Copyright DASSAULT SYSTEMES FreeStyle Shaper, Optimizer & Profiler CATIA Training Foils Version 5 Release 8 February 2002 EDU-CAT-E-FSS-FF-V5R8 Illustration of the course

Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn how to create style design surfaces, analyze their quality and modify them. You will discover two possible approaches: the surface based approach and the curve based approach. Targeted audience Surface Designers Prerequisites Fundamentals about CatiaV5 0.5 days

Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to FreeStyle p.4 Workbench Presentationp.5 2. Fundamentals of FreeStyle p.13 Surface Based approachp.14 Curve Based Approachp.29

Copyright DASSAULT SYSTEMES Introduction to Freestyle You will become familiar with … User interface Terminology General Process

Copyright DASSAULT SYSTEMES Workbench Presentation (1/8) In this lesson, you will learn about the FreeStyle workbench by Accessing the workbench Exploring the User Interface Compass Visualization tools The FreeStyle Dashboard

Copyright DASSAULT SYSTEMES Workbench Presentation (2/8) Accessing the Workbench At any time, the current workbench is indicated by an icon on the right hand Tool Bar.

Copyright DASSAULT SYSTEMES Workbench Presentation (3/8) Free Style tools... Part tree Standard tools Features... Compass Dashboard The User Interface:

Copyright DASSAULT SYSTEMES Workbench Presentation (4/8) The User Interface: FreeStyle tools

Copyright DASSAULT SYSTEMES The compass A tool bar is available by hitting F5 key In this toolbar you have the choice of the main plane/direction Activate the,main plane that is the most visible on your viewing position - Use a plane or 3 points to define a plane/direction Reset the compass in xyz mode Switch the compass from not linked to linked to the entity When linked to an entity, create the compass plane for later use Hitting F5 several times and you will switch from x0y to y0z to z0x The compass also has an associated popup The compass is used to: 1- Select a plane/direction to perform an action 2- Display according to a main plane 3- Apply a transformation to one or several entities. Position the compass : You may Drag and Drop your compass to: A curve: you will define the plane normal to the curve A surface you will define the plane tangent to the surface where you dropped the compass The compass is then switched from x,y,z to a u,v,w trihedron Then hitting F5 you will flip from u,v to v,w then w,x plane definition Workbench Presentation (5/8)

Copyright DASSAULT SYSTEMES Just click on the x, y or z letter to display corresponding, y0z, z0x and x0y view A second click on the same letter invert the direction of viewing Pan the display click+hold on x,y or z axis and moving the mouse Rotate the display by click+hold on the arcs of circle and moving the mouse Display according to a main plane : Link the compass to an entity and then use the axes/rotation circles from the compass, the entity will physically move in your model You can also manipulate several entities: first position your compass on an entity, then multi-select the entities to be moved and act on the compass To reset the compass drag and drop it on the asbolute xyz axis (bottom right of the screen) Apply a transformation to one or several entities : Z translation Y rotation X rotation Y translation X translation Z rotation The compass is used to: 1- Select a plane/direction to perform an action 2- Display according to a main plane 3- Apply a transformation to one or several entities. Each time you find the following icon: Or use it to project control points within Control Point menu Once a plane/direction is selected You may use this plane/direction definition in relevant action : Workbench Presentation (6/8) The compass

Copyright DASSAULT SYSTEMES Visualization tools FreeStyle Visualization Options are sometime very useful to display some characteristics of entities To do this use the Tools / Visualization Option menu The 2 menus are also available in the bottom tool bar Select the entities to process Click on the Remove Visualization menu Remove the visualization options : This dialog box is used to define what will be displayed using option Apply You may display the control Points of the entities or its segmentation and change the symbol used for points. Select the entities to process Apply dress up : Geometric information Select an entity Click on Geometric information Information such as entity type and order are displayed in a box Click on the icon again to exit the function Workbench Presentation (7/8)

