number of patterns as specified in the instances field are created in the specified direction, each separated from the previous/next one of the angular angle value.

•

Angular spacing & total angle: as many patterns as possible are created over the total angle, each separated from the previous/next one of the angular angle value.

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geometry

•

Complete crown: the number of patterns as specified in the instances field are created over the complete circle (360 deg).

•

Instances & unequal angular spacing: the number of patterns as specified in the instances field are created using a specific angular spacing between each instance. Angular spacing values are displayed between each instance.

To edit the values between each instance, you need to edit them individually. Select the angular spacing of interest, then choose one of the methods described hereafter: For instance, if you wish to change 72 degree for 100 degree for the angular spacing selected as shown in our picture, you can: 1. double-click the angle value in the 3D geometry. This displays the Parameter Definition dialog box in which you can enter the new value. 2. directly enter the new value in the Angular spacing field of the Circular

302

What's New Pattern Definition dialog box.

If you set Instance(s) & total angle or Angular spacing & total angle parameters, note that you cannot define the length by using formulas. Now you are going to add a crown to this pattern. 5. Click the Crown Definition tab, and choose which parameters you wish to define the crown.

This figure may help you define these parameters:

• • •

Circle(s) and crown thickness: you define the number of circles and they are spaced out evenly over the specified crown thickness Circle(s) and circle spacing: you define the number of circles and the distance between each circle, the crown thickness being computed automatically Circle(s) spacing and crown thickness: you define the distance between each circle and the crown thickness, and the number of circles is automatically computed.

For example, using the values described above for the Angular spacing 303

geometry & total angle option, you could define the crown as:

Note that a few patterns are created beyond the surface. You can delete instances of your choice when creating or editing a pattern. To do so, just select the points materializing instances in the pattern preview. The instance is deleted, but the point remains, as you may wish to click it again to add the instance to the pattern definition again.

6. Click the More>> button to display further options: These options let you position the instances in relation to the first selected

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What's New element.

Using these options, you can change the position of the selected element within the crown. For example, if you set the Rotation angle parameter to 30 and you uncheck the Radial alignment of instance(s) option, this is what you obtain: the initially selected element has moved 30 from its initial location, based on the rotation direction, and all instances are normal to the lines tangent to the circle.

•

The Simplified representation option lets you lighten the pattern geometry, when more than 15 instances are generated. What you need to do is just check the option, and click Preview. The system automatically simplifies the geometry:

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geometry

Not simplified geometry

Simplified geometry

You can also specify the instances you do not want to see by double-clicking them . These instances are then represented in dashed lines during the pattern definition and then are no longer visible after validating the pattern creation. The specifications remain unchanged, whatever the number of instances you view. This option is particularly useful for patterns including a large number of instances. • When checking the Radial alignment of instances, all instances have the same orientation as the original feature. When unchecked, all instances are normal to the lines tangent to the circle.

7. Click OK to create the pattern. The pattern (identified as CircPattern.xxx) is added to the specification tree.

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What's New

Patterning User Features (UDFs) is not allowed.

Patterning Volumes This capability is only available with Generative Shape Optimizer. Open the PatterningVolumes2.CATPart document. 1. Click the Circular Pattern icon.

2. Select the element you wish to replicate as a pattern. The Circular Pattern Definition dialog box is displayed. 3. Click the Reference element field and select a direction to specify the first direction of creation. 4. Define the Axial Reference by choosing the Parameters type:

5. Click OK to create the pattern.

Creating the Nearest Entity of a Multiple Element

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geometry

This task shows you how to create the nearest entity of an element that is made up from several sub-elements. Open the Near1.CATPart document. 1. Select the Insert -> Operations -> Near command. The Near Definition dialog box appears.

2. Select the element that is made up from several sub-elements. 3. Select a reference element whose position is close to the sub-element that you want to create. This example shows a parallel curve comprising three subelements. This example shows the subelement that is nearest to the reference point.

4. Click OK to create the element. This element (identified as Near.xxx) is added to the specification tree. The Near Definition dialog box is automatically displayed, when a non-connex element is detected at creation time so that you can directly choose which element should be created.

Extrapolating
Extrapolating Surfaces

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What's New

This task shows you how to extrapolate a surface boundary. Open the Extrapolate1.CATPart document. 1. Click the Extrapolate icon .

The Extrapolate Definition dialog box appears.

2. Select a surface Boundary. 3. Select the surface to be Extrapolated. 4. Specify the Limit of the extrapolation by either: • • • entering the value of the extrapolation length selecting a limit surface or plane using the manipulators in the geometry.

5. Specify the Continuity type: • Tangent • Curvature

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geometry

Tangent

Curvature

The following options are not available with the Curvature continuity type: Up to element, Extremit Internal Edges. 6. Specify Extremities conditions between the extrapolated surface and the support surface.

• Tangent: the extrapolation sides are tangent to the edges adjacent to the surface boundary • Normal: the extrapolation sides are normal to the original surface boundary.

Tangent 7. Specify the Propagation type:

Normal

• Tangency continuity to propagate the extrapolation to the boundary's adjacent edges. • Point continuity to propagate the extrapolation around all the boundary's vertices.

