CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Additional Features
Student Notes:
In this lesson you will learn how to create additional CATIA features.
Lesson Contents:
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Case Study: Additional Features Design Intent Stages in the Process Create Feature Profiles and Axis system Create Shaft and Groove Features Create Basic Wireframe Geometry Shell the Model
Duration: Approximately 0.5 day
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Case Study: Additional Features
Student Notes:
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The case study for this lesson is the Suspension Seat used in the Front Suspension and Engine assembly shown below. The Suspension Seat is part of the Damper subassembly. The focus of the case study is creation of features that incorporates the design intent of the part.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Design Intent
Student Notes:
The Suspension Seat must meet the following design intent requirements: The axis of main flange must be at 5 degrees from Z axis. • The axis of revolution of main flange must make an angle of 5 degrees to Z axis.
The main flange must be at 12 degrees from horizontal plane. • The sketch of main flange must make an angle of 12 degrees to horizontal plane.
One large hole of diameter 50mm must be created for Pillar clearance. • Create a shaft of diameter 58mm and shell it to get hole diameter of 50mm.
The thickness of Seat must be 4 mm. Create a Shell of default thickness 4 mm.
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Apply Fillets at all sharp corners.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Stages in the Process
Student Notes:
Use the following steps to create the Suspension Seat: 1. Create a reference geometry. 2. Create an Axis System. 3. Create a sketched geometry. 4. Create shafts. 5. Create fillets. 6. Create a pocket. 7. Shell the model.
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8. Create a hole.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Create Feature Profiles and Axis system
Student Notes:
In this section you will learn about additional sketch tools.
Use the following steps to create the Suspension Seat: 1. 2. 3.
Create Basic Wireframe Geometry. Create Shaft and Groove Features. Shell the Model.
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4.
Create Feature Profiles and Axis System.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Additional Sketcher Tools Lesson 2 introduced you to the basic Sketcher tools and the Sketcher environment. This lesson will introduce you to the advanced Sketcher tools. Sketcher includes the following additional tools: Axis creation tool Re-limitation tools Transformation tools Project 3D element tools Analyze a sketch using the Sketch Analysis tool.
Axis Creation
Re-limitation
Project 3D elements
Transformations
In addition, you will learn how to:
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Create Equivalent dimensions Create Formula
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Sketch Analysis
Formula creation
Equivalent dimension creation
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Sketcher Re-limitation Tools The Re-limitation tools trim or extend the existing sketched geometry. They can be found in the Relimitation toolbar, which is a flyout menu in the Operation toolbar.
Available re-limitation tools include the following: A. Trim B. Break
A B
C. Quick Trim
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D. Close
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E. Complementary Angle
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Re-limitations Tool
Geometry
Description Trims two curves. Keeps the part of the curves you selected. This option can also be used to extend to elements.
Break
Breaks a curve at a selected point.
Quick Trim
Trims an intersected element.
Close
Closes the selected arc.
Complement
Creates the complementary arc.
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Trim
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Trim Options Once the Trim tool is selected, the Sketch Tools toolbar expands to display two modes for trim:
A. The Trim All Elements mode trims both the selected elements. B. The Trim First Element mode trims only the first selected element; the second element is left unchanged.
First Element
Second Element
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B
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Quick Trim Options Before
Once the Quick Trim tool is selected, the Sketch Tools toolbar expands to display several modes for quick trim: A. The Break and Rubber In mode removes a selected portion of an element up to its intersection with other elements. B. The Break and Rubber Out mode keeps the selected portion of an element up to its intersection with other elements. C. The Break and Keep mode keeps the entire elements but breaks the element at the intersection with other elements.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Sketcher Transformation Tools Transformation tools are used to modify existing sketcher geometry. They can also be used to create a duplicate of the existing sketcher geometry. Transformation tools are found in the Transformation toolbar, which is a flyout menu in the Operation toolbar. Available Transformation tools include the following: Mirror Symmetry Translate Rotate Scale Offset
A B C D E F
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A. B. C. D. E. F.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Mirror and Symmetry Options Both options, Mirror and Symmetry, allow you to mirror the selected geometry about an axis. The Mirror option retains the original geometry, while the Symmetry option removes it. Use the following steps to use the Mirror and Symmetry tools:
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1. Select the geometry to mirror. Use the key to select multiple items. 2. Select the tool. a. Mirror b. Symmetry 3. Select the symmetry axis.
