Copyright DASSAULT SYSTEMES CATIA Training Foils Part Design Fundamentals Version 5 Release 8 January 2002 EDU-CAT-E-PDG-FF-V5R8

Copyright DASSAULT SYSTEMES Course Presentation Objectives of the course In this course you will learn basic methods to create and modify solids features and parts Targeted audience New CATIA V5 Users Prerequisites CATIA Basics 1 day

Copyright DASSAULT SYSTEMES Table of Contents 1. Introduction to Part Designp.4 2. Sketch Based Featuresp.11 Padsp.12 Pocketsp.27 Shaftsp.37 Limiting Featuresp.51 Holesp.59 3.Dressing-Up Featuresp.70 Draftsp.71 Filletsp.89 Chamferp.108 Drafted Filleted Pads/Pocketsp.117 Threads and Tapsp.129 Patternsp.134 Mirrorp Modifying Partsp.147

Copyright DASSAULT SYSTEMES Introduction to Part Design You will become familiar with CATIA V5 Part design main features

Copyright DASSAULT SYSTEMES The Version 5 Part Design application makes it possible to design precise 3D mechanical parts with an intuitive and flexible user interface, from sketching in an assembly context to iterative detailed design. Version 5 Part Design application will enable you to accommodate design requirements for parts of various complexities, from simple to advanced. This new application, which combines the power of feature-based design with the flexibility of a Boolean approach, offers a highly productive and intuitive design environment with multiple design methodologies, such as post-design and local 3D parameterization. As a scalable product, Part Design can be used in cooperation with other current or future companion products such as Assembly Design and Generative Drafting. The widest application portfolio in the industry is also accessible through interoperability with CATIA Solutions Version 4 to enable support of the full product development process from initial concept to product in operation. What is Part Design?

Copyright DASSAULT SYSTEMES Anywhere from 1- Start menu 2- File / New menu Accessing the Part Design Workbench 1 2

Copyright DASSAULT SYSTEMES CATPart extension Part Design tools... Sketcher access... Part tree Standard tools Features... Part design Interface : General Presentation

Copyright DASSAULT SYSTEMES See Wireframe and Surfaces Insert menu Sketch-based Dress-up Transformations Operations Constraints Part Design Interface

Copyright DASSAULT SYSTEMES A Part is a combination of one or more features, and bodies The first feature is generated from a sketch (profile), by extrusion or revolution Features are components based on sketches (sketch-based) or on existing features (dress-up and transformation). They can also be generated from surfaces (surface-based) A body is a set of features that can be assembled to a part through boolean operations (Assemble, remove,...) Part Design Terminology

Copyright DASSAULT SYSTEMES From Assembly > create a new part (Top-down approach) or Create a new part > insert in assembly (Bottom-up approach) Generate the main pad Create additional features Add dress-up features Modify & reorder features Insert new features or bodies for more complex parts Part Design General Process Sketch the profile of the main pad

Copyright DASSAULT SYSTEMES Sketch Based Features You will learn how to create and limit the most frequently used sketch-based features such as pads, pockets, shaft, and holes Creating Pads Pad: Reverse Side Multi-Pad Creating Pockets Pocket: Reverse Side Multi-Pocket Creating Shafts Shaft: Several Profiles Limiting Features Creating Holes Sketching During Pad, Pocket or Shaft Creation

Copyright DASSAULT SYSTEMES You will learn how to create simple pads from a 2D profile (or sketch) Creating Pads Extruded Pad

Copyright DASSAULT SYSTEMES A pad is a basic solid which is extruded from a 2D profile, called sketch It is one of the first features that can be created when starting a new part Extruded pad What is a Pad ? 2D profile (sketch) Its length can be defined by dimensions (exact values) or with respect to other 3D elements (thus associative). Length Length types

Copyright DASSAULT SYSTEMES Creating Simple Pads... Select the profile Define pads dimensions 2 1 OK to validate 3

Copyright DASSAULT SYSTEMES Select Profile sketch to be used for the Pad The Pad definition can be modified after creation by double clicking on the Pad geometry or product structure Modify Pad definition 3 1 Select Pad icon Creating a Simple Pad 2 You get:

Copyright DASSAULT SYSTEMES Pad : Selection of a Sub-Part of a Sketch (1/2) Select the Pad icon (be sure that no sketch is selected) If necessary, select the Sub-elements option from the appearing dialog box Using the right mouse button (MB3) on the Profile Selection field, select Go to profile definition When creating a Pad, it is possible to select only certain sub-elements of a sketch as the pad profile

Copyright DASSAULT SYSTEMES Pad : Selection of a Sub-Part of a Sketch (2/2) Select one edge of the sub- element you want to extrude 4 When creating a Pad, it is possible to select only certain sub-elements of a sketch as the pad profile 5 Select OK You get: 6 Select OK

Copyright DASSAULT SYSTEMES Multi-length Pad (1/3) Select the Multi-length pad icon The Pad Definition dialog box is displayed. You can see the number of domains to be extruded. You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pad capability lets you do this at one time. 1 2 Select the Sketch. Note that all profiles must be closed and must not intersect. 3

Copyright DASSAULT SYSTEMES Multi-length Pad (2/3) A red arrow is displayed normal to the sketch. It indicates the proposed extrusion direction. To reverse it, you just need to click it. 4 You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pad capability lets you do this at one time. 5 Select a Domain in the list. This one now appears in blue in the geometry area.

Copyright DASSAULT SYSTEMES Multi-length Pad (3/3) Specify the length by entering a value. For example, enter 20mm. Repeat the operation for each extrusion domain. 6 You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pad capability lets you do this at one time. 7 Click OK to create the Multi-height Pad. Note that you can multiselect extrusion domain from the list before defining a common length or thickness.

