Copyright DASSAULT SYSTEMES Generative Shape Design CATIA Training Foils Version 5 Release 8 January 2002 EDU-CAT-E-GSD-FF-V5R8
Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course This course covers tools for surface design included in the Generative Shape Design Workbench that are not present in the Wireframe and Surface Design Workbench. At the end of the course, the student will be able to model complex fillets and analyze surface quality. Targeted audience Mechanical Designers Prerequisites Wireframe and Surface Design 1 day
Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to Generative Shape Designp.6 2. Creating Wireframe Geometryp.12 Creating an Extremump.13 Creating a Polar Extremump.21 Creating a Reflect Line Methodology p.29 Creating a Spinep.39 Creating a Parallel Curve onto a Support within GSDp. Extracting Multiple Edges from a Sketchp. Tools for Wireframe Geometry Creationp. 3. Creating Surfacesp.67 Creating Swept Surfacesp.68 Creating an Adaptative Swept Surfacep.72
Copyright DASSAULT SYSTEMES Table of Contents 4. Performing Operationsp.67 Joining Elementsp. Healing Elementsp. Smoothing Curvesp. Extracting Elementsp. Federating Elementsp. Creating Filletsp. Inverting Orientationp. Creating Lawsp. 5. Using Analysis Toolsp. 6. Managing Features and Open Bodiesp. 7. Hybrid Design (Working with Hybrid Parts) p.
Copyright DASSAULT SYSTEMES Generative Shape Design Workbench Generative Shape Design Interface Generative Shape Design Terminology 1 hour In this lesson you will see V5 Generative Shape Design user interface and basic functions Introduction to Generative Shape Design
Copyright DASSAULT SYSTEMES From the MENUBAR Start/Shape/Generative Shape Design Accessing the Workbench 1 2 By clicking on the current Workbench icon (top right) to access the Favourite Workbenches window.
Copyright DASSAULT SYSTEMES Shape Design tools... Sketcher access... Part Tree Standard tools All Non-Solids (i.e. Points, Curves, Surfaces) grouped under Open Body User Interface: Generative Shape Design General Presentation
Copyright DASSAULT SYSTEMES User Interface: Generative Shape Design (1/2)
Copyright DASSAULT SYSTEMES User Interface: Generative Shape Design (2/2)
Copyright DASSAULT SYSTEMES The PartBody is the default Body for a Part where Solids are stored The Open Body is where non-solids (points, curves, surfaces) are stored Terminology A Part is a combination of one or more Bodies and Open Bodies Wireframe features Surface features Group :Set of surfacic features
Copyright DASSAULT SYSTEMES From Assembly > create a new part (Top-down approach) or Create a new part > insert in assembly (Bottom-up approach) General Process Go into the Sketcher to create the planar Wireframe Geometry Create Surfaces on the Wireframe Use GSD to create all required 3D Wireframe Geometry Optional : Join Multiple Surfaces then Offset a solid Use GSD to create Planes in 3D to support 2D Wireframe geometry
Copyright DASSAULT SYSTEMES Creating Wireframe Geometry In this lesson, you will learn how to create all types of Wireframe elements.
Copyright DASSAULT SYSTEMES WFS Wireframe versus GSD Wireframe Wireframe & Surface Design and Generative Shape Design are two workbenches which have many common functionalities. Within GSD you will discover new functionalities that are not in WFS and also advanced capabilities in some functions that exist in both workbenches. Functionalities specific to the Generative Shape Design workbench. WFS GSD Functionality common to both workbenches but with more capabilities within GSD.
Copyright DASSAULT SYSTEMES Review of WFS Wireframe Geometry You can review the tools covered in the Wireframe & Surface Design Course which are also included in the Generative Shape Design Workbench. Creating Points in 3D Creating Lines in 3D Creating Planes in 3D Creating Curves in 3D
Copyright DASSAULT SYSTEMES In this Skillet you learn what is an Extremum and how to create it. Creating an Extremum
Copyright DASSAULT SYSTEMES Why Create an Extremum? In order to help CATIA find the maximum or minimum point of a curve or surface along any direction chosen by the user. Maximum Extremum on a Curve along the Z Axis Minimum Extremum on a Surface along the X Axis The element might be a sketch, a 3D curve or line, a surface or a solid face. Maximum Extremum on a solid face along the Z Axis
Copyright DASSAULT SYSTEMES Select the Extremum Icon. Creating an Extremum 5 Select the element on which to find the Extremum. 3 Click OK to confirm. The Extremum is added to the specification tree Select a line or a plane (normal direction) to specify the direction to evaluate the Extremum Select Max or Min according to your requirement. 4
Copyright DASSAULT SYSTEMES Additional Information on Extremum If the element is a surface, you may specify two others optional directions. If the Element is a surface, according to the chosen direction you can obtain a curve or a line as Extremum.
Copyright DASSAULT SYSTEMES In this Skillet you learn what is a Polar Extremum and how to create it. Creating a Polar Extremum
Copyright DASSAULT SYSTEMES What is a Polar Extremum? Any planar curve can be defined with its polar equation (relation linking the radius and the angle). The polar extremum function allows you to find the points on the curve corresponding to : The minimum radius from a specified origin : The maximum radius from a specified origin : The minimum angle regarding to a specified direction : The maximum angle regarding to a specified direction : The polar extremum is calculated in an axis system defined by : - An origin. - A reference direction.
Copyright DASSAULT SYSTEMES Creating a Polar Extremum 1 Select the Polar Extremum Icon. 2 Select the type of polar extremum you want to create. 3 Select the planar contour on which you want to create the polar extremum and its supporting plane. 4 Select the origin point from the polar extremum will be calculated. 5 Define the reference axis. 6 Click OK to confirm the polar extremum creation.
Copyright DASSAULT SYSTEMES Creating a Reflect Line Methodology You will learn what is a Reflect Line and how create it.
Copyright DASSAULT SYSTEMES What is a Reflect Line Reflect lines are curves for which the normal to the support surface in each point presents the same angle with a specified direction. It is very useful to find the parting plane of a complex surface. If we perform a Draft analysis on this part, we can see, thanks to the red areas that the part is non extractible. Thanks to the Reflect Line curve, we can cut the part in two extractible parts.
Copyright DASSAULT SYSTEMES Select a support surface and a direction. Creating a Reflect Line 4 Click OK to confirm reflect line creation Key in an angle representing the value between the selected direction and the normal to the surface. Support 3 Reflect lines You can define one of the X,Y or Z axis by opening a contextual menu in the Direction field. Direction
Copyright DASSAULT SYSTEMES Creating a Spine You will learn what is a Spine and how create it.
Copyright DASSAULT SYSTEMES What is a Spine ? Profile Guide Curve In this Swept surface, the Spine is, by default, the guide curve. Each section of the swept surface is perpendicular to this Guide Curve Swept sections are perpendicular to the guide curve The swept sections may be oriented by another Spine (not the default one). For instance you want to get the swept sections perpendicular to the green spine: Spine Swept sections are perpendicular to the Spine. For the Swept and Lofted surface, there is a default spine (the guide or a computation from the guides). If you want to fix an orientation for your surface sections you will have to define a Spine. The Spine icon will allow you to create a curve that will be use later as a spine There are two ways to build a spine : Curve normal to a list of ordered planes or planar curves Spine curve computed from several guide curves
Copyright DASSAULT SYSTEMES Select the Spine Icon. Creating a Spine from planes and planar curves Successively select planes or planar profiles. 3 Click OK to confirm. The Spine is added to the specification tree. You can also select a start point. The point is projected onto the first plane as the spine starting point. Use these three buttons to replace, delete or add a plane or a profile.