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Result of Mirror
Result of Symmetry
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Translation (1/2) The Translation tool moves the selected geometry along a translation vector.
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Use the following steps to translate geometry: 1. Select the entities to move. 2. Select the Translate tool. 3. Select the Duplication mode option. When the Duplication mode option is selected, the original geometry is unchanged and a copy of the geometry is created in the new location. You can also create multiple instances which are equidistant to each other. In this example, two instances are created.
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4. If in the duplicate mode, specify the constraint conditions.
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You may choose to keep all internal constraints, and/or all external constraints.
5. Select a point on the screen to act as the start point.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Translation (2/2) Use the following steps to translate geometry (continued): 6. 7.
8.
Optionally, enter a distance value in the length field and click OK. Move the start point on the screen. If no distance has been specified (step 6), you can place the selected elements anywhere. If a distance has been applied and OK is selected, you will have to define the direction. Click to place the geometry.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Rotation (1/2)
Student Notes:
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The Rotate tool lets you rotate selected sketched element(s) about a point. Use the following steps to rotate geometry: 1. Select the entities to rotate. 2. Select the Rotate tool. 3. Select the Duplication mode option. When the Duplication mode option is selected, the original geometry is unchanged and a copy of the geometry is created in the new location. You may create multiple instances which are equidistant to each other. In this example, one instance is created.
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4. If in duplicate mode, specify Constraint Conservation. If selected, all internal constraints will be maintained. 5. Select a point on the screen to act as the center of rotation. Copyright DASSAULT SYSTEMES
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Rotation (2/2) Use the following steps to rotate geometry (continued): 6. Select a point on the screen to define a reference line for the angle. 7. Specify a value in the Angle field or move the mouse to rotate the elements. 8. Click OK or click on the screen to complete the rotation.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Scale (1/2) The Scale tool allows you to resize the selected sketched element(s).
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Use the following steps to scale sketched element(s): 1. Select the entities to scale. 2. Select the Scale tool. 3. Select the Duplication mode option. When the Duplication mode option is
selected, the original geometry is unchanged and a copy of the geometry is created in the new location.
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4. If in duplicate mode, specify Conservation of the constraints. If selected, all the constraints will be maintained, but they will be converted into reference dimensions.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Scale (2/2) Use the following steps to scale sketched element(s) (continued): 5. Select a point on the screen to act as the center point for scaling. 6. Specify a value in the Scale field or move the mouse to scale the elements. 7. Click OK or click on the screen to complete the scaling.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Offset Propagation Modes The Offset tool lets you offset one or more sketched elements. Once the Offset tool is selected, three propagation modes become available from the Sketch Tools toolbar: A. In No Propagation mode, only the selected element(s) is offset. B. In Tangent Propagation mode, the selected element(s) and all elements tangent to it are offset. C. In Point Propagation mode, the selected element(s) and all elements that form a chain with it are offset.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Offset (1/2) Use the following steps to offset sketched element(s): 1. 2. 3. 4. 5.
Select the sketched element(s) to offset. Click the Offset icon. Select the Propagation mode. Click the Both sides icon if you want to offset the element on both sides. Enter the number of instances. Each instance will be equi-distant from each other. In this example, two instances are created.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Offset (2/2) Use the following steps to offset sketched element(s) (continued): 6. 7. 8.
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Move your pointer to the side on which you want to create the offset. Press the key until the Offset field is highlighted. Specify the offset distance. Press the key to place the offset.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Project 3D Elements Several tools are available to project the existing 3D elements onto the sketch plane. These projected elements can be used as a standard sketch geometry, or converted into a construction geometry. 3D projection tools are found in the 3D Geometry toolbar, which is a fly-out menu in the Operation toolbar. Available projection tools include the following: A
A. Project 3D Elements B. Intersect 3D Elements
B C
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C. Project 3D Silhouette Edges
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
3D Geometry Elements
Tool Project 3D Elements
Intersect 3D Elements
Description
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Project 3D elements onto the sketch plane.
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Intersect 3D elements with the sketch plane.
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Project the silhouette of a cylindrical element onto the sketch plane. The axis of revolution for the projected element must be parallel to the sketch plane.