Copyright DASSAULT SYSTEMES Pad : Reverse Side The Reverse Side button applies for open profiles only. This option lets you choose which side of the profile is to be extruded Select the Pad icon 1 Select the open sketch 2 Modify the Pad length 3 Select the arrow to reverse the pad side (or click the Reverse Side button in the dialog box) 4 Select OK in the dialog box 5 You get:

Copyright DASSAULT SYSTEMES Cavity ArcPad Square & circle Open profiles CATIA allows you to create pads from open profiles provided existing geometry can trim the pads. Example on the right illustrates this concept. Multiple profiles Pads can also be created from sketches including several profiles. These profiles must not intersect. In this example, the sketch to be extruded is defined by a square and a circle. Applying the Pad command on this sketch lets you obtain a cavity Additional Information (1/5)

Copyright DASSAULT SYSTEMES Additional Information (2/5) Adding Sub-elements It is also possible to Add other sub-elements during the profile definition Select Add Select the Sub-element to be added

Copyright DASSAULT SYSTEMES Additional Information (3/5) Removing Sub-Elements It is also possible to Remove other sub-elements during the profile definition Select Remove Select the Sub-element to be removed

Copyright DASSAULT SYSTEMES Additional Information (4/5) Solving ambiguity Capability to solve ambiguity when selecting a sub part of a sketch Select the edge Ambiguity Select the edge to solve the ambiguity You get:

Copyright DASSAULT SYSTEMES Additional Information (5/5) If no sketches have been created when activating the Pad icon, you can access to the sketcher by selecting the Sketcher icon in the dialog box. When you have completed the sketch, you can leave the sketcher then you will return to the Pad creation Select the Sketcher icon in the dialog box then select the sketch plane

Copyright DASSAULT SYSTEMES You will learn how to create simple pockets from a 2D profile (or sketch) Creating Pockets Through PocketBlind Pocket

Copyright DASSAULT SYSTEMES A pocket is removing material from an existing feature, by extruding a 2D profile Pocket What is a Pocket ? 2D profile (sketch) Its length can be defined by dimensions (exact values) or with respect to other 3D elements (thus associative). Length Length types

Copyright DASSAULT SYSTEMES Creating Simple Pockets Select the profile Define pockets dimensions 2 1 OK to validate 3

Copyright DASSAULT SYSTEMES Select Profile sketch to be used for the Pocket Pockets can also be created from sketches including several profiles. These profiles must not intersect Modify Pocket definition 3 1 Select Pocket icon Creating a Simple Pocket 2 You get:

Copyright DASSAULT SYSTEMES Multi-length Pocket (1/3) Select the Multi-length pad icon The Pocket Definition dialog box is displayed. You can see the number of domains to be extruded. You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pocket capability lets you do this at one time. 1 2 Select the Sketch. Note that all profiles must be closed and must not intersect. 3 Note that a red arrow is displayed normal to the sketch. It indicates the proposed extrusion direction. To reverse it, you just need to click it.

Copyright DASSAULT SYSTEMES Multi-length Pocket (2/3) 4 You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pocket capability lets you do this at one time. 5 Select a Domain in the list. This one now appears in blue in the geometry area. Specify the length by entering a value. For example, enter 10mm. Repeat the operation for each extrusion domain. Note that you can multiselect extrusion domain from the list before defining a common length or thickness.

Copyright DASSAULT SYSTEMES Multi-length Pocket (3/3) 6 You can extrud multiple profiles belonging to a same sketch using different length values. The multi-pocket capability lets you do this at one time. Click OK to create the Multi-height Pad.

Copyright DASSAULT SYSTEMES Pocket : Reverse Side The Reverse Side button applies for open profiles only. This option lets you choose which side of the profile is to be extruded Select the Pocket icon 1 Select the open sketch 2 Modify the Pocket Depth 3 Select the arrow to reverse the pocket side (or click the Reverse Side button in the dialog box) 4 Select OK in the dialog box 5 You get:

Copyright DASSAULT SYSTEMES pockets Open profilePocket 8 profiles Open profiles CATIA allows you to create pockets from open profiles if existing geometry can limit the pockets. The example illustrates this concept. Multiple profiles Pockets can also be created from sketches including several profiles. These profiles must not intersect. In the example, the initial sketch is made of eight profiles. Applying the Pocket command on this sketch lets you create eight pockets Can a pocket create material? If your pocket is the first feature of a new body, CATIA creates material. Additional Information (1/2)

Copyright DASSAULT SYSTEMES Additional Information (2/2) If no sketches have been created when activating the Pocket icon, you can access to the sketcher by selecting the Sketcher icon in the dialog box. When you have completed the sketch, you can leave the sketcher then you will return to the Pocket creation Select the Sketcher icon in the dialog box then select the sketch plane

Copyright DASSAULT SYSTEMES You will learn how to create simple Shafts from a 2D profile (or sketch) Creating Shaft Shaft

Copyright DASSAULT SYSTEMES Limits : First angle A shaft is a basic solid which is obtained from the revolution of a 2D profile around an axis The axis and the profile must be created on the same sketch Shaft What is a Shaft ? 2D profile (sketch) This angle is defining the revolution angle of the profile around the axis starting from the profile position and orientated in the clockwise direction Angular Limits Limits : Second angle This angle is defining the revolution angle of the profile around the axis starting from the profile position and orientated in the counterclockwise direction

Copyright DASSAULT SYSTEMES Creating Simple Shafts Select the profile Define the shafts angular limits 2 1 OK to validate 3

Copyright DASSAULT SYSTEMES Select Profile sketch to be used for the Shaft By offsetting the rotation axis off of the profile, a hole can be placed in the resulting part. 1 Select Shaft icon In order to create a shaft, the sketch must contain the rotation axis Creating a Shaft Modify Shaft definition 3 2 You get:

Copyright DASSAULT SYSTEMES Shaft : 3d Line axis Select the Shaft icon 1 2 Select the profile When creating a shaft, it is possible to use a 3d line or a sketched line not included in the sketch of the profile as the rotation axis 3 Select the Axis field in the dialog box 4 Select the 3d line as the rotation axis You can modify the Limits parameters then select OK, you get: 5