Copyright DASSAULT SYSTEMES Select the Spine Icon. Creating a Spine from Guide Curves Click in the field Guide 3 Click OK to confirm. The Spine is added to the specification tree. Use these three buttons to replace, delete or add a plane or a profile. Select the Guide Curves 4 Sweep using the default spine (guide curve 1) Sweep using the user created spine
Copyright DASSAULT SYSTEMES Creating a Parallel Curve onto a Support Within GSD You will learn how create various parallel curves.
Copyright DASSAULT SYSTEMES Creating a Curve Parallel to another on a Support (1/3) 2 Choose the parallelism type : Geodesic : The distance between the curves will be calculated taking the support curvature into account. Reference curve Euclidean Parallel Curve Geodesic parallel curve Support Euclidean : The distance between both curves will be calculated without taking in account the support curvature. Reference curve Parallel Curve Geodesic Euclidean
Copyright DASSAULT SYSTEMES Creating a Curve Parallel to another on a Support (2/3) Select the reference curve and the support plane or surface. Click OK to continue The created curve is defined as an Object, i.e. the reference for creating the other curves Specify the Offset by entering a value or using the graphic manipulator (green arrows). 4 Reference curve Support If you want to create several parallel curves separated by the same offset check the option Repeat object after OK If you have chosen the euclidean parallel type, you can choose to offset the curve at a constant distance or according to a law. 5 6 Check here to create two parallel curves symmetrically in relation to the reference curve. Select the parallel corner type.
Copyright DASSAULT SYSTEMES Define the number of parallel curves to be created 8 Click OK to confirm parallel curve creation As many parallel curves as indicated in the Object Repetition dialog box are created, including the object parallel curve. The parallel curves are separated from the object line by a multiple of the offset value. The curve instances are grouped in a new Open Body if you have checked the option. Creating a Curve Parallel to another on a Support (3/3) Object parallel curve Parallel curve instances in a new Open Body You can choose to create or not the instances in a new Open Body.
Copyright DASSAULT SYSTEMES Extracting Multiple Edges from a Sketch. You will learn to extract some geometrical elements from a Sketch.
Copyright DASSAULT SYSTEMES Extracting Multiple Edges 2 Select the Extract Multiple Edges icon If you have a sketch containing several elements, you can extract a subpart of these elements to create geometry. Select the geometry of the multi profile sketch that you want to extract 3 Click on OK, the extract is added to the specification tree Click on this button to delete a sub element of the list
Copyright DASSAULT SYSTEMES Tools for Wireframe geometry creation. Stacking Commands Work on Support Now let us look at some Wireframe tools common to the WFS and GSD Workbenches...
Copyright DASSAULT SYSTEMES You will learn how to stack commands while creating wireframe elements. Stacking Commands
Copyright DASSAULT SYSTEMES What about stacking commands ? You can create the following construction elements: - points,- planes, - intersections. - lines,- projections, You have access to the stacking commands capability while creating: - points,- circles,- translations, - lines,- conics- rotations, - planes, - corners, - symmetry. Why Do You Need to Stack Commands ? Stacking commands allows you to create construction elements while creating an element which requires those construction elements. Using mouse button 3 you display a contextual menu listing all the elements you can create using the stacking commands capability.
Copyright DASSAULT SYSTEMES You define the parameters of the construction element. Let s see now the way to stack commands... Stacking Commands… While creating an element you may need a construction element that you will create on the fly. The construction element is created and selected at the same time. When using the stacking command capability you can check the status of the stack in the Running Commands window.
Copyright DASSAULT SYSTEMES Stacking Commands (1/4) Select the type of plane you want to create. When you create some wireframe elements (point, line, plane, circle, corner, conic) or when you perform a translation, a rotation or a symmetry on an object you can create on the fly the missing construction elements, i.e. points, lines, planes, intersections or projections. In the following example you will see how to create a plane from scratch. 3 Using mouse button 3 click in the Point field and select the Create Point option. The Point Definition window is displayed.
Copyright DASSAULT SYSTEMES Stacking Commands (2/4) 4 Define the parameters to create the point. The status of the stacking commands is also displayed in the Running Commands window. 5 Click OK to accept point creation. The Plane Definition window is displayed again with Point.1 in the Point field. The Point button next to the Point field allows you to edit the point parameters. 6 Using mouse button 3 click in the Line field and select the Create Line option. The Line Definition window is displayed.
Copyright DASSAULT SYSTEMES Stacking Commands (3/4) 7 Define the parameters to create the line. The status of the stacking commands is also displayed in the Running Commands window. 8 To create the points needed for the line you can also use the stacking commands. In that case the Running Commands window will look like this:
Copyright DASSAULT SYSTEMES Stacking Commands (4/4) 9 Once the two points are created click OK to accept the line creation. The Plane Definition window is displayed again with Line.1 in the Line field. The Line button next to the Line field allows you to edit the Line parameters. 10 Click OK to accept the plane creation. If you want to modify a parameter of the plane you can also double-click on its identifier in the specification tree. Point.1 Point.2 Point.3 Line.1 Plane.1
Copyright DASSAULT SYSTEMES You will learn how to define a planar or non-planar support, work on it with or without a grid and snap to a point. Working on a Support
Copyright DASSAULT SYSTEMES What about support ? If you define a plane as a support a grid is displayed and positioned in the plane of the screen. In that case you have access to the Snap to Point capability. If you define a surface as a support the elements created after selection of the surface will be located on the surface by default. Why Do You Need to Work on a Support ? You can select a plane or a surface to use it as a support for further element creation. Support plane = YZ With the Snap to Point capability the created points are located at the nearest intersection of the grid. Support surface = Extrude.1 When you create a point after selecting the surface as a support the Point Definition window automatically displays the option On surface.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (1/3) 1 2 Select the plane you want to define as a support, here the YZ plane. The Work on Support window is displayed. A Working support.1 feature is added to the specification tree under the Working supports entry. By default the last created working support (current) is displayed in red in the specification tree. The not current working supports are displayed in blue.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (2/3) The Work on Support window changes and displays several options to define the grid. Define the number of steps in a grid subdivision Selected plane Define the total length of the grid subdivision Check this option if you want a different primary spacing in the second direction Define which axis is taken as H direction in the 2D plane 3 Click OK to confirm grid creation. Set the grid visualization parallel to the screen If you enter coordinates when the Snap to point icon is active, the system does not take the grid into account. 4 If you want your cursor to move directly to an intersection point of the grid click on the Snap to Point icon.
Copyright DASSAULT SYSTEMES Working on a Support – Plane Support (3/3) Here you are creating a point. Note that : - the point type is automatically set to On plane, - the cursor points only on the grid intersection points. Create an element on the support. 5 Exit the working support : 6 Using the Working Supports Activity icon Using the Set as Not Current option in the contextual menu
Copyright DASSAULT SYSTEMES Working on a Support – Surface Support (1/2) 1 2 Select the surface you want to define as a support, here the extruded surface. The Work on Support window is displayed. A Working support.1 feature is added to the specification tree under the Working supports entry. By default the last created working support (current) is displayed in red in the specification tree. The not current working supports are displayed in blue.
Copyright DASSAULT SYSTEMES Working on a Support – Surface Support (2/2) 3 Click OK to confirm grid creation. Here you are creating a point. Note that the point type is automatically set to On surface. Create an element on the support. 4 Exit the working support : 5 Using the Working Supports Activity icon Using the Set as Not Current option in the contextual menu
Copyright DASSAULT SYSTEMES Creating Surfaces In this lesson, you will review all the Surface creation tools that were covered in WFS and that are also available in the GSD Workbench
Copyright DASSAULT SYSTEMES What about surfaces ? You can create a surface from: - a line, curve or sketch - other surfaces You can use basic surfaces either to create a new part or to complete the design of a solid part Surface of revolution created from a profile (Spline) and an axis of revolution Offset surface created from another surface and a direction For each type of surface you will also define its limits or the angle of revolution Why Do You Need Surfaces ?