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Project 3D Silhouette Edges
Geometry
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Isolate Projected Elements
Student Notes:
By default, projected elements are linked to the 3D geometry from which they were created. You can break this link by right-clicking on the projected element and clicking Mark.x object > Isolate from the contextual menu. Once the element is isolated, it will no longer be associative with the 3D geometry from which it was projected. This means that modifications to the 3D geometry will not impact the sketched elements created from it.
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Once isolated, the projected geometry converts into standard sketched elements (e.g., lines, points, arcs).
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Sketch Analysis
Student Notes:
The Sketch analysis tool can be used to help resolve problems with the sketch. This tool can be used to determine a sketch’s constraint status (i.e., Under-constrained, Isoconstrained, Over-constrained, or Inconsistent), and where degrees of freedom still exist in the sketch.
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The Sketch Analysis tool can also be used to determine whether a profile is open or closed. This is useful if you receive an error while trying to create sketched-based features.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Sketch Analysis Window (1/3) The sketch analysis window has three tabs. Each tab contains information to analyze the sketch.
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The Geometry tab is used to determine whether the sketch geometry is valid or not: A. The General Status area analyzes several elements in the context of the entire sketch. B. The Detailed Information area provides the status and comment on each geometric element in the sketch. C. The Corrective Actions area lets you correct geometry. You can: a. Convert an element into a construction element. b. Close an open profile. c. Erase unwanted geometry. d. Hide all the constraints. e. Hide all the construction geometries.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Sketch Analysis Window (2/3) The Projections/Intersections tab is used to determine the status of all the projected elements:
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B a
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A. The Detailed Information area provides a the status and comment on each projected or intersected element in the sketch. B. The Corrective Action area lets you correct geometry. You can: a. Isolate geometry. b. Activate or Deactivate a constraint. c. Erase geometry. d. Replace a 3D geometry. e. Hide all the constraints. f. Hide all the construction geometries.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Sketch Analysis Window (3/3) The Diagnostics tab displays a full diagnosis of all the sketched geometries. It provides an analysis of the sketch as well as information on individual geometrical elements:
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A. The Solving Status area provides an overall analysis of the sketched geometry. B. The Detailed Information area provides a description and status on each constraint and geometric element in the sketch. C. The Action area enables you to: a. Hide all constraints. b. Hide all the construction geometries.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Performing a Quick Geometry Diagnosis (1/2) Use the following steps to analyze a sketch: 1. 2.
3.
Click the Sketch Solving Status icon. The Sketch Solving Status dialog box appears. It indicates the overall status of the Sketch Geometry. In this case, the sketch is under-constrained even though the sketch appears to be green (isoconstrained). Under- and over-constrained geometrical elements are highlighted on the sketch and in the specification tree.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Performing a Quick Geometry Diagnosis (2/2) Use the following steps to analyze a sketch (continued): 4. Click the Sketch Analysis icon in the window or in the toolbar. 5. The Sketch Analysis window appears. In this example, the profile needs to be closed and the point needs to be changed to a construction element. 6. Click Close to close the Sketch Analysis window.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Create Relationships between Dimensions
Student Notes:
Relationships between Dimensions can be created by usinga. Equivalent Dimensions b. Formula The Equivalent Dimensions feature can be used to define an equality between a set of Angles or Length parameters. The formula can be used to relate one parameter to another.
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Highlighted dimensions are Equivalent Dimensions
Highlighted dimension is driven by a formula
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Equivalent Dimensions
Student Notes:
The Equivalent Dimensions feature can be found in the Knowledge toolbar, which can be accessed in any workbench (such as Sketcher, Part Design) . The value of Length or Angle can be modified through the editor and is propagated to all the parameters belonging to the equivalence.
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Equivalent Dimensions feature help toa. Increase designers’ productivity. b. Reduce the model size.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Creating Equivalent Dimensions Use the following steps to create Equivalent Dimensions through a sketcher: 1. 2. 3.
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Edit the sketch to enter the Sketcher Workbench. Select the dimensions that you want to equalize and click Equivalent Dimensions icon. Equivalent Dimension edition dialog box is displayed. a.
b. c. d. e.