Copyright DASSAULT SYSTEMES Shaft Creation: Using a 3d Wireframe as Profile Select the Shaft icon 1 2 Select the following 3d wireframe as the Profile It is possible to select a planar wireframe as the profile when creating a shaft 3 Select the axis selection field 4 Select the following sketch as the axis Select Ok i n the dialog box 5 You get:

Copyright DASSAULT SYSTEMES Shaft : Reverse Side The Reverse Side button applies for open profiles only. This option lets you choose which side of the profile is to be extruded Select the Shaft icon 1 Select the open sketch 2 Modify the Shaft Angles 3 Select the arrow to reverse the shaft side (or click the Reverse Side button in the dialog box) 4 Select OK in the dialog box 5 You get:

Copyright DASSAULT SYSTEMES Shaft with two angular limits : Error Additional Information (1/5) Axis on a profile edge : Axis outside the profile : Axis cutting the profile : Open profile : Open profile and axis outside the profile : Error

Copyright DASSAULT SYSTEMES Additional Information (2/5) It is also possible to use a 3d wireframe as profile when creating a groove, a stiffener, a rib, or a slot

Copyright DASSAULT SYSTEMES Additional Information (3/5) Like for pad or pocket creation, you can use sub-element of a sketch to create a shaft

Copyright DASSAULT SYSTEMES You can create Shafts from sketches including several closed profiles. These profile must not intersect Additional Information (4/5)

Copyright DASSAULT SYSTEMES Additional Information (5/5) If no sketches have been created when activating the Shaft icon, you can access to the sketcher by selecting the Sketcher icon in the dialog box. When you have completed the sketch, you can leave the sketcher then you will return to the Shaft creation Select the Sketcher icon in the dialog box then select the sketch plane

Copyright DASSAULT SYSTEMES You will learn the different ways to limit features Limiting Features Up-to-next LimitUp-to-last Limit

Copyright DASSAULT SYSTEMES You can specify dimensions to limit a feature You can also limit features onto existing elements. In this case, associativity will propagate design changes Why different types of Limits ? Using "Up to Last" to extrude the pad maintains the configuration even with the insertion of a new feature (see example below) Up to Last To capture the design intent

Copyright DASSAULT SYSTEMES Limiting Features... Dimension type: you specify the dimensions (ex: 25 mm) Mirrored Extent: Mirrors the feature about it's profile Up to LastUp to Next Up to Plane Up to Surface Uses a plane or face to limit feature Uses a surface to limit feature Uses the last encountered material to limit feature Uses the next encountered material to limit feature. LIM1 LIM2 Different types of limits

Copyright DASSAULT SYSTEMES Select Profile sketch to be used for the Pad The Up to Last type is also used for defining the limits of Pockets Modify Pad definition to include type Up to last 3 1 Select Pad icon Up to Last Pads/Pockets 2 You get:

Copyright DASSAULT SYSTEMES Select Profile sketch to be used for the Pad The Up to Surface type is also used for defining the limits of Pockets Modify Pad definition to include type Up to Surface 3 1 Select Pad icon Select limit surface on part 4 Up to Surface Pads/Pockets 2 You get:

Copyright DASSAULT SYSTEMES Using Mirrored Extent instead of the Mirror function streamlines your product structure Select Profile sketch to be used for the Pad 1 Select Pad icon 2 Select Mirrored Extent to mirror the Pad about the profile with the specified limit 3 Mirroring a Pad with Mirrored Extent You get:

Copyright DASSAULT SYSTEMES Offset on Pad Limit (1/2) Activate the Pad icon Select the Up to surface from the First Limit Option from the combo Select the Profile When creating a pad using the Up to surface option as one of the pad limit, it is possible to define a positive or negative offset from the selected surface 4 Select the face

Copyright DASSAULT SYSTEMES Offset on Pad Limit (2/2) Enter -25 as the Offset 5 6 Select OK When creating a pad using the Up to surface option as one of the pad limit, it is possible to define a positive or negative offset from the selected surface You get :

Copyright DASSAULT SYSTEMES Whatever hole you choose, you need to specify the limit you want. There is a variety of limits: Up-to-Plane / Surface Limiting Holes & Pockets Up-to-Last Blind / Dimension Up-to-Next When using Up-to-Next option: Special case Additional Information (1/2)

Copyright DASSAULT SYSTEMES Additional Information (2/2) When creating a pad/pocket using the Up to surface option as one of the pad/pocket limit, you can access to the following contextual menu in the Offset field: To create or edit a formula between The Offset and another parameter To change the Offset value through a dialog box To add a maximum and minimum tolerance on the Offset parameter To modify the incrementation value of the Offset To enter a measure dialog box, in order to send the result of the measure into the Offset parameter To define a range from which the Offset value cannot go beyond or below To add a comment on the Offset parameter

Copyright DASSAULT SYSTEMES You will learn create different types of holes and locate them on existing features Creating Holes Through Hole...Blind HoleCountersunk

Copyright DASSAULT SYSTEMES What is a Hole ? A hole is removing circular material all at once, from an existing feature Its length can be defined by dimensions or with respect to other 3D elements Note that you do not need a sketch to create a hole. The sketch of the hole is automatically created. To locate precisely a hole after creation, you edit its sketch and constrain its center point for example Concentric Hole Approximate location The hole can be roughly or precisely located. You can locate precisely a hole at or after creation Rough or Precise Location? Sketch or not ? You will use Hole instead of Pocket because you can create holes including technological information such as thread, angle bottom, counterbore...