Copyright DASSAULT SYSTEMES FreeStyle Dashboard The FreeStyle dashboard groups options that are common to several functions Create Datum: When the option is ON, the result of the current action is a datum, not a feature. It has no link with its parent entities, it cannot be updated when its parents are modified. Click the button to activate the option, Click again to cancel it, Double-click the button to make the option permanent. Applies to 3D Curve, Styling Sweep, Net Surface. Keep original: When the option is activated, the input entity is not deleted when the new one is created. Applies to Offset, Project Curve, Break, Untrim, Fragmentation, Disassemble… Snap: These options activate the automatic detection of vertices, edges, control points and segments for snapping. Applies to Control Points, Match, Global Deformation, Planar Patch, 3D Curve… Attenuation: These buttons allow a quick setting of the attenuation, I.e. the parameter that defines the speed of the movements controlled by the mouse. Applies to Control Points, Match, Offset, Blend, 3D curve … Continuity: When the option is ON, continuities of the current element are displayed and can be frozen. Applies to Control Points, Match, Blend, Fill … Contact Points: When the option is ON, contact points are displayed and can be moved by dragging or assigned a precise location. Applies to Match, Blend, Styling Sweep, Curve on Surface, Styling Corner… Tensions: When the option is ON, tangent and curvature tensions of the entity being created can be displayed and changed manually. Applies to Match, Blend… U,V orders: When the option is ON, the order of the element being created is displayed and can be changed. Applies to Control Points, Match, Fit … Furtive display: When the option is ON, the control points of the entity being created are displayed. Applies to Blend, 3D Curve, … Workbench Presentation (8/8)

Copyright DASSAULT SYSTEMES Fundamentals on FreeStyle You will become familiar with … Surface Based Approach -intuitive to those who are used to manipulating shapes by their control points -intended to serve user sensibility and creativity Curve Based Approach -fits the needs of those who can control shapes through minimal mathematical concepts -allows associativity for easy shape modification

Copyright DASSAULT SYSTEMES Surface Based Approach In this lesson you will learn how to create surfaces using control points Creating Simple surfaces Creating Surfaces by extrusion Modifying Surfaces by their control points Matching surfaces Blending curves and surfaces Creating curves on surfaces Breaking curves and surfaces Analyzing quality Creating offset surfaces Deforming surfaces

Copyright DASSAULT SYSTEMES Planar Patch: you can create a planar patch by selecting two points which define the diagonal of a rectangle. Simple surfaces: you usually use one of these 4 functions to create the basic surfaces that you will after shape by their control points The selected points can be existing points such as curve or patch vertices. You can also pick a point in space, the selected point will then be the projection of the pick to the current privileged plane defined by the compass. 3-Points Patch: you create a rectangular patch by selecting 2 points which define the length and a third one which defines the width. Creating simple patches The rules for the selection of points are the same as for Planar Patch. Geometry extraction: you extract a rectangular area of a patch by selecting 2 points which define the diagonal of the rectangle. The sides will be taken as parallel to U and V directions of the support patch. The selected points must be on the same surface. 4-Points Patch: you can create a patch by selecting four points which define the four corners of the patch. The selected points must be existing points such as curve or patch vertices. You cannot pick a point in space.

Copyright DASSAULT SYSTEMES Extrude Surface This function will allow you to create a surface by dragging a curve in a given direction Just select any kind of curve: a planar curve, 3D curve, a curve on surface or a surface edge and activate Extrude Surface Normal to the plane of the curve Following the normal of the Compass The extrusion direction is : Directly input via keyboard Using the mouse, you may drag the outside boundary to the desired location. combining with Snap on vertex option (dashboard option) is very convenient to stop the extension. The extrusion length is : Plain line shows a segment limit Dashed line shows the order of your segment Temporary display of the resulting surface : Creating Surfaces by Extrusion

Copyright DASSAULT SYSTEMES in the privileged plane (change the privileged plane if necessary), perpendicular to the privileged plane, along directions defined by the segments connecting the control points, parallel to the tangent direction of the curve at the considered point, parallel to the normal direction of the curve at the considered point, in a local plane automatically detected by the system to preserve tangency directions (for example to allow the surface to be tangent to its symmetric). Control Points - To modify a shape by its control points, : 1- select the control points that are free to move (the others remain fixed), 2- choose a direction for moving the control points that you pull, 3- if several control points are free to move, define a deformation distribution law. Choose the possible directions with the icons of the dialog box as follows: The possible directions are shown by green arrows when you bring your cursor close to a control point or a line. You can use the Smooth or Harmonize functions to automatically reorganize the control points and get a more regular polygon. Define a deformation distribution law with the icons of the dialog box as follows: all the selected points are equally moved, the deformation distribution on selected points is linear from the pulled point (maximum deformation) to the last selected point (no deformation), the deformation law is concave, i.e. that the deformation attenuates quickly (local deformation), the deformation law is convex, i.e. that the deformation attenuates slowly (more global deformation), the deformation varies slowly at both ends and quickly in the middle. When you select and drag an arrow, the control point (or the line) becomes the pulled point (or line) and is moved in the direction of the arrow. The other selected points are moved according to the chosen deformation law. Modifying Surfaces by their control points