Click Edit List to add/remove parameters for equivalent dimensions. A dialog box is displayed for you to select the equivalent parameters. Use arrows to add/remove parameters for equivalent dimensions. Click OK to go back to Equivalent Dimension edition dialog box. In Equivalent Dimension edition dialog box, specify the value of equality.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Editing Equivalent Dimensions through Feature Tree 1. The Equivalent dimension feature is displayed in the Relations node of the feature tree.
a. Double-click on it to view the list of parameters, modify it or change the value. b. Double-click on Value to change the value of equality.
Student Notes:
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2. Any dimension in the list of equivalent dimensions can be selected graphically and edited in order to modify all the dimensions. The big advantage is that there is no unique driving dimension. a. Double-click the value: the dialog box displays an icon next to the value which shows that this is an equivalent dimension. The value can be modified in the same way as you modify a standard constraint
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Formula A formula is used to relate one parameter to another. It can be created by: 1. 2.
Using the formula window. Editing the dimension value with the contextual menu.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Creating a Formula Use the following steps to create a formula through a sketcher: 1. Edit the sketch to enter the Sketcher Workbench. 2. Double-click the dimension to which you want to associate a formula. 3. From Contextual menu in the value field select Edit Formula. 4. In the Formula Editor dialog box, add a relation. 5. Symbol f(x) appears in front of a dimension to which the formula is associated.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Editing Formula through Feature Tree 1.
The Formula feature is displayed in the Relations node of the feature tree. a.
b.
Double-click it to view the relation and to modify it. The highlighted value is a driving dimension.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Create an Axis System A local axis is a user-defined axis system that can be used to define local coordinates. For example, it is often easier to build a point by coordinates, with respect to a local axis rather than creating it in the absolute coordinates system. An axis system can automatically be generated when a new part is created. This axis system is defined at the origin of the model and uses the default reference planes for direction.
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Local Axis System
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Types of Axis System The following types of local axis systems can be defined: 1. 2. 3.
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Standard Axis System: is defined by a origin and three orthogonal directions. Rotation Axis System: is defined by an origin, three orthogonal directions, and an angle based on a selected reference. Euler Axis System: is defined using Euler angles to specify its orientation.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Creating an Axis System 1
Use the following steps to create a local standard axis system: 1. Click the Axis System icon. 2. Select the pad vertex as origin point. 3. To define an axis direction, click on the appropriate axis field and select an element to define direction. For example, to define the direction of the X axis, click on the X axis field and select the element to define the direction. 4. Click on a second axis field and define its direction. The direction of the third axis will automatically be defined based on the previous selections. 5. Select the Reverse option to reverse the axis direction, if necessary. In this example, the X axis is reversed. 6. Click OK to create the axis.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Axis System: Set as Current
Student Notes:
By default, the last created axis system becomes the active system. The current axis system is highlighted in the specification tree, and is displayed with solid lines on the model. All the other axis systems are dashed lines on the model.
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To change the active axis system, right-click on the system to be made current and click Axis System.x object > Set as Current.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Axis System with New Part
Student Notes:
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An axis system can automatically be generated when a new part is created. This axis system is defined at the origin of the model and uses the default reference planes for direction. If this option needs to be changed, click Tools > Options > Infrastructure > Part Infrastructure. Then from the Part Document tab, select the Create an Axis System when creating a new part option.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Additional Sketcher Tools
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a positioned sketch in order to control the profile’s orientation and position with respect to an existing environment. You will use some of the additional sketcher tools you have learned in this lesson to complete the exercise. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a positioned sketch Use a sketch analysis tool Create a fully constrained sketch
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Use an Axis System
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/18) 1.
Load the part and create an Axis System a. b. c. d. e. f. g.
Load Ex4A.CATPart from the database. Click the Axis System icon. Select Standard as Axis system type. Select Point.2 as Origin. Select YZ plane of Axis System.2 as X axis and select the Reverse option. Select ZX plane of Axis System.2 as Y axis and select the Reverse option. Click OK.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/18) 2. Create a positioned sketch . Create a positioned sketch that contains one open profile. You will use this sketch to create an Extruded surface in a later step. a. Click the Positioned sketch icon. b. Select the YZ plane of Axis System.3 as sketch support. c. Select the Implicit as the Origin. d. Select Reverse H. e. Click OK to enter Sketcher workbench.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/18)
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3. Sketch a profile. To begin the sketch, create a profile using the profile tool that is the general shape and size the final sketch will be.