Copyright DASSAULT SYSTEMES Creating and Locating Holes... Place the hole Define holes dimensions 2 1 To create a hole you need to define its position then its dimensions OK to validate 3

Copyright DASSAULT SYSTEMES Multi-select 2 edges for position reference Since holes are sketch based we can also position them after they have been created by editing the sketch Select the face the hole will start on Modify distance to edges 5 Modify hole definition Select Hole icon 2 Creating and Positioning a Hole You get:

Copyright DASSAULT SYSTEMES Offset on Hole (1/2) Select the Hole icon Activate the Up to plane option and enter 30 as the hole diameter Select the face on which the hole will be placed When creating a hole using one of the Up to option, it is possible to define an offset in accordance with this limit. The offset can be positive or negative

Copyright DASSAULT SYSTEMES Offset on Hole (2/2) Select the Limit field Enter -10 as the Offset 45 6 Select the Select the limiting plane (face) When creating a hole using one of the Up to option, it is possible to define an offset in accordance with this limit. The offset can be positive or negative 7 Select OK You get: 10

Copyright DASSAULT SYSTEMES Standard Thread Definition (1/2) Select the Hole iconSelect the V-Bottom option from the Bottom combo Select the face on which the hole will be placed Access to standard thread design tables when creating a threaded hole 4 Select the Tread Definition tab 5 Select the Threaded buttonSelect the Metric Thick Pitch type of thread 6

Copyright DASSAULT SYSTEMES Standard Thread Definition (2/2) Select M20 as the Thread Diameter Enter 20 as the Thread Depth Enter 35 as the Hole Depth Access to standard thread design tables when creating a threaded hole 10 Select OK You get: Note: a threaded hole will appear as shown below (ISO)

Copyright DASSAULT SYSTEMES Types of hole: CounterboredSimple Tapered CountersunkCounterdrilled Threading: you can indicate the depth of threading when creating a threaded hole Types of extensions: Flat bottomV bottom Additional Information (1/3)

Copyright DASSAULT SYSTEMES Additional Information (2/3) Hole Diameters, Pitch, Right or Left Thread, Add or Remove Standards Other Thread Parameters You can choose a left or right threaded hole by selecting one of these two buttons By default, the Pitch is automatically calculated in accordance with the Thread Diameter and the standard, nevertheless, you can modify it to get a non standard thread To add or remove one or several standards, you can use these two buttons By default, the Hole Diameter is automatically calculated in accordance with the Thread Diameter and the standard, nevertheless, you can modify it to get a non standard thread

Copyright DASSAULT SYSTEMES Additional Information (3/3) A coincidence constraint is automatically created between the selected axis and the anchor point when creating a hole not normal to the selected surface Coincidence

Copyright DASSAULT SYSTEMES Dressing-Up Features You will learn how to dress-up a part with drafts, fillets, Chamfers, Drafted Filleted Pads/Pockets, shells, and patterns Drafts Filleting Edges and Corners Chamfering Drafted Filleted Pads/Pockets Shelling a Part Thread and Tap Creating Patterns

Copyright DASSAULT SYSTEMES You will learn how to create Drafts on a 3D Part Creating Drafts Drafted Part

Copyright DASSAULT SYSTEMES Drafts are angled faces defined on molded parts to make them easier to remove from molds What is a Draft ? Material gets added or removed based on the draft angle applied to the part during the operation Material removed or added? Drafted part Pulling direction: this direction corresponds to the reference from which the draft faces are defined Draft angle: this is the angle that the draft faces make with the pulling direction from the neutral element. This angle may be defined for each face Neutral element: this element defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft. The neutral element and parting element (this plane,face or surface cuts the part in 2 and each portion is drafted according to its previously defined direction) may be the same element Pulling direction Neutral element Draft angle Basic Draft definition Note : You can enter negative angle value

Copyright DASSAULT SYSTEMES Creating Basic Drafts Select the face to be drafted Select the neutral element 2 1 To create a draft angle, you need to define the faces to be drafted then the neutral element Define the draft angle 3 OK to validate 4

Copyright DASSAULT SYSTEMES The Neutral Element will remain the same during the draft Specify Selection by Neutral Face and specify draft angle 2 Select the neutral face 3 The neutral element is displayed in blue, the neutral curve is in pink. The faces to be drafted are in dark red Select Draft icon Basic Draft 1 You get:

Copyright DASSAULT SYSTEMES Draft Angle: Neutral Multi-Faces (1/3) Select the Draft Angle icon Enter 25 in the Angle field Select the faces to be drafted It is now possible to select several faces to define the neutral element. By default, the pulling direction is given by the first face you select

Copyright DASSAULT SYSTEMES Draft Angle: Neutral Multi-Faces (2/3) Select the Neutral Element Selection field a 4 5 Select the following faces in the indicated order It is now possible to select several faces to define the neutral element. By default, the pulling direction is given by the first face you select b c

Copyright DASSAULT SYSTEMES Draft Angle: Neutral Multi-Faces (3/3) Select OK in the dialog box 6 You get: It is now possible to select several faces to define the neutral element. By default, the pulling direction is given by the first face you select

Copyright DASSAULT SYSTEMES Draft Angle: Parting = Neutral (1/3) Select the Draft Angle icon Select the Neutral Element Selection field Select the faces to be drafted When building a draft angle with a parting element, you can have, by default, the parting element equal to the neutral element

Copyright DASSAULT SYSTEMES Draft Angle: Parting = Neutral (2/3) Select the plane as the Neutral Element 4 5 Select the More button in the dialog box When building a draft angle with a parting element, you can have, by default, the parting element equal to the neutral element

Copyright DASSAULT SYSTEMES Draft Angle: Parting = Neutral (3/3) Select the Parting = Neutral button then select OK 6 You get: When building a draft angle with a parting element, you can have, by default, the parting element equal to the neutral element

Copyright DASSAULT SYSTEMES Initial sketch changed If you edit the sketch used for defining the initial pad, CATIA integrates this modification and computes the draft again. In the following example, a chamfer was added to the profile Design changes There are two ways of determining the objects to draft: either by explicitely selecting the object or by selecting the neutral element, which makes CATIA detect the appropriate faces to use. Selection A plane, face or surface that cuts the part in two Parting element Neutral element (here same as parting element) Drafted portion Parting element: Additional Information