Copyright DASSAULT SYSTEMES Project end points is used if you match a boundary much smaller than the reference boundary and you want to keep the global dimension of the shape. Project boundary is used to match on a curve lying on a surface (rather than a surface boundary) To update the continuities of a surface relatively to another. Available choices: 1- Point continuity (the surface boundary will be replaced by the new selected one 2- Tangent continuity where the surface (the first selected) will be set tangent to the referenced one (the second selected) at the selected boundary, 3- Curvature as for the previous case we will get a curvature continuous result Select first the boundary you want to adjust, then select the curve you want to match it to. The constraint on the opposite boundary can be displayed (dashboard option) and adjusted Analytic: deformation of the original surface Approximated: A new surface is computed In any case you may let the system decide by switching the Auto mode Match Type could be Analytic or Approximated : The modified surface is automatically computed and displayed Distance, Angles, Curvature through Quick connect Checker Control Points to check/ modify quality of the resulting surface Display : Match type Order of the result Number of Patches Information on the match surface can be displayed: Contact points (dashboard option) allows to dynamically limit the portion of the border to match using manipulators Adapt Curvature tension Edit local tangent angle through contextual menu you get Target (referenced element), Initial (tangent first surface), or User (input a specific value) Global Tension and local tangent using manipulators (dashboard option): Move on main axis : move the control points according to your compass orientation Diffusion : propagates smoothly the deformation applied to reach the desired continuity to whole the control points, it moves more points but the result is more regular Modifying Surfaces by Match

Copyright DASSAULT SYSTEMES Blend Curves : Use this menu to connect 2 curves together. You manage the continuities with the connected curves: 1- select the first curve to connect 2- select the second curve to connect 3- Switch the continuities according to the expected result (simple, tangent or curvature continuity). Contact Points: You can tune the location of the each blend end point on the original contours by activating this option (dashboard). A manipulator allows you to slide these points on the curves. Continuities: Update the continuity level of the blend curve by switching this option on (dashboard)and then right click on the displayed continuity to select the appropriate level. You may also just click on the continuity to flip to the next level of continuity. Tension: Display tangency tension (dashboard) and adjust it by acting on the manipulators you will change the shape of the blend or use right click on the value to enter a new value Blending curves and surfaces (1/2) Blend curve

Copyright DASSAULT SYSTEMES Basic = Analytic, the result is mono patch Advanced = Approximated, the result may be multi patch Auto: The system optimizes the choice between the 2 previous methods Blend Surfaces: Use this menu to connect 2 surfaces together. You manage the continuities with the surface connected: 1- select the Boundary of the first surface to connect 2- select the boundary of the second surface to connect 3- Switch the continuities according to the expected result (simple, tangent, proportional or curvature continuity). 3 types are available: Project end points is used in case you blend a boundary much smaller than the other and you want to keep the global dimension of the shape Adapt tangency and Curvature tension by acting on the manipulators you will change the resulting shape. Adjusting Tangency and curvature: Contact points allows to dynamically limit the portion of the border to match using manipulators Furtive display (dashboard) gives the characteristics of the resulting surface: -Type of blend -Number of resulting patches Blending Curves and Surfaces (2/2) Blend surface

Copyright DASSAULT SYSTEMES Contact points: will allow you to modify points you entered. -U,V orders: displays the order of the curve you are creating. Very useful to create trimming curves on a surface: 1- Select surface on which the curve will lay 2- Draw your curve Display Two dashboard options are available: Creation Type You have the choice between: Different types of mode As for 3D curves you have 3 modes : - Enter by its control points: more than 6 points you will create mutli-arc curve -Near Points: The result will be a Mono Arc curve smoothed on the points. You may choose the resulting order -Through points: The result will be a spline contour made of (Nb of points-1) curves of order 4 - Point by Point: you will enter a series of points (see Mode) - Isoparameter: You will create an Iso U or Iso V of your patch. Creating Curves on surfaces Curve on surface