Copyright DASSAULT SYSTEMES WFS Surfaces versus GSD Surfaces Wireframe & Surface Design and Generative Shape Design are two workbenches which have many common functionalities. Within GSD you will discover new functionalities that are not in WFS and also advanced capabilities in some functions that exist in both workbenches. Functionality specific to the Generative Shape Design workbench. Functionality common to both workbenches but with more capabilities within GSD. WFS GSD
Copyright DASSAULT SYSTEMES Review of WFS Surfaces You can review the tools covered in the Wireframe & Surface Design Course which are also included in the Generative Shape Design Workbench. Creating a Surface from a profile - Creating a Extruded Surface - Creating a Surface of Revolution - Creating a Sphere Creating a Surface from Boundaries - Creating a Fill Surface - Creating a Blend Surface Creating a Surface from another Surface - Creating an Offset Surface Creating a Lofted Surface
Copyright DASSAULT SYSTEMES Explicit Swept Surfaces Implicit Swept Surfaces You will learn how to create Explicit and Implicit Swept Surfaces within the Generative Shape Design Workbench Creating Swept Surfaces
Copyright DASSAULT SYSTEMES You will learn how to create swept surfaces using Any Profile Creating Explicit Type Swept Surfaces
Copyright DASSAULT SYSTEMES Confirm swept surface creation Creating an Explicit-type Swept Surface (1/7) Select the guide curve and the profile. You can then choose to give a reference plane or surface (Reference tab) or to select another guide curve and anchor points (Second Guide tab). If no spine is selected the guide curve is used as spine. Select the Sweep Surface icon. By default, the swept profile is constant in each section along the guide curve.
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (2/7) You can define a reference surface to control the position of the profile along the sweep. Using a reference surface : You can define a law to drive the angle evolution between the profile and the reference surface
Copyright DASSAULT SYSTEMES Using positioning and a reference surface : The guide curve axis system is now oriented regarding the reference surface orientation : Using positioning : The profile is oriented in the guide curve axis system. Using no positioning : When the profile position is fixed with respect to the guide curve, the sweep lies on the profile and on the guide curve (if it intersects the profile) or on the parallel to the guide curve crossing the profile (minimum distance). Creating an Explicit-type Swept Surface (3/7) You can position the profile with the guide curve. Using the Position profile mode, the reference is no more the profile but the Guide Curve. Green axis-system : current profile orientation Grey axis-system : profile reference axis Position Profile
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (4/7) In the Position profile mode you can display parameters to modify the position of the sweep profile on the guide curve defining a new origin and a rotation angle or direction. These coordinates (or the selected point) define the position of the origin of the positioning axis system (green) in the first sweep plane. The direction defines the X axis of the positioning axis system. Position Profile : Parameters Or 45 deg You can rotate the positioning axis system around the guide curve with respect to initial axis system of the profile.
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (5/7) In the Position profile mode you can display parameters to modify the position of the sweep profile on the guide curve defining a new origin and a rotation angle or direction. You may want to invert the orientation of the X or Y axes of the positioning axis system. You can select a point defining the origin of the axis system linked to the profile. Position Profile : Parameters
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (6/7) You can select a second guide curve to define the sweep. Second Guide Curve and Anchor Points If you check the Profile extremities inverted option, the profile extremities connected to the guides are inverted. If you check the Vertical orientation inverted option, the vertical orientation of the profile is inverted. If no spine is selected, the first guide curve is the spine : You can create a spine if you want to obtain a more regular surface :
Copyright DASSAULT SYSTEMES Creating an Explicit-type Swept Surface (7/7) Second Guide Curve and Anchor Points You also can use Anchor Points to position the profile on the guide curves. Anchor points Profile Guide curves While creating the swept surface, the anchor points are remaining on the guide curves all the sweep long. So, the profile is positioned regarding to the initial geometrical conditions between the profile and the anchor points.
Copyright DASSAULT SYSTEMES You will learn how to create swept surfaces using Linear Profiles Creating Line Type Swept Surfaces
Copyright DASSAULT SYSTEMES Creating a Line-type Swept Surface : Two Limits Line type : 3 Confirm surface creation Click on the Line icon, then select the Two limits subtype and the two guide curves. If no spine is selected the first guide curve is used as spine. Subtype : Two limits Length 1 Length 2 Guide curve 1 Guide curve 2 You can select the second guide curve as middle curve instead of entering length values (same as Limit and middle subtype)
Copyright DASSAULT SYSTEMES Creating a Line-type Swept Surface : Reference Surface Line type : 3 Confirm surface creation Click on the Line icon, then select the With reference surface subtype, the guide curve and the reference surface. Key in an angle value and define the length of the surface. If no spine is selected the first guide curve is used as spine. Subtype : With reference surface Angle between the sweep and the reference surface. Length 2 Length 1 Guide curve 1 Reference surface Angle
Copyright DASSAULT SYSTEMES Creating a Line-type Swept Surface : Tangency Surface Line type : 3 Confirm surface creation Click on the Line icon, then select the With tangent surface subtype, the guide curve and the tangency surface. If no spine is selected the first guide curve is used as spine. Subtype : With tangency surface Tangency surface Guide curve 1
Copyright DASSAULT SYSTEMES You will learn how to create swept surfaces using Circular Profiles Creating Circle Type Swept Surfaces
Copyright DASSAULT SYSTEMES Creating a Circle-type Swept Surface : Two Guides and Radius Circle type : 3 Confirm surface creation Click on the Circle icon, then select the Two guides and radius subtype, the two guide curves and the radius. If no spine is selected the first guide curve is used as spine. Subtype : Two guides and radius Radius In case of several solutions you can check them all and then select one of them (green color = active solution)
Copyright DASSAULT SYSTEMES Creating a Circle-type Swept Surface : Center and Radius Circle type : 3 Confirm surface creation Click on the Circle icon, then select the Center and radius subtype, a center curve and a radius. If no spine is selected the center curve is used as spine. Subtype : Center and radius
Copyright DASSAULT SYSTEMES Click on the Circle icon, then select the one guide and tangency surface as subtype. Select the guide curve, the tangency surface, and key in a radius sufficient to link the guide curve and the tangency surface. Creating a Circle-type Swept Surface : One Guide and Tangency Surface Circle type :Subtype : One Guide and Tangency Surface 1 2 In case of several solutions you can check them all and then select one of them (orange color = active solution)
Copyright DASSAULT SYSTEMES You will learn how to create swept surfaces using Conical Profiles Creating Conical Type Swept Surfaces
Copyright DASSAULT SYSTEMES Creating a Conical-type Swept Surface : Two Guide Curves Conical type : 3 Confirm surface creation Click on the Conic icon, then select Two guide curves and their tangency supports. Define an angle between the swept surface and the tangency surface Subtype : Two Guide curves Set the parameter value (ranges from 0 to 1) indicating the sweep proximity to the spine.
Copyright DASSAULT SYSTEMES Creating a Conical-type Swept Surface : Five Guide Curves Conical type : 3 Confirm surface creation Click on the Conic icon, then select Four guide curves and a tangency support. You can specify a Spine curve. The default spine is always the first guide curve. Subtype : Five Guide curves Five Guide Curves
Copyright DASSAULT SYSTEMES You will learn what is an Adaptative Swept Surface and how create it Creating an Adaptative Swept Surface
Copyright DASSAULT SYSTEMES What is an Adaptative Swept Surface. You can modify the constraints defined in the original sketch independently for each section. Sketch By giving some points, you will define automatically intermediate sections on the spine. This particular sweep uses a Sketch as Implicit profile along a Guiding Curve. The guiding curve is used as the default spine. Guiding Curve The Sketch has been designed in context directly from the dialog box and represent a connex profile
Copyright DASSAULT SYSTEMES What are the differences with the Classic Sweep. In an adaptative sweep, the surface inherits of the sketch constraints. In the Explicit sweep the surface does not inherit of the constraints defined in the sketch. The Implicit sweep is always defined from a sketch. This leads to build a surface that inherits of the sketch constraints scheme on the whole surface. Besides you can create on the fly intermediate sections along the guiding curve and modify the constraints independently in each section. If we analyse the connections between the surfaces, there is a few acceptable tangency discontinuity areas. If we analyse the connections between the surfaces, there are important tangency discontinuities. What does that mean ?