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What's New

Tangent continuit y 8. Click OK to create the extrapolated surface.

Point continuity

The surface (identified as Extrapol.xxx) is added to the specification tree.

•

Check the Constant distance optimization option to perform an extrapolation with a constan and create a surface without deformation.

This option is not available when the Extend extrapolated edges option is checked. Open the Extrapolate4.CATPart document. 1. 2. 3. 4. Select Boundary.1 as the Boundary and Surface.1 as the surface to be Extrapolated. Set a Length of 10mm. Check the Constant distance optimization option. Click OK to create the extrapolated surface.

Constant distance optimization option checked •

Constant distance optimization option unchecked

The Internal Edges option enables to determine a privileged direction for the extrapolation. select one or more edges (in the following example we selected the edge of Surface.1) that extrapolated in tangency. You can also select a vertex once you have selected an edge in or an orientation to the extrapolation.

You can only select edges in contact with the boundary.

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geometry

One edge selected

Two edges selected

The Internal Edge option is not available with the Wireframe and Surface product. • •

Check the Assemble result option if you want the extrapolated surface to be assembled to t surface.

Check the Extend extrapolated edges to reconnect the features based on elements of the ex surface. This option is especially useful if you work within an ordered geometrical set environment. Open the Extrapolate3.CATPart document.

1. Set Extrude.1 as the current object. 2. Select the boundary of Extrude.1 and Extrapol.1 as the surface to be extrapolated. Extrude.3 is automatically rerouted, as well as all edges based on Extrude.1.

This option is only available when both Continuity and Extremity types are specified as Tangent, an the Assemble result option is checked. It is not available when the Constant distance optimization option is checked.

Extrapolating Curves
This task shows you how to extrapolate a curve. Open the Extrapolate2.CATPart document.

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•

Click the Extrapolate icon

.

The Extrapolate Definition dialog box appears.

• • •

Select an endpoint on a curve. Select the curve to be Extrapolated (it can be a wire, an edge, a curve or a line) Select the extrapolation type: 2. Length: enter the value in the Length field or use the manipulators in the 3D geometry. In Curvature mode, this length actually is the distance on the tangent extrapolation at which a plane normal to the curve is located. This plane is used to split the extrapolated curve. 4. Up to: the Up to field is enabled. Select a curve belonging to the same support as the curve to be extrapolated (surface or plane).

Extrapolating a curve Up to a non wire element is not possible if the element is a plane with a curv continuity and without support. 5. Specify Continuity conditions: 1. Tangent: the extrapolation side is tangent to the curve at the selected endpoint. 2. Curvature: the extrapolation side complies with the curvature of the selected curve. This option is not available with the Up to type with a support.

Length extrapolation in Tangent mode

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Length extrapolation in Curvature mode

Up to extrapolation in Tangent mode

If needed and if the initial curve lies on a plane or surface, you can select this support. In this case extrapolated curve lies on the surface too, and is relimited by the support boundary.

Extrapolation without support 6. Click OK to create the extrapolated curve.

Extrapolation with a support

The curve (identified as Extrapol.xxx) is added to the specification tree.

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Editing Surfaces and Wireframe Geometry
Editing Surfaces and Wireframe Geometry
Generative Shape Design provides powerful tools for editing surfaces and wireframe geometry. Edit definitions: double-click on the element in the tree and modify its parameters Replace elements: select the element to be replaced, choose the Replace... contextual command, then select the replacing element. Create elements from an external file: key in space coordinates of elements into an Excel file containing macros, then run the macro. Select implicit elements: press and hold the Shift key while clicking the element to which the implicit element belongs. Manage the orientation of geometry: double-click a line or a plane in the specification tree, and change the Angle value. Delete geometry: select the element, choose the Delete command, set the deletion options Deactivate elements: select the element to be deactivated, choose the Deactivate contextual menu and choose to deactivate its children as well, if needed. Isolate geometric elements: select the element to be isolated, choose the xxx object -> Isolate contextual menu. Edit parameters: click Preview while creating the element, or, if the element is already created, select it and choose the xxx object -> Edit Parameters contextual menu. Upgrade features: select the elements to be upgraded, choose the xxx object -> Upgrade contextual menu.

Replacing Elements

This task shows how to replace a geometric element by another. This may be useful when a modification occurs late in the design as the whole geometry based onto the element that is replaced is updated according to the new specifications coming from the replacing elements. Open the Replace1.CATPart document. 8. Right-click the pink curve (Profile.1) and choose the Replace contextual menu. The Replace dialog box appears.

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9. Click the With field and select the blue curve in the geometry. The Replace dialog box is updated accordingly and the geometry displays the curves orientation.

You can check the Delete replaced elements and exclusive parents if you do not need these elements for later operations. A warning message is issued if the element to replace is a published element.

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What's New 10. Click Yes to replace the published element 11. Click No to cancel the operation and close the Replace dialog box. In our example, we published Profile 1.

11. Click OK to validate the replacement. The geometry is updated accordingly.

12. You cannot replace elements that are not updated. 13. You cannot replace solid elements such as pads for instance. 14. You can only replace a body that is pointed by an Add feature (Boolean Operation). Refer to Adding Bodies in the Part Design User's Guide.

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