Copyright DASSAULT SYSTEMES Relimit: the surface is relimited and the control points of the initial surface are kept. - Approximation / Exact: the surface is not relimited and its limits are redefined. A new surface is created. The maximum order of the new surface can be defined thru a contextual menu To redefine the limits of a surface by splitting it along one or more curves: 1- select surface to be split, 2- Select the curve(s) that will cut the surface in 2, and chose the projection direction if the curve(s) does not lie on the surface. 3- Adjust the symbols to define what you keep and what you remove Depending on the type of curve you create, you can choose one of the following break types in the Break Options dialog box : In case the curve does not cut the surface totally in 2, the curve are extended using a tangent line to split the surface totally Direction: If the curve is not a curve on Surface you need to chose the way you will project the curve onto the surface: - Normal to the Surface - Along the normal of the Compass privilege plane. Keep original option (dashboard) will enable you to keep the original surface Symbols allow you to define : - the side you keep - the side you remove Hint: Use menu Untrim Surface or Curve to restore the complete surface (use Keep original option of dashboard if necessary) Trimming Surfaces Break surface or curve

Copyright DASSAULT SYSTEMES Display either curvature or radius of curvature on curves 1- select the curves to be analyzed 2- Pick menu Curvature analysis Type: choose between Curvature or radius of curvature Option reverse is used to display the spikes on the other side of the contour Curvature graph option will create a separate window of the curvature graph of the curves. You can slide your cursor in this graph to check values at different points of the curve Use Automatic to dynamically scale the display according to your viewing. You may decide to impose the size factor by input of the amplitude. Project on plane decides whether you want the 3D curvature or the curvature of the curve projected in the preference plane (compass) Particular: displays the min and max values Density: Number of displayed curvature values You can slide your cursor on the display to check the value along the contour. Using right click you can also create the highlighted point Curvature display: you can choose comb (the spikes) and/or envelop (curve connecting the extremities of the spikes) Analyzing curves Porcupine curvature analysis

Copyright DASSAULT SYSTEMES Display analysis lines on surfaces, for example: 1- cutting planes 2- reflection lines Analyzing surfaces Cutting planes Reflection lines The cutting planes can be parallel according to the direction defined by the compass, perpendicualr to a curve, anywhere, they are then selected manually one by one. The number of planes is explicitely entered or defined by a step between planes. The section lines can be created as curves through a contextual menu (right-click). The reflection lines are produced by a set of parallel lines reflecting on the surface. The reflection can be computed in screen direction (then the lines are constantly updated when the view direction changes), or according to a fixed eye position (then they do not change when the view direction changes). The position of the lines is defined by the compass. Their number and spacing is entered directly in the dialog box. The line can also be created as curves.

Copyright DASSAULT SYSTEMES A tolerance and then you do not control the order, it will be an information only. or The maximum order of the resulting surface, (Delta U, Delta V) there you will not control the accuracy of the offset, it will be an information only. To create new surface(s) at a given distance from original one(s). The distance can be constant (simple) or variable (variable): 1- select the surface(s) 2- choose type (simple or variable), 3- define the offset distance. Characteristics of the result. You can specify: Offset value: editable (right click) to be modified. Normals: important field to check the coherence of the offset on several patches. You may reverse the offset side by clicking the vector. Order : displays the order in U and V. Tolerance: displays the exact tolerance deviation. Corner (only simple mode): allows to use Snap on geometry to define the offset The following information can be displayed and modified: Variable offset: You will have to define the offset values for each corner If you offset a trimmed surface, the temporary display will be based on the untrimmed surface. However the result will be made on the trimmed surface Parallel surfaces Offset Surface

Copyright DASSAULT SYSTEMES To to deform a set of surfaces in one operation: 1- select the surface to deform 2- choose type (intermediate surface or axis use) and guide (No, 1, or 2 guides) 3- Run and use the displayed Control Points box to perform modifications. Guides: They are used to impose continuities control along 1 or 2 surfaces A pseudo patch is computed : it is a planar patch in the privilege plane bounding the deformed surface. Check this patch and use F5 to adjust it before hitting the RUN option. The Control Point Box is then displayed and acting on the Control Points of the Pseudo Patch you will dynamically deform your surfaces It is a nice way of creating families of models from a reference, also you may try different shape modifications to satisfy to the desired style. Type : intermediate surface Global modification Global deformation

Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on the first master exercise, to learn about: Creating surfaces Modifying surfaces Blending and trimming surfaces Analyzing surfaces Creating offset surfaces Modifying surfaces globally

Copyright DASSAULT SYSTEMES To Sum Up In this course you have seen the surface approach to: create surfaces modify surfaces analyze surfaces