Copyright DASSAULT SYSTEMES Creating an Adaptative Swept Surface (1/3) 2 Select the Adaptative Sweep icon. Select the Guide Curve and the Sketch to be swept. 3 Select predefined points or vertices on the guide curve to add intermediate sections. Sketch Guiding Curve Intermediate sections
Copyright DASSAULT SYSTEMES Creating an Adaptative Swept Surface (2/3) Under the Parameters tab, you can modify the constraints defined in the original sketch for each section independently 75 mm radius 22 mm radius Use this icon to remove a section
Copyright DASSAULT SYSTEMES Creating an Adaptative Swept Surface (3/3) Under the Moving Frame tab, you can replace the spine (the default one is the guiding curve). Click OK to confirm the surface creation 6 The Discretization scroll bar allows you to define the precision of the surface. The step value define the number of virtual intermediate sections used to create the surface. Result with a discretization step = 1.00 Result with a discretization step = 0.50
Copyright DASSAULT SYSTEMES Additional Information on Adaptative Sweep (1/2) If you want to create an adaptative swept surface which lays on other surfaces, you will create your sketch in context because you want to put some associative constraints with the existing geometry. Here we want that the sketch keeps its tangency with the surfaces (the intersection between the surface and the sketch plane) in each section of the sweep. In many cases, you will meet some difficulties to build associative elements from existing geometry. To avoid this problem, it is better to build its sketch directly from the Adaptative sweep dialog box. Open a contextual menu in the Sketch field then choose Edit Sketch.
Copyright DASSAULT SYSTEMES Additional Information on Adaptative Sweep (2/2) The Sketch Creation for Adaptative Sweep dialog box is displayed. You just have to follow the instructions of the prompt bar. Click on OK, the sketch is automatically defined with the construction elements. Associative construction elements
Copyright DASSAULT SYSTEMES In this lesson, you will review WFS tools to transform, to split, and to trim 3D geometrical elements. You will also see additional, powerful tools in GSD for Filleting, Extrapolating, Healing, and inverting the orientation of Surfaces. Review of WFS Operations Joining Surfaces Healing Surfaces Smoothing Curves Extracting Elements Federating Elements Creating Fillets Inverting Orientation Creating Laws Performing Operations on the Geometry
Copyright DASSAULT SYSTEMES WFS Operations versus GSD Operations Wireframe & Surface Design and Generative Shape Design are two workbenches which have many common functionalities. Within GSD you will discover new functionalities that are not in WFS and also advanced capabilities in some functions that exist in both workbenches. Functionalities specific to the Generative Shape Design workbench. WFS GSD
Copyright DASSAULT SYSTEMES Review of WFS Operations You can review the tools covered in the Wireframe & Surface Design Course which are also included in the Generative Shape Design Workbench. Restoring Surfaces Disassembling Surfaces Splitting Elements Trimming Elements Transforming Elements - Translating an Element - Rotating an Element - Applying a Symmetry to an Element - Scaling an Element - Creating an Affinity - Performing an Axis-to-Axis transformation Extrapolating Elements Creating Near Elements Creating Patterns
Copyright DASSAULT SYSTEMES You will learn how to join wireframe or surface elements Joining Elements Element 1 Element 2 Join result
Copyright DASSAULT SYSTEMES What about joined elements ? You can create joined elements from: - adjacent curves - adjacent surfaces You can join elements to use two or more elements as a single element in a further operation. Why Joining Elements ? Four adjacent surfaces. Join result Two adjacent splines.
Copyright DASSAULT SYSTEMES Let s see now the way to join elements... How to Join Elements…
Copyright DASSAULT SYSTEMES Select one by one the elements to be joined together. Joining Elements (1/2) 3 Click OK to confirm join operation. To modify the join definition you can edit it and remove elements or replace an element by another. This option checks the connexity between the elements in the resulting join. CATIA will: - reduce the number of resulting elements - ignore the elements that do not allow the join to be created. You can define a merging distance, i.e. the maximum distance below which two elements are considered as only one element. Element 1 Element 2
Copyright DASSAULT SYSTEMES Joining Elements (2/2) While joining elements you can exclude some sub-element from the joined surface. Face to be removed You can also select sub- elements to exclude from the joined surfaces. You can create another join surface with the excluded sub-elements.
Copyright DASSAULT SYSTEMES While joining surfaces, you can specify an angle tolerance. If the angle value on the edge between two elements is greater than the Angle Tolerance value, the elements are not joined Additional Information on Joining Select the elements to be joined. The tangency discontinuity between these surfaces is 6deg : Activate the new option Angle Tolerance. CATIA refuses to create the join surface because the tangency discontinuity between the surfaces is greater than the specified angle tolerance:
Copyright DASSAULT SYSTEMES Healing Surfaces You will learn about the Healing operation
Copyright DASSAULT SYSTEMES Why Healing? While Join is a topological integration of surfaces into one logical surface, HEALING will mathematically deform the shape of surfaces at boundary areas so they smoothly blend into one another. When physical parts are manufactured from CAD models, the machining is guided by the exact representation of the individual surfaces. Hence, Healing is important to ensure that each one of these surfaces transitions smoothly between one another.
Copyright DASSAULT SYSTEMES Healing Surfaces (1/3) 3 Choose if you want to heal the point discontinuities or the tangency discontinuities. Select the Join where you know there is a gap that you would like to Heal. You can also select directly the surfaces to heal.
Copyright DASSAULT SYSTEMES Healing Surfaces (2/3) : Parameters The objective of the parameters is to choose the discontinuities you want to heal or not : 4 Key in parameters : Note : a quick violation analysis can help to choose these parameters : HealedNot healed Merging distance HealedNot healed Tangency angle Not healedHealed Distance Objective Not healedHealed Tangency Objective Gap value Tangency discontinuity value These parameters are thresholds that allows you to: - define the discontinuities to be healed (Merging distance and Tangency angle). - define the discontinuities you consider it is not necessary to heal (Distance Objective and Tangency Objective).
Copyright DASSAULT SYSTEMES Healing Surfaces (3/3) 5 Click OK to confirm the healed surface creation. Note : a quick violation analysis now shows :
Copyright DASSAULT SYSTEMES Smoothing Curves In this Skillet you will learn how smoothing curves.
Copyright DASSAULT SYSTEMES We want to create a Line-type sweep from this curve using the plane as reference surface. Why Smoothing Curves Sometimes when you want create a sweep for instance, CATIA answers you that the profile curve is not continue in tangency and that it could not build the geometry as you whish. The Smoothing Curve function allows you to clean these curves in distance and tangency. We need to smooth the curve before generating the sweep. We can see the discontinuity points and their values to correct the curve. Using the smoothed curve, we can create the swept surface.
Copyright DASSAULT SYSTEMES Select the curve to be smoothed. Smoothing Curves (1/2) 3 Using the displayed values, set the tangency and curvature thresholds up to the value you want to repair. Select the Smoothing Curve icon. A discontinuity analysis is displayed : - In area : discontinuity type and value before smoothing. - Out area : discontinuity status after smoothing. 4 Click on OK to create the smoothed curve
Copyright DASSAULT SYSTEMES Smoothing Curves (2/2) Click OK to create the smoothed curve : it will lie on the surface. 1 2 Select the curve to smooth. 3 Define the smooth parameters. 4 Select the support surface (the curve to smooth must lie on this surface). 5 Smoothing a curve, you have the possibility to select a support surface.