Copyright DASSAULT SYSTEMES You will learn how to create Variable Drafts on a 3D Part Variable Draft Angle

Copyright DASSAULT SYSTEMES Definitions: What is a Variable Draft Angle ? Drafts are angled faces defined on molded parts to make them easier to remove from molds. Sometimes, it is necessary (for resistance or remove from mold reasons) to define not constant draft angle values Pulling direction: this direction corresponds to the reference from which the draft faces are defined Draft angle: this is the angle that the draft faces make with the pulling direction from the neutral element. This angle may be defined for each face Neutral element: this element defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft. The neutral element and parting element may be the same element Points: this field is used to define the location of the angle values at the intersection between the neutral element and the faces to be drafted. The draft angel varies between these points

Copyright DASSAULT SYSTEMES Define the vertices and the angles 3 Creating Variable Drafts... Select the faces to be drafted Select the Neutral Element 2 1 Select OK 4

Copyright DASSAULT SYSTEMES Variable Draft Angle (1/4) You can define several angles when crating a draft angle Select the Draft Angle icon 1 Select the Variable icon 2 Select the face to be drafted 3

Copyright DASSAULT SYSTEMES Variable Draft Angle (2/4) You can define several angles when crating a draft angle Select the Neutral Element Selection field Select the neutral face Select the Points field 5 6 4

Copyright DASSAULT SYSTEMES Variable Draft Angle (3/4) You can define several angles when crating a draft angle Select the two following points Change these two angles to 30 (double clicking) Select Preview in the dialog box 9 7 8

Copyright DASSAULT SYSTEMES Variable Draft Angle (4/4) You can define several angles when crating a draft angle Select OK in the dialog box 10 You get:

Copyright DASSAULT SYSTEMES You will learn how to fillet 3D parts Filleting Fillets

Copyright DASSAULT SYSTEMES A fillet is a curved face of a constant or variable radius that is tangent to, and that joins, two surfaces. Together, these three surfaces form either an inside corner (fillet) or an outside corner (round) What is a Fillet ? Tritangent Edge fillets: Smooth transitional surfaces between two adjacent faces Face-face fillet: Used when there is no intersection between the faces or when there are more than two sharp edges between the faces Variable radius Fillets: curved surfaces defined according to a variable radius Tritangent fillets: Involves the removal of one of the three faces selected Different types of fillets Face-face Edge Propagation modes Tangency Minimal Variable

Copyright DASSAULT SYSTEMES Creating Fillets... Select the edge to be filleted 1 To create a fillet, you need to select the edge to be filleted and to enter the fillet radius Enter the fillet radius 2 OK to validate 3

Copyright DASSAULT SYSTEMES Specify Fillet Radius 2 Select Edge Fillet icon Select upper face and four side edges 3 1 Edge Fillets You get:

Copyright DASSAULT SYSTEMES Notice that when the fillet runs over the edge of the part, CATIA alters the edge to accommodate the fillet Specify Fillet Radius Select Edge Fillet icon Select edge to be filleted 1 Round Corner Fillets 2 3 You get:

Copyright DASSAULT SYSTEMES Activate the Edge fillet icon and select the edge to be filleted 2 Select the More button in the dialog box (2) 3 Select the Edge(s) to keep field (1) 4 Select the edge on which the fillet will roll You get : (3) (4) 5 Enter the radius value (eg : 30) then select OK (5) Note : This option is also available with the variable fillet function Creating a Fillet with Keep Edge : Rolling on an Edge

Copyright DASSAULT SYSTEMES Activate the Edge fillet icon and select the edges to be filleted 2 Select the More button in the dialog box (2) 3 Select the Edge(s) to keep field (1) 4 Select the edge on which the fillet will roll You get : (3) (4) 5 Enter the radius value (eg : 5) then select OK (5) Note : This option is also available with the variable fillet function Creating a Fillet with Keep Edge : Rolling around an Edge

Copyright DASSAULT SYSTEMES Edge Fillet with Limiting Planes, Faces or surfaces (1/3) You can limit the propagation of an edge fillet using a plane, a face or a surface Select the Edge Fillet icon 1 Select the edge on which you want to create a fillet 2 To expand the dialog box, select the More button 3

Copyright DASSAULT SYSTEMES Edge Fillet with Limiting Planes, Faces or surfaces (2/3) You can limit the propagation of an edge fillet using a plane, a face or a surface Select the Limiting element field 4 Select the limiting surface 5 Select to change the direction 6

Copyright DASSAULT SYSTEMES Edge Fillet with Limiting Planes, Faces or surfaces (3/3) You can limit the propagation of an edge fillet using a plane, a face or a surface You get: Select OK in the dialog box 7

Copyright DASSAULT SYSTEMES Edge Fillet: Trim Ribbons When choosing the Tangency propagation mode, you can also trim overlapping fillet. To do so, simply check the Trim Ribbons option in the dialog box Select the Edge Fillet icon 1 Select the edges to be filleted 2 Modify the fillet radius and activate the Trim Ribbons option 3 Select OK in the dialog box 4 You get:

Copyright DASSAULT SYSTEMES You generally 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 Select Face-Face Fillet icon 2 Multi-select faces to be filleted 1 Specify Fillet Radius 3 Face-Face Fillets You get:

Copyright DASSAULT SYSTEMES Select the face to be removed by the fillet 3 Select Tritangent Fillet icon Multi-select two faces to be filleted 1 Multi-selecting all three faces tells CATIA to remove the third face selected Tritangent Fillets 2 You get:

Copyright DASSAULT SYSTEMES Select edge to be filleted 1 Select Variable Radius Fillet icon By double clicking, modify the radii 3 Variable Radius Fillets 2 You get:

Copyright DASSAULT SYSTEMES Variable Radius Fillet: Circular Close Edge (1/2) Select the Variable Radius Fillet icon Select the Points field Select the edge to be filleted It is possible to build a variable radius fillet on a circular close edge 4 Deselect the default vertex Select the two new vertices 5

Copyright DASSAULT SYSTEMES Variable Radius Fillet: Circular Close Edge (2/2) Double click on the following radius Select OK in the main dialog box Enter 20 in the Value field then select OK It is possible to build a variable radius fillet on a circular close edge You get:

Copyright DASSAULT SYSTEMES Select the Variable fillet icon 2 Select the edge to be filleted Once an edge has been selected during a variable radius fillet creation, two radius labels appear at the edge extremities. If you modify the radius value in the dialog box, the two radius label will be modified at the same time. If you want to modify only one of the radii, you will have to double click on the radius label and modify its value 3 Enter a new radius value ( eg :10) 4 Notice that the two radius values are modified at the same time Radius Definition per Edge when Creating a Variable Radius Fillet

Copyright DASSAULT SYSTEMES Variable radius fillet To add additional points on the edge to be filleted, you can select planes. CATIA computes the intersections between these planes and the edge to determine the useful points. In this example, three planes were selected. Now, if you move these planes later, CATIA will compute the intersections again and modify the fillet accordingly. The intermediate radii can be nil Variable Radius Fillets Additional Information (1/2)

Copyright DASSAULT SYSTEMES Capability to create a variable radius fillet with the fillet sections keeping a constant direction in accordance with a spine Spine The fillet sections are perpendicular to the spine The fillet sections are perpendicular to filleted edge Edge to be filleted The dotted blue circles indicate the fillet sections but CATIA DOES NOT SHOW THEM when creating a fillet With spine Without spine Additional Information (2/2)

Copyright DASSAULT SYSTEMES You will learn how to create chamfers on 3D parts Chamfering Chamfers

Copyright DASSAULT SYSTEMES Chamfering consists in removing or adding a flat section from a selected edge to create a beveled surface between the two original faces common to that edge. You obtain a chamfer by propagation along one or several edges. What is a Chamfer ? Propagation modes Tangency Minimal

Copyright DASSAULT SYSTEMES Creating Chamfers... Select the edge to be chamfered 1 To create a chamfer, you need to select the edge to be filleted and to enter the chamfer dimensions Enter the chamfer dimensions 2 OK to validate 3

Copyright DASSAULT SYSTEMES Multi-select edges to be chamfered 1 Select Chamfer icon Modify Chamfer definition 3 Symmetric Chamfer 2 You get:

Copyright DASSAULT SYSTEMES Multi-select edges to be chamfered 1 Select Chamfer icon Modify Chamfer definition 3 Non Symmetric Chamfer If necessary, reverse the chamfer then select OK 4 2 You get:

Copyright DASSAULT SYSTEMES Chamfers can be created by selecting a face whose edges are to be chamfered Chamfers Select faceChamfer Additional Information...

Copyright DASSAULT SYSTEMES Drafted Filleted Pad You will learn how to create a pad which includes fillets and a draft angle This function will allow you to create a pad with draft and fillets simultaneously, rather than creating each feature separately

Copyright DASSAULT SYSTEMES What is Pad with Integrated Draft and Fillets ? Lateral Radius Draft Angle First limit radius Second limit radius A pad with an integrated draft angle and fillets is a solid which is extruded from a 2D profile, and which includes fillets and draft angle

Copyright DASSAULT SYSTEMES Creating Pads with Integrated Draft and Fillets... Select the profile 1 To create a pad with integrated draft and fillets, you need to select a profile then enter the pad dimensions Enter the pad dimensions 2 OK to validate 3

Copyright DASSAULT SYSTEMES (1) 1 Select the Drafted Filleted Pad icon 2 Select the sketch that will build the pad The Drafted Filleted Pad function allows you to create a pad which includes a general draft, a Lateral Radius, a First Limit Radius and a Second Limit Radius. The draft angle and the radii are created as individual features (2) 3 Select the second limit (3) 4 Enter the pad Length 5 Enter the draft angle 6 Enter the lateral radius 7 Enter the First limit radius 8 Enter the Second limit radius 9 If necessary, reverse the pad direction 10 Select OK You get : First limit radius Second limit radius Lateral Radius Draft Angle By default, the neutral element used to compute the draft angle is the first limit of the pad. However, you can use the second limit as the neutral element Drafted Filleted Pad

Copyright DASSAULT SYSTEMES A pad A draft angle Three fillets After a drafted filleted pad creation, the tree contains : Additional Information...

Copyright DASSAULT SYSTEMES Drafted Filleted Pocket You will learn how to create a pocket which includes fillets and a draft angle This function will allow you to create a pocket with draft and fillets simultaneously, rather than creating each feature separately

Copyright DASSAULT SYSTEMES What is Pocket with Integrated Draft and Fillets ? Lateral Radius Draft Angle First limit radius Second limit radius A pocket with an integrated draft angle and fillets is a solid which is extruded from a 2D profile, and which includes fillets and draft angle

Copyright DASSAULT SYSTEMES Creating Pockets with Integrated Draft and Fillets 1 To create a pocket with integrated draft and fillets, you need to select a profile then enter the pocket dimensions 2 3 Select the profile Enter the pocket dimensions OK to validate

Copyright DASSAULT SYSTEMES (1) 1 Select the Drafted Filleted Pocket icon 2 Select the sketch that will build the pocket The Drafted Filleted Pocket function allows you to create a pocket which includes a general draft, a Lateral Radius, a First limitd Radius and a Second limit Radius. The draft angle and the radii are created as individual features. (2) 3 Select the second limit (3) 4 Enter the pocket depth 5 Enter the draft angle 6 Enter the lateral radius 7 Enter the First limit radius 8 Enter the Second limit radius 9 If necessary, reverse the pocket direction 10 Select OK You get : Lateral Radius Draft Angle By default, the neutral element used to compute the draft angle is the first limit of the pocket. However, you can use the second limit as the neutral element First limit radius Second limit radius Drafted Filleted Pocket