Copyright DASSAULT SYSTEMES Curve Based Approach In this lesson you will learn how to create surfaces based on curves. Creating curves Creating surfaces Using associativity to modify shapes

Copyright DASSAULT SYSTEMES Just select the points to be used as Control Points/ near points/ passing through points. If you select a point in space, its position will be defined by the privileged plane. If you select a point on existing geometry (existing point, vertex, point on curve or on surface…), a constraint will be created between the point and the existing geometry. If the existing geometry is changed, the 3D Curve is updated. If you do not want such a constraint, activate the option Disable geometry detection. 3D Curve: Free form curve in space. This will allow you to create curves by points in space, with or without links to existing elements. 3D Curves are features, they can be edited by double-click and they are updated if their parent entities are modified. Input of Points: If you select too many points (>6), you will create multi-arc elements. At any time you may come back to an already selected point and modify its location Control Points: The result will be a spline contour made of (Nb of points-1) curves of order 4. Through Points: The result will be a Mono Arc curve You may input the order of the resulting curve. Near Points: You can at any time edit a 3D Curve (double-click) and move the input points. You may also use the buttons of the dialog box to: Insert a point: add a new point. Remove a point: suppress a point. Free or constrain a point: create a link between a point and another element (point, curve, surface) or on the contrary free a point so that it becomes independent from its support. Creating Curves

Copyright DASSAULT SYSTEMES Attention: -The contours have to be W&S joined entities or boundaries -There must be a contact between Profile and Spine as well as between Profile and Guide Simple sweep: One contour is moved along one spine Sweep and snap: The profile is rotated or slided around the spine contact point normal plane to keep profile contact with the guide contour Sweep and fit: Is this case a global transformation of the profile is applied to ensure the contact with the guide contour Sweep near profiles: In this case you have several profiles, a first one + one or several reference profile giving the coupling and side conditions (tangency, curvature) on the guide an spine contours. It does not insure that the result will pass through the reference profiles Styling sweeps allow you to generate surfaces by moving a section along one or several curves: 1- First input is the profile to be swept 2- Second input is the Spine contour which you will sweep the profile 3- Third input is the Guide contour used to sweep the profile. You have 4 different kind of sweep: In case the spine is a surface boundary you may also slide the profile on the spine to stay tangent to supporting surface. It is also true on the guide side for Sweep and fit and for sweep near profile Translation: the profile is only translated along the spine contour On contour: the profile is location is computed according to the contour trihedron (T, N, B) Fixed direction: The normal is replaced by the fixed direction. The binormal is then recomputed using the tangent and the fixed direction. This is specially useful to avoid cork screw or waving effects. Moving frame: they are used to impose the way we will position the intermediate profile along the spine: You can check the evolution of your moving frame evolution by dragging the manipulator along the spine Creating Surfaces (1/2) Styling sweeps

Copyright DASSAULT SYSTEMES Net surfaces allow you to generate on two sets of curves 1- curves of the first set are used as guides 2- curves of the second set are used as profiles 3- continuity constraints can be given on sides to connect with existing surfaces. The first selected guide is taken as dominant and marked guide(d) on screen: this curve will impose its U parameterization to the resulting net surface. The other guides are re- approximated to follow the same parameterization as the dominant guide. The net surface will not go exactly through the non-dominant guide. The dominant guide can be changed by selecting another guide curve (with CTRL key). Ant time an outside guide or profile is lying on a curve, a continuity constraints can be selected to ensure continuities in point, tangency or curvature with the support surfaces. The level of continuity is changed via the labels displayed when the corresponding option is active in the dashboard. Creating Surfaces (2/2) Net surfaces The first selected profile is taken as dominant and marked profile(d) on screen: this curve will impose its V parameterization to the resulting net surface. The other guides are re-approximated to follow the same parameterization. The profiles do not need to intersect the guides exactly. They are re- approximated to make them intersect if necessary The net surface does not go exactly through the profiles, even the dominant one. The dominant profile ban be changed by selecting another profile curve (with CTRL key).

Copyright DASSAULT SYSTEMES Exercise Presentation And now practice on the second master exercise, to learn about: Creating curves Creating surfaces by FreeStyle Sweeps Creating surfaces by FreeStyle Nets Modifying the surfaces by modifying the input curves

Copyright DASSAULT SYSTEMES To Sum Up In this course you have seen : Creating associative curves Creating associative surfaces Modifying surfaces with associativity