Copyright DASSAULT SYSTEMES Additional Information on Smooth Curve(1/2) Meaning of the boxes colour: The status of the discontinuities is displayed using a colour code. red box A red box means that the discontinuity has not been corrected. Reason : the discontinuity is not within the specified threshold. yellow box A yellow box means that the discontinuity has been partially corrected. Reason : the discontinuity in tangency is within the tangency threshold, but the curvature discontinuity is not within the curvature threshold. green box A green box means that the discontinuity has been completely corrected. Reason : both tangency and curvature discontinuity are within the curvature and tangency threshold.
Copyright DASSAULT SYSTEMES Additional Information on Smooth Curve (2/2) You can choose to visualize only the non-corrected discontinuities : You can choose to visualize the discontinuities interactively, placing the mouse on the discontinuity to make the text box appear : You can also display the information sequentially : The total number of discontinuities is displayed.
Copyright DASSAULT SYSTEMES You will learn how to extract edges and faces from a surface. Extracting Elements Edge extraction Face extraction
Copyright DASSAULT SYSTEMES Select a surface edge and choose the propagation type. Click OK to confirm edge extraction. Extracting an Edge from a Surface Selected edge According to the selected propagation type you get : 1- No propagation3- Point continuity2- Tangent continuity Here there is an ambiguity about the propagation side you are prompted to select a support face. In this case, the dialog box dynamically updates and the Support field is added. You can extract one or several edges of a surface which can be either boundaries or limiting edges of faces. You cannot define limit points. Selected support face
Copyright DASSAULT SYSTEMES Select a face and choose the propagation type. Click OK to confirm face extraction. Extracting a Face from a Surface You can extract one or several faces of a surface with or without propagation. The complementary mode : Switching on this button, you can de-select the elements to extract, and select the non-selected elements :
Copyright DASSAULT SYSTEMES You will learn how to federate elements while joining surfaces and extracting faces Federating Elements
Copyright DASSAULT SYSTEMES Why federate ? (1/2) 1- Surfaces are made of several faces. Elements created from a surface are in fact created from its faces. 2- A modification of the part geometry may lead to a change of the supporting face. The pad has been created with the option Up to surface, using the blue surface. A fillet have been added to the top edge of this pad. This edge depends on a face of the blue surface. The sketch supporting the pad have been modified so that the filleted edge does not lie anymore on the same face
Copyright DASSAULT SYSTEMES Why federate ? (2/2) 3- This change can lead to an update error because the elements created from these faces are no longer recognized. 4- Federating the faces of the surfaces, this kind of update error does not occur anymore. During the update of the part, an update error occurred : the filleted edge is not recognized : To solve the problem, you just have to federate the faces of the blue surface. Then the part is updated without any problem :
Copyright DASSAULT SYSTEMES Lets see now how to federate... How to Federate Elements The federation of elements is available through the Join and the Extract tools :
Copyright DASSAULT SYSTEMES Click OK to create the federated joined surface. 1 2 Select one by one the elements to be joined together. Federating Elements while Joining Surfaces 3 Expand the new Federation panel in the join dialog box. 4 Select one face of the join surface and choose a propagation type. 5 Joining surfaces, you have the possibility to federate the faces of the resulting surface
Copyright DASSAULT SYSTEMES Click OK to create the federated extracted surface. 1 2 Select one face of the solid. Federating Elements while Extracting Faces 3 Choose a propagation type. 4 Activate the federation switch. 5 Extracting faces from a solid, you have the possibility to federate the faces of the resulting surface
Copyright DASSAULT SYSTEMES Creating Fillets Filleting is an operation that is used to smoothly connect surfaces. You will learn how to create Shape, Edge, Variable, Face-To-Face, and Tri- Tangent Fillets
Copyright DASSAULT SYSTEMES Why Fillets? Fillets were originally used in industry to remove sharp edges on parts. More and more, people having been using Fillets as a general modelling tool for surface creation.
Copyright DASSAULT SYSTEMES Select the Shape Fillet Icon Creating a Shape Fillet (1/3) 5 Choose one of the Extremities conditions (Switch between the four types - and Apply - to see the difference) 3 Click OK to confirm. The Shape Fillet is added to the specification tree Select two surfaces and put in the required radius value. Make sure the red arrows point towards the concave side of the fillet. 4 Decide which supporting surface you want to trim. Use these command to create a fillet between two surfaces
Copyright DASSAULT SYSTEMES Creating a Shape Fillet (2/3) : Extremity Type Here are the different types of extremities
Copyright DASSAULT SYSTEMES Creating a Shape Fillet (3/3) : Trimming the supports Four combinations are possible : No support are trimmed Both support are trimmed The second support is left unchanged. Only the first support is trimmed. The first support is left unchanged. Only the second support is trimmed.
Copyright DASSAULT SYSTEMES Select the Edge Fillet Icon Creating an Edge Fillet (1/2) Select one or more internal edges of a surface Use these command to provide a transitional surface along a sharp internal edge of a surface You can control the Extremities of the Fillet the same way as for the Shape Fillet 3 Enter the Radius value. You can also fillet an entire face
Copyright DASSAULT SYSTEMES Creating an Edge Fillet (2/2) Choose a Propagation type : 4 Click OK to confirm. The Edge Fillet is added to the specification tree 5 If Minimal, only the selected edges will be filleted. If Tangency, all edges tangent to the selected edges will also be filleted.
Copyright DASSAULT SYSTEMES Select the Variable Fillet Icon Creating a Variable Fillet (1/3) 3 Select one or more internal edges of a surface 4 You can specify a Zero radius value at limit points of a Variable Fillet Double-Click on any of the shown radius values to change it Select inside this box then select anywhere along the edge to put in an additional radius value along the edge. (You can also create a point on the edge and select this point if accuracy is required) In this type of fillet the radius varies at selected points along a selected edge You can control the Extremities of the Fillet the same way as for the Shape Fillet and the Propagation type the same way as for the Edge Fillet
Copyright DASSAULT SYSTEMES Creating a Variable Fillet (2/3) Choose a radius variation type : Cubic (function ax 3 +bx 2 +cx+d) Click OK to confirm. The Variable Fillet is added to the specification tree 6 5 Linear (function ax+b)
Copyright DASSAULT SYSTEMES Creating a Variable Fillet (3/3) Edge to be filleted You have the capability to create a variable fillet with the fillet sections keeping a constant direction in accordance with a spine The fillet sections are perpendicular to filleted edge The fillet sections are perpendicular to the Spine Spine
Copyright DASSAULT SYSTEMES Select the Face-To-Face Fillet Icon Creating a Face-To-Face Fillet 3 Click OK to confirm. The Face-To-Face Fillet is added to the specification tree Select the two faces (belonging to the same surface) between which you want to create the Face-To- Face Fillet The shape of the Face-To-Face Fillet is basically generated by lying a Cylinder with a specific radius into the gap between two faces. If the radius is too small, the Cylinder will not be able to touch both faces at once. If the radius is two big, we will not be able to achieve a Cylinder tangent to the faces. Put in the desired radius 4 Use the Face-Face fillet command when there is no intersection between the faces or when there are more than two sharp edges between the faces. You can control the Extremities of the Fillet the same way as for the Shape Fillet
Copyright DASSAULT SYSTEMES Select the Tri-Tangent Fillet Icon Creating a Tri-Tangent Fillet 3 Click OK to confirm. The Tri-Tangent Fillet is added to the specification tree. Select the two faces you want to keep The Tri-Tangent Fillet is a variable radius Fillet tangent to all three faces selected. Select the face to be removed. 4 The creation of tri-tangent fillets involves the removal of one of the three selected faces. The three faces must belonging to the same surface.
Copyright DASSAULT SYSTEMES Additional Information on Fillet : Hold Curve and Spine This option concerns with all type of fillet : we will focus on the shape fillet creation. Creating Fillets, you can now choose a curve sketched on one of the support to be connected to control the radius variation. Spine Curve Hold Curve Select a hold curve lying on one support to drive the fillet radius, And a spine curve. Note : the result is a variable radius fillet whose radius is driven by the hold curve.