Copyright DASSAULT SYSTEMES Additional Information... A pocket A draft angle Three fillets After a drafted filleted pocket creation, the tree contains :

Copyright DASSAULT SYSTEMES You will learn how to shell 3D part Shelling a Part Shelled Part

Copyright DASSAULT SYSTEMES Shelling a feature means emptying it, while keeping a given thickness on its sides Shelling may also consist in adding thickness to the outside You can have different thicknesses per faces What is Shelling ? Faces to be removed Shell Other thickness face

Copyright DASSAULT SYSTEMES Creating Shells... Select the face to be opened 1 To create a shell, you need to select the face(s) to be opened then to define the thickness(es) of the shell Enter the shell thickness 2 OK to validate 3

Copyright DASSAULT SYSTEMES The Outside Thickness entry adds material to the outside of the part definition Multi-select the faces to be removed in shelling operation Select Shell icon 2 Specify the wall thickness for the Shell 3 Shelling a Part You get: 1 Select the Other thickness faces field 4 Double click on the dimension in order to modify the thickness of the face 5 Enter 10mm in the appearing dialog box then select OK 6 Select OK in the main dialog box 7

Copyright DASSAULT SYSTEMES Shelling a feature means emptying it, while keeping a given thickness on its sides. Shelling may also consist in adding thickness to the outside Thickness inside & outside Inside onlyInside & Outside Additional Information... It is possible to create a shell with a thickness greater than the smallest fillet radius on the part Shell with Thickness > Curvature Faces to be removed Modified thicknesses Dotted blue lines = Cube before the shell operation R5 Thickness=15

Copyright DASSAULT SYSTEMES You will learn how to create threads and taps Thread and Tap

Copyright DASSAULT SYSTEMES You can create threads and tap with CATIA, you will not see them in 3D but all the information will be recorded. The result of a thread or a tap will be see on a drawing in accordance with the drawing standard Thread What are Thread and Tap ? A thread is an helical groove made on a cylinder Thread Tap A tap is an helical groove made inside a hole Tap Different Standards Customized Standards Not seen like this in CATIA

Copyright DASSAULT SYSTEMES Creating Thread and Tap... Define the Lateral and Reference surface 1 To create a thread: Define the thread parameters 2 The thread appears in the tree 3

Copyright DASSAULT SYSTEMES Select the Thread/Tap icon 2 Select the Lateral Face on which the thread will be grooved 3 Select the Reference Face from which the thread will begin 4 In order to define the standard for the thread, select the Metric Thin Pitch in the dialog box 5 To define the Thread Diameter, select M10 in the dialog box 6 As the Thread Depth, enter 26 in the Thread Depth field Creating Thread and Tap (1/2)

Copyright DASSAULT SYSTEMES Select the Preview button in the dialog box, you will get a preview of the thread 8 Select the OK to validate the thread creation You get: During the thread creation CATIA helps you with the thread parameters in accordance with the selected standard Creating Thread and Tap (2/2)

Copyright DASSAULT SYSTEMES You will learn how to create patterns out of an existing feature Creating Patterns Rectangular Pattern Circular Pattern User Pattern

Copyright DASSAULT SYSTEMES Patterns allow you to create several identical features from an existing one and to simultaneously position them on a part What is a Pattern ? Rectangular pattern CATIA allows you to define three types of patterns which makes the creation process easier : rectangular circular user patterns 3 types of patterns Pad with pattern feature

Copyright DASSAULT SYSTEMES Creating Patterns... Select feature to be duplicated 1 Select the directions then fill the dialog box 2 OK to validate 3

Copyright DASSAULT SYSTEMES Select Rectangular Pattern icon … then select pocket to use for pattern Specify the second direction as in step 2 under the Second Direction tab (Reverse if necessary) 3 Specify the first direction of the pattern by selecting an edge using Reverse to change the direction if needed 2 Rectangular Pattern 1 You get:

Copyright DASSAULT SYSTEMES Select the feature to be patterned 1 Select Circular Pattern icon Define pattern parameters and specify the rotation axis of the pattern by selecting the face 3 Circular Pattern 2 You get:

Copyright DASSAULT SYSTEMES Select User Pattern icon Select hole to be patterned 1 Select 'Sketch 4' in the specification tree. This sketch includes the nine points you need to locate the duplicated holes 3 User Pattern 2 You get:

Copyright DASSAULT SYSTEMES With the Ctrl key held down, select the hole and the fillet (you can select them from the solid or from the tree) 2 Activate the Circular pattern icon It s possible to apply a rectangular, circular or user pattern to several features in one shot. We are going to apply a circular pattern to a hole and a fillet (2) 3 Select the Reference field (1) 4 Select the circular edge to define the pattern axis of rotation (3) (4) 5 Select the Instance(s) field and enter 6 6 Select the Angular spacing field and enter 60 (6)(5) Pattern of a Selection of Features (1/2)

Copyright DASSAULT SYSTEMES Select the Crown Definition tab It s possible to apply a rectangular, circular or user pattern to several features in one shot. We are going to apply a circular pattern to a hole and a fillet (10) 9 Select the Circle spacing field and enter 20 (9) 10 Select OK You get : (8) (7) 8 Select the Circle(s) field and enter 4 Pattern of a Selection of Features (2/2)

Copyright DASSAULT SYSTEMES Exploding a Pattern Capability to explode a pattern in order to get one feature per instance Select the Update icon 2 Select the Explode command from the pattern contextual menu 1 You get:

Copyright DASSAULT SYSTEMES Select the planar face (or plane) that will be the plane of symmetry 1 Activate the Mirror icon Before building a part, you can search for the symmetry and decide to build only the half of the part, then use the Mirror function to get the whole part (1) 3 Select OK (2) (3) You get : Mirror