Copyright DASSAULT SYSTEMES Additional Information on Fillet : Limiting Elements This option concerns the edge, the variable radius, the face-face and the tri-tangent fillets. While creating one of these fillets, you can limit it by selecting an element (plane or surface) that intersects it completely : Edge to fillet Limiting element Edge to fillet Limiting element
Copyright DASSAULT SYSTEMES Additional Information on Fillet : Trim ribbon This option concerns the edge and the variable radius fillets. In some case, fillets may be overlapping. The Trim ribbons option lets you solve this by trimming the fillets where they overlap. Overlapping fillets
Copyright DASSAULT SYSTEMES Additional Information on Fillet : Rolling Edge (1/2) This option concerns the edge and the variable radius fillets. In some case, you may need to indicate that an edge should not be filleted, if a radius is too large for instance. Click on the more button to expand the dialog box, then select the edge you wish to keep.
Copyright DASSAULT SYSTEMES Additional Information on Fillet : Rolling Edge (2/2) You may need that a fillet roll around an edge. You just have to expand the edge fillet dialog box clicking on the more button, then select the edge on which the fillet will roll in the Edge to keep field.
Copyright DASSAULT SYSTEMES Inverting Orientation You will learn how to invert the orientation of Curves and Surfaces Inverting a Curve Inverting a Surface
Copyright DASSAULT SYSTEMES Why Invert Orientation? The results of most surface creation and trimming operations depend on the orientations of the elements involved. Most menu interfaces allow the user to change these orientations on the fly. The Invert Orientation operation exists solely for the users convenience.
Copyright DASSAULT SYSTEMES Access the Invert Orientation from the Menubar - under Insert/Operation How to Invert Orientation 3 Click OK to confirm. The Invert operation is added to the specification tree Select the curve or surface to invert its orientation. The initial display of the red arrow is the already inverted direction. Clicking on the red arrow or on the Reset Initial button displays the initial (uninverted) orientation of the element 4
Copyright DASSAULT SYSTEMES Laws You will learn how to create evolution laws, to be used later on when creating Generative Shape Design elements, such as swept surfaces, or parallel curves.
Copyright DASSAULT SYSTEMES What are Laws? A law is computed as the distance between points on the reference line and their matching points onto the definition curve. d Reference Line Definition Curve The law is defined on the common length between both entities. L The law define the variations of d along L. The interest to define laws is to reuse them in others tools. You can reuse this variable distance only to create parallel curves or sweeps. Instead having a constant distance for a parallel curve you will be able to make vary this distance with a predefined law.
Copyright DASSAULT SYSTEMES Select the Law Icon. Creating Laws Click OK to confirm. The law is added to the Specification Tree. Select the line you want as reference line. Select the line or curve you want as definition curve for the evolution law. 4 When the reference line and definition curve do not present the same length, only the common area is used to compute the law. Create an evolution function from existing geometry. Reference Definition curve 3 Fix a X value or use the manipulators to see the corresponding Y value
Copyright DASSAULT SYSTEMES Additional Information on Laws You can combine the laws created within GSD with laws created with the Knowledge Law Editor Reuse these law combinations in Parallel curves or classic sweeps creation like the other laws. Define the parameter names and types Select the Law icon in the Knowledge toolbar. To reuse the graphic law, check Select Feature then use the Evaluate object as written above.
Copyright DASSAULT SYSTEMES In this lesson, you will learn how to use the Draft, Curvature, and Connection Analysis Tools The Connect Checker The Curve Connect Checker Draft Analysis Curvature Analysis Porcupine Curvature Analysis Using Analysis Tools
Copyright DASSAULT SYSTEMES The Connect Checker You will learn how to use the Connect Checker tool to analyze the connection between surfaces.
Copyright DASSAULT SYSTEMES Why the Connect Checker? For surface modeling, to ensure good transition from one surface to another, the Connect Checker allows the user to examine : the distance (mm) the tangency (deg) the curvature (%) along an edge joining two surfaces. Tangency analysis Curvature analysis Distance analysis
Copyright DASSAULT SYSTEMES Multi-Select the two surfaces between which you would like to check the connection How to use the Connect Checker (1/2) 3 Select the Connect Checker Icon Choose the Analysis Type : distance, tangency or curvature 4 5 Adjust the color ranges taking account your Minimum and Maximum values Choose the type of Display you require. Note the Minimum and Maximum values between the two surfaces.
Copyright DASSAULT SYSTEMES How to use the Connect Checker (2/2) Click OK to confirm. The Connection Analysis is added to the specification tree 7 The number of selected elements and the number of detected connections are displayed. Select the Quick button to obtain a simplified analysis taking into account tolerances (distance, tangency and curvature). Check the analysis result on the geometry. 6
Copyright DASSAULT SYSTEMES The Curve Connect Checker You will learn how to use the Connect Checker tool to analyze the curvature discontinuities on curves.
Copyright DASSAULT SYSTEMES Why the Curve Connect Checker ? For wireframe based surface modeling, it is necessary to use curve that are continuous in tangency and in curvature. The curve connect checker allows you to detect the point, tangency or curvature discontinuities in order to smooth the non-continuous curves : the distance (mm) the tangency (deg) the curvature (%) This curve is discontinuous in tangency. Building a circle sweep on it, you get a surface that is not continuous in tangency.
Copyright DASSAULT SYSTEMES How to use the Curve Connect Checker (1/2) This tool allows you to detect the point, tangency and curvature discontinuities on curves. Distance analysis Tangency analysis Curvature analysis The point discontinuities are displayed on the analysed curve. The curvature discontinuities are displayed on the analysed curve. The tangency discontinuities are displayed on the analysed curve. 1 Select the Curve Connect Checker icon and the curve to analyse. 2 Select the Analyse Type you want to process.
Copyright DASSAULT SYSTEMES How to use the Curve Connect Checker (2/2) This option allows the user to give thresholds bellow which the discontinuity is not detected. If both tangency and curvature discontinuities are detected, only the tangency discontinuity is displayed. Display of the maximum discontinuity values on the curve. 3 Select the Quick Violation Analysis mode by clicking on the Quick button. Click OK to confirm. The Curve Connect Checker Analysis is added to the specification tree : 4
Copyright DASSAULT SYSTEMES Draft Analysis You will learn how to use the Draft Analysis tool to analyze the draft values of surfaces or solids
Copyright DASSAULT SYSTEMES Why analyze Draft? For mold design, Drafts need to be analyzed to determine extractability of the part. For NC Machining, a part is analyzed to look for negative Draft angles in order to determine if a 5-Axis NC machine will be required to cut the part.
Copyright DASSAULT SYSTEMES How to use the Draft Analysis Tool (1/2) 3 Select the customized view render style. Adjust the color range fields - here Red is negative draft, Dark Blue is 0-3 Degrees (probably vertical), Light Blue is 3-15 Degrees, and Green is Degrees Select the surface(s) or solid where you want to examine Draft Select the Draft Analysis Icon. The analysis is displayed on the selected element. 4 The Draft analysis tool gives you at every point the angle between the normal to the surface and the Draft direction which is by default the Z axis.
Copyright DASSAULT SYSTEMES How to use the Draft Analysis Tool (2/2) Click Close when done. The default Draft direction is the Z axis. To modify it drag and drop the compass on a plane or on the surface. 7 Activate the fly analysis checkbox and navigate with the pointer over the surface Arrows are displayed under the pointer. Green arrow is the normal to the surface, red represent draft direction. The displayed value indicates the angle between the draft direction and the normal to the surface at the current point. The part is not extractible Using this draft direction, the part sould be extractible Click on this button to invert the draft direction. You can manipulate the compass, the analysis follows the w axis as draft direction
Copyright DASSAULT SYSTEMES Curvature Analysis You will learn how to use the Mapping Analysis tool to analyze surface curvature
Copyright DASSAULT SYSTEMES Why Curvature Analysis? Curvature analysis of surfaces in generally used to help model high quality surfaces. Abrupt change of curvature on a surface (for example on a car exterior body) can be readily seen by the naked eye and must be smoothed.
Copyright DASSAULT SYSTEMES What is a Curvature Analysis? (1/2) Curvature analysis of surfaces is used to detect the defaults on high quality surfaces. Abrupt change of curvature on a surface can be readily seen by the naked eye and must be smoothed. The curvature analysis measure the curvature on each point of a surface according to the following method : curvature radius in one point (R): represents the local convexity of the surface The curvature in one point (C): C = 1 / R is the inverse of the radius Radius measure of the surface intersection with a cutting plane Curvature measure of the surface intersection with a cutting plane Radius (R) Curvature (C) If radius R curvature C Intersection Plane / Surface
Copyright DASSAULT SYSTEMES What is a Curvature Analysis? (2/2) If we rotate planes around the normal on a point of the surface, we can build the intersection of these planes with the surface. Point on surface Normal On these intersection curves we can measure an infinity of curvature values in this point. In each point we will have a maximum curvature value CM and a minimum curvature value Cm. The Mapping analysis tool allows you to measure these minimum and maximum values, the mean value (Gaussian analysis) and to see the inflection areas. Gaussian : C = CM.Cm MinimumMaximumInflection area
Copyright DASSAULT SYSTEMES Measuring the Mean Curvature on a Surface. 3 Click Close when done Select the Mapping Analysis Icon 4 5 Adjust the color range fields taking into account your observation in Step 3. The objective is to differentiate the various curvature sub-areas of the surfaces Pass the mouse over the surfaces and read the curvature values shown in order to get a general idea of curvature variation on the part Select the surfaces where you want to examine Curvature Select the customized view render style. Select Gaussian as analysis type. Change the color scale to linear
Copyright DASSAULT SYSTEMES Measuring the Minimum or Maximum Curvature on a Surface. 3 Click Close when done Select the Mapping Analysis Icon 4 5 Adjust the color range fields taking into account your observation in Step 3 : drag and drop the arrows or key in directly the right values in the fields. Pass the mouse over the surfaces and read the curvature values shown in order to get a general idea of curvature variation on the part. Select the surfaces where you want to examine Curvature Select the customized view render style. Select Minimum or Maximum as analysis type. Notice that the minimum curvature is always in the perpendicular plane to the maximum curvature.
Copyright DASSAULT SYSTEMES Checking a Surface Using the Limited Radius 3 Click Close when done Select the Mapping Analysis Icon 4 6 Select the surfaces where you want to examine Curvature Select the customized view render style. Select Limited as analysis type. Use the Limited Radius analysis to check if the surface can be offset or to check if tool (an end mill) with a end radius can mill the part. 5 Set the Limited Radius value. In the green area, the defined tool could not mill the part.
Copyright DASSAULT SYSTEMES Checking the Inflection Areas on Surfaces. 3 Click Close when done Select the Mapping Analysis Icon 4 5 Select the surfaces where you want to examine Curvature Select the customized view render style. Select Inflexion Area as analysis type. In the blue areas, the Gaussian curvature (mean) is negative. In the green area, the Gaussian curvature (mean) is positive. Using the Inflection Area analysis type you can check where are the curvature sign changes.
Copyright DASSAULT SYSTEMES The Analysis is calculated on the mesh used to display the object, the precision of the analysis depends upon the display settings. Additional Information on Mapping Analysis (1/2) Fix the 3D Accuracy to the minimum value to have a better analysis rendering.
Copyright DASSAULT SYSTEMES Additional Information on Mapping Analysis (2/2) Case of a multi surface analysis : The analysis is done on each surface apart. The displayed curvature information values are the values of the last selected surface The analysis is done on all the set of surfaces The displayed curvature information values are kept on the set of surfaces Global analysis Multi surfaces analysis
Copyright DASSAULT SYSTEMES Porcupine Curvature Analysis You will learn how to use the Porcupine Curvature Analysis tool to analyze surfaces boundaries curvature
Copyright DASSAULT SYSTEMES Why Porcupine Curvature Analysis? The Porcupine Curvature analysis is an easy curvature discontinuities visualization tool. The boundaries of a surface are impacted by the curvature discontinuities of the surface. The Porcupine Curvature analysis analyses the surfaces boundaries in order to detect the surfaces curvature discontinuities.
Copyright DASSAULT SYSTEMES Using the Porcupine Curvature Analysis (1/4) This tool can be applied on : -A curve. -A surface (boundaries analysis). This tool allows you to detect the curvature discontinuities on curves and to visualize them.
Copyright DASSAULT SYSTEMES Using the Porcupine Curvature Analysis (2/4) Analysis type : Curvature discontinuities displayed with a curvature type analysis. Curvature discontinuities displayed with a radius type analysis. You can choose between a curvature type and a radius type analysis. - Curvature : you visualize the curvature evolution on the curve. - Radius : you visualize the radius evolution along the curve.
Copyright DASSAULT SYSTEMES Using the Porcupine Curvature Analysis (3/4) The diagram : You can choose to visualize the curvature evolution using the diagram: -Each curve analysis posses its own color for a clearer visualization. - The extremum values are displayed in the diagram window. - You can slide the pointer over the diagram to display the amplitude at a given point of the curve.
Copyright DASSAULT SYSTEMES Using the Porcupine Curvature Analysis (4/4) The Porcupine Curvature Analysis visualization parameters : Reverse the curvature values on the analyzed curves. Display all the extremum on the analyzed curves. Fills the analysis area. Envelop the analysis area. Adjusting these parameters, you can optimize the analysis visualization. It has no effect on the curvature values along the curves.
Copyright DASSAULT SYSTEMES In this lesson, you will learn advanced tools for managing Open Bodies in the specification tree. You will also learn how to work in a Hybrid environment and in a Multi-Model environment. Review of miscellaneous WFS tools Manipulating Elements Editing Surface and Wireframe Definition Creating Datum Features Updating a Part Applying Material onto Surfaces Managing the Geometry Using the Historical Graph Quick Edition of Geometry Deleting Useless Elements Auto-Sorting an OpenBody Managing OpenBodies Creating a Group Creating a New OpenBody Changing the Father Node of an OpenBody Selecting Bodies using the Body Selector Duplicating an OpenBody Managing Features and OpenBodies
Copyright DASSAULT SYSTEMES WFS Management Features versus GSD Management Features Wireframe & Surface Design and Generative Shape Design are two workbenches which have many common functionalities. Within GSD you will discover new functionalities that are not in WFS and also advanced capabilities in some functions that exist in both workbenches. Functionalities specific to the Generative Shape Design workbench. WFS GSD
Copyright DASSAULT SYSTEMES Review of WFS Miscellaneous Tools Manipulating Elements Editing Wireframe and Surface Definition Creating Datum Features Updating a Part Managing OpenBodies You can review the tools covered in the Wireframe & Surface Design Course which are also included in the Generative Shape Design Workbench.
Copyright DASSAULT SYSTEMES Managing the Geometry You will learn the following tools to help you manage Open Bodies in the specification tree: Using the Historical Graph Quick Edition of Geometry Deleting Useless Elements Auto-Sorting an OpenBody
Copyright DASSAULT SYSTEMES Using the Historical Graph (1/2) 3 Select the feature from which you want to know the hierarchy. The Historical Graph allows you to display the hierarchical links between the different features of a part. Select the Historical Graph icon. Select the Surface Presentation to display the surfacic hierarchical elements.