Copyright DASSAULT SYSTEMES With the Ctrl key held down, select the pad (Pad.2) and the two last fillets (you can select them from the solid or from the tree) 2 Activate the Mirror icon It s possible to apply a Mirror to several features in one shot (2) 3 Select the Mirroring element (plane or planar face) (1) 4 Select Ok in the dialog box (3) (4) You get : Mirror of a Selection of Features

Copyright DASSAULT SYSTEMES Deleting the instances of your choice is possible when creating the pattern. In the pattern preview, just select the points materializing instances. Conversely, selecting these points again will make CATIA create the corresponding instances Deleting or adding instances at creation Instances selection To define a direction, you can select an edge or a planar face. Selecting a face will allow both directions of a rectangular pattern to be defined or the axis of rotation normal to the face for a circular pattern Direction of creation Additional Information (1/2)

Copyright DASSAULT SYSTEMES Select the Object field in the dialog box Adding or removing a feature from the list of feature when creating or editing a pattern To remove a feature from the list of features: Additional Information (2/2) Select the feature to be removed from the tree Select OK

Copyright DASSAULT SYSTEMES Modifying Profile Geometry Reordering Features Modifying Features Modifying Parts You will learn how to modify profiles and features to change 3D part

Copyright DASSAULT SYSTEMES You will learn how modify 2D sketch elements to propagate changes to 3D parts Modifying Profile Geometry After ChangeBefore

Copyright DASSAULT SYSTEMES Sketch-based features rely on profiles for their shape Especially if defined with the proper constraints that represent the design intent of the part, the profile geometry can easily be changed for downstream design changes Modified cube Why Modify Profile Geometry? Chamfer added from sketch Changing the sketch that defines a feature propagates that change to all subsequent operations involving the feature Design change

Copyright DASSAULT SYSTEMES Modifying Profiles... Edit the sketch corresponding to the feature to be modified 1 Modify the profile or dimensions 2 Update the Part 3

Copyright DASSAULT SYSTEMES Alter the existing coordinates of the line to new parameters (V: 50mm) 2 H: -40 V: 50 This method works on most construction entities, opening the appropriate dialog for the entity selected Double click line to edit its coordinates 1 Modifying Profile Element Coordinates

Copyright DASSAULT SYSTEMES You have modified the shape of the profile without the use of any intermediary menu options The profile stretches based on where you move the element and the constraints you have applied 2 Click and drag the line downward to its new location 1 Editing Profile Shape and Size

Copyright DASSAULT SYSTEMES Select the element to be deleted 1 Select Edit->Delete and the element is erased. Now multi-select additional elements to delete 2 Use the contextual menu (select Mouse Button 3 while cursor is on one of the selected elements) to delete 3 Deleting Sketcher Elements You get:

Copyright DASSAULT SYSTEMES To delete a set of 2D elements, multi-select the elements you wish to delete using the click and drag method. Then go to the Edit menu and select delete Deleting elements Multi-selection Additional Information...

Copyright DASSAULT SYSTEMES You will learn how to reorder features making up a 3D part Reordering Features Pad moved before mirrorPad after mirror operation

Copyright DASSAULT SYSTEMES Reorder allows you to correct a part so that your design intent is preserved One cylinder Why to Reorder Features ? Changes and features created later in the process can easily be incorporated into the part structure taking into account the design intent Design change Two cylinders when moved before mirror

Copyright DASSAULT SYSTEMES Reordering Features... Select Reorder from the feature contextual menu 1 Select the feature after which the hole will be placed 2 Update the Part 3

Copyright DASSAULT SYSTEMES Right click the feature to be reordered to get a contextual menu 1 Pad.2 was incorrectly created after the mirror operation, so we must reorder the pad before the mirror Select Reorder 2 Select Pad.1 in the specification tree as the feature to reorder after (Pad.1 is shown as the preview) 3 Reordering Features You get:

Copyright DASSAULT SYSTEMES You will learn how to modify 3D features parameters Modifying Features Modified Pad

Copyright DASSAULT SYSTEMES Often, as a design matures, the initial configuration of a part needs refinement through the modification of feature parameters or the addition/removal of features Why Modify Features ? Modified pad Draft angle Pad length

Copyright DASSAULT SYSTEMES Modifying Features... Double click on the feature to be modified 1 Modify the feature dimensions 2 Update the Part 3

Copyright DASSAULT SYSTEMES Modify the draft specifications by double clicking the dimension or entering in the dialog box 2 Double click the feature or its specification to edit the feature 1 Next, modify Pad.1 of the part by right clicking the feature in the specification tree and selecting Definition... 3 …then modify the dimension directly or through its dialog box Redefining Feature Parameters You get:

Copyright DASSAULT SYSTEMES Double click feature or its specification in the tree to edit hole 1 Change the hole definition in the dialog box or double click on dimensions to modify directly 2 Modify position dimensions by double clicking them to modify directly Editing Holes You get:

Copyright DASSAULT SYSTEMES Double click on the pad to be modified 2 Select the sketch icon from the dialog box in order to activate the sketcher (2) 3 Modify the constraint (1) 4 Leave the sketcher by selecting the Exit icon 5 If necessary, select the Update All icon You get : (3) (4) (5) Sketch Edition During Pad Edition

Copyright DASSAULT SYSTEMES Double click on the pad to be modified 2 Select the sketch field from the dialog box (2) 3 Select the replacing sketch (1) 4 Select OK You get : (3) (4) 5 If necessary, select the Update All icon (5) Replacing Sketch During Pad Edition

Copyright DASSAULT SYSTEMES CATIA allows to delete features simply by selecting the feature to delete and selecting delete in the Edit menu (or right clicking the selected feature and selecting delete in the contextual menu Deleting features Deleting a feature produces a dialog that can be expanded to show the impact of deleting the feature, allows you to manage the deletion and actually gives you the opportunity to replace it with another element Deleting a sketch Additional Information...