Copyright DASSAULT SYSTEMES Using the Historical Graph (2/2) 4a4a Click on plus to expand the tree. to Remove the Graph Select the Parameter Filter button. to Add a Graph Reframe the Graph You can Edit and modify a Parameter directly by double click on it 4b4b Double click a feature to edit and modify it.
Copyright DASSAULT SYSTEMES Quick Edition of Geometry. 1 Select the geometry Select the Quick Edit icon. 2 The Quick Edit allows you to quickly access to the parent elements of the selected object. You identify the generating elements. Informations are displayed on the whole geometry : Green : the last element generated in the selected geometry Red : the direct parent of the last generated element Purple (with G letter) : the first element that generate the final one Compare with the historical graph. You can Edit and modify an element directly by double click on it
Copyright DASSAULT SYSTEMES Deleting Useless Geometry 1 Select Delete useless elements… in the Tools menu. 2 This command allows you to quickly delete all un-referenced datums, that are not participating in the creation of other geometrical elements. CATIA gives you a list of elements to delete and ask you to confirm before delete Click on Yes to confirm.
Copyright DASSAULT SYSTEMES Auto-Sorting OpenBodies 1 Select the OpenBody node in the Specification tree. 2 This command allows you to sort hierarchically the wireframe features under the selected OpenBody. Open a contextual menu, then select Auto-Sort OpenBody. In this specification tree certain features are not in a hierarchical order.
Copyright DASSAULT SYSTEMES Managing Open Bodies You will learn the following tools to help you manage Open Bodies in the specification tree: Creating a Group Creating a new Open Body Changing the Father node of an Open Body Duplicating an Open Body
Copyright DASSAULT SYSTEMES Why Open Body Management Tools? In V5, during the creation and trimming of surfaces, the history of parent surfaces is kept in its entirety in order to allow for automatic update of downstream geometry following a modification of any parent surface. Due to this fact, the specification tree can get large and often confusing. The tools listed below help manage this tree. Creating a Group Hides all the nodes of an Open Body except for specific nodes the user chooses to see. Creating a new Open Body Creates a new Open Body branch in the specification tree with the option of putting nodes from existing Open Bodies into it. (Allows for multiple groups containing related elements) Changing the Father node of an Open Body Allows the user to change the position of an Open Body in the specification tree. Duplicating an Open Body One of the modes of this tool duplicates the Open Body in its entirety. This allows the user to edit nodes in the copied Open Body without affecting the original Open Body.
Copyright DASSAULT SYSTEMES Activate Create Group in the Contextual Menu for the Open Body you would like to group. Creating a Group 3 Click OK to confirm. The Open Body is replaced by a group of hidden nodes + the nodes in the Open Body that the user specified to remain displayed. Name the group. Select nodes in the Open Body that you would like to remain displayed in the specification tree. 4 Hide all the nodes of an OpenBody except for specific nodes the user chooses to show.
Copyright DASSAULT SYSTEMES Activate Expand Group in the Contextual Menu for the Group you would like to open. Expanding and Collapsing a Group 2 Expand the tree under the group node see its contents, and collapse it when it is opened. Activate Collapse Group in the Contextual Menu for the Group you would like to close.
Copyright DASSAULT SYSTEMES Activate Insert/Open Body from the Menubar. Creating a New Open Body 3 Click OK to confirm. The new Open Body is added to the specification tree. Specify the node under which the new Open Body will be inserted. 4 If Part.1 was selected as the Father, the new Open Body will be created under this node Select nodes from existing Open Bodies that you want to move to the new Open Body.
Copyright DASSAULT SYSTEMES Changing the Father Node of an OpenBody or a Feature 3 Click OK to confirm. Select the destination node (new Father node) for your Open Body (or your feature) Activate Change Body in the Contextual Menu for the Open Body (or the feature) you would like to move. The Open Body is moved to its new location.
Copyright DASSAULT SYSTEMES Selecting Bodies using the Body Selector Open the combo box of the Body Selector in the Tools toolbar, then choose the new active body. The body selector allows you to quickly select a specific body to define it in Work Object. 2 You can also rename directly the body in the combo box.
Copyright DASSAULT SYSTEMES Duplicating an Open Body (1/2) Click on the Selected then select the corresponding generating features as shown below Select the Open Body to be duplicated Select the Duplicate OpenBody icon in the Replication toolbar 3 Click on the green arrow to reverse the extrude direction Click on Use identical name to just create an identical second instance of the selected Openbody.
Copyright DASSAULT SYSTEMES Duplicating an Open Body (2/2) Click on OK to confirm the duplication Select As Specified in Part document as format 5
Copyright DASSAULT SYSTEMES In this lesson, you will learn tools to build Hybrid Part using surfacic and solid features. You will also learn how to work in a Multi-Model environment. Working with Hybrid Part. Review of WFS Skillet. Creating a Solid from Surfaces Working in a Multi-Model Environment. Hybrid Design
Copyright DASSAULT SYSTEMES Working with Hybrid Parts You will learn how Surfaces and Solids can be used as modeling tools together within the same model
Copyright DASSAULT SYSTEMES Why Hybrid Modeling? With Hybrid modeling we have the best of both worlds: - the ease of use and concise (inside/outside) mathematical definition of solids - the capability to create complex surfaces In this illustration, the Extrude.1 surface is used to create the ThickSurface.1 solid. Later, the Offset.1 surface was defined from the opposite face of the ThickSurface.1 solid.
Copyright DASSAULT SYSTEMES V5 and Hybrid Modeling Surface to Solid Tools Solid to Surface Tools Access from within the Part Design Workbench In general, solid edges are seen by V5 surfaces as any ordinary curve. Solid faces are seen as any ordinary surface. Hence, surface creation tools can use solid edges and faces as input. Create a surface offset from a solid face Create a Fill Surface from solid edges JOIN solid edges into section curves then LOFT between these section curves Create a Blend Surface between two solid faces Extract a surface from a solid face
Copyright DASSAULT SYSTEMES You will learn how to create a solid from surfaces Creating a Solid from Surfaces
Copyright DASSAULT SYSTEMES What about solids created from surfaces ? You can use a surface to: - split a solid body - create a solid body by thickening the surface - close it into a solid body - sew it onto a solid body You may need to create a surface just for using it in a solid body. The surface is integrated into the body design. Why Do You Need to Create a Solid from Surfaces ? Split Body Thicken Surface Close Surface Sew Surface
Copyright DASSAULT SYSTEMES For each type of feature a dialog box is displayed. 1 Click on any Surface-Based Features icon. 2 Select the surface to be processed. Let s see now the different ways to create surface-based features... 3 Confirm feature creation. Creating a Solid from a Surface …
Copyright DASSAULT SYSTEMES Splitting a Body with a Surface Select the surface used as splitting element and orient the arrow towards the material to be kept. Splitting surface Material to be kept 3 Click OK to split the body.
Copyright DASSAULT SYSTEMES Thickening a Surface Select the surface to be thickened. Surface to be thickened 3 Click OK to thicken the surface. Offset direction
Copyright DASSAULT SYSTEMES Closing a Surface into a Body Select the surface to be closed. Surface to be closed 3 Click OK to close the surface.
Copyright DASSAULT SYSTEMES Sewing a Surface to a Body Select the surface to be sewn onto the body and orient the arrow towards the material to be kept. Surface to be sewn Material to be kept 3 Click OK to sew the surface to the body.
Copyright DASSAULT SYSTEMES Working in a Multi-Model Environment
Copyright DASSAULT SYSTEMES Why Work in a Multi-Model Environment? - To reuse already existing geometry - To establish associativity between parts
Copyright DASSAULT SYSTEMES Surface Modeling and Multi-Model Environment Directly select geometry in the Passive Model to create a surface in the Active Model The passive element selected is shown as an External Reference within the specification tree of the Active Model In this case, the Offset.1 surface has the Surface.1 External Reference as its parent. As usual, changes in the parent will propagate downstream. Select the Offset icon (for instance) 2