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a. Select Point.1 and click Project 3D element icon. b. Select the Profile icon and click this projected element to define the starting point. c. Draw a horizontal line. d. Select the Three point Arc icon. e. Create the arc shown. f. The profile tool will default back to Line. Create another horizontal line. g. Create an inclined line. h. Create third horizontal line. i. Create second inclined line. j. Create fourth horizontal line. k. Create third inclined line.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/18) 4. Create geometrical constraints. Note: The profile must be constrained with respect to Axis System.3 and not to the standard orthogonal planes. a. Select the two horizontal lines by pressing and holding key. b. Select the Constrain Defined in Dialog Box icon. c. Select Coincidence in Constraint Definition box.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/18) 4.
Create a geometrical constraints. (Continued) d. e.
f.
Select the constraint icon. Select the two inclined lines by pressing and holding key. Angle dimension is displayed. Right mouse click on the dimension and select Parallelism.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (6/18) 5. Create a horizontal dimension and radius dimension. Dimension the horizontal line and arc using the Constraint tool.
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a. Select the Constraint icon. b. Select the top horizontal line. c. Drag the mouse to the place the dimension and left mouse button click to complete its placement. d. Double-click the dimension and change its value to [140mm]. e. Select the Constraint icon. f. Select the arc. g. Drag the mouse to place the dimension. Left mouse button click to complete the dimension. h. Double-click the value and change its value to [870mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (7/18) 6. Create vertical and horizontal dimensions. Create the overall vertical length of the profile using the Constraint tool.
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Select the Constraint icon. Select the sketch horizontal direction. Select the bottom horizontal line. Drag the mouse to place the dimension and left mouse click to complete it. e. Double-click the dimension and enter [370mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (8/18) 6. Create vertical and horizontal dimensions. (Continued) Create the horizontal dimension using the Constraint tool.
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Select the Constraint icon. Select the sketch vertical direction. Select the end point of arc. Drag the mouse to the place the dimension and left mouse click to complete its placement. j. Double-click the dimension and change its value to [390mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (9/18) 6. Create vertical and horizontal dimensions. (Continued) Dimension the horizontal line using the Constraint tool.
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k. Select the Constraint icon. l. Select the line segment. m.Drag the mouse to place the dimension. Left mouse click to complete the dimension. n. Double-click the value and change its value to [140mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (10/18) 6. Create vertical and horizontal dimensions. (Continued) Create a horizontal dimension using the Constraint tool.
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Select the Constraint icon. Select the sketch vertical direction. Select the end point of line segment. Drag the mouse to place the dimension. Left mouse click to complete the dimension. s. Double-click the value and change its value to [720mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (11/18) 6. Create vertical and horizontal dimensions. (Continued) Create a horizontal dimension using the Constraint tool.
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t. Select the Constraint icon. u. Select the sketch vertical direction. v. Select the end point of line segment. w. Drag the mouse to place the dimension. Left mouse click to complete the dimension. x. Double-click the value and change its value to [1120mm].
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6t
6u
6v
6x
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (12/18) 7. Create dimensions. Dimension the inclined line using the Constraint tool. a. Select the Constraint icon. b. Select the left inclined line. c. Drag the mouse to the place the dimension and left mouse click to complete its placement. d. Double-click the dimension and change its value to [400mm].
7a
7b
7d
Dimension the vertical distance using the Constraint tool.
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e. Select the Constraint icon. f. Select the two horizontal lines. g. Drag the mouse to place the dimension. Left mouse click to complete the dimension. h. Double-click the value and change its value to [25mm].
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7h
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (13/18) 7. Create dimensions. (Continued) Create an angular dimension between the bottom horizontal line and the adjacent line using the constraint tool. i. Select the Constraint icon. j. Select the bottom horizontal line. k. Select the angled line. l. Place the dimension. m.Edit the angular value to [105] degrees.
7i
7j
7k
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7m
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (14/18) 8. Sketch solving status and corrective action. Perform the quick analysis on sketch.
8a
8b
a. Select the Sketch Solving Status icon. b. Click Sketch Analysis icon. c. Click Diagnostic. d. Line.5 and Point.7 are UnderConstrained. e. Select Line.5 in Detailed Information, it gets highlighted in sketcher.
8c
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8d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (15/18) 8. Sketch solving status and corrective action. (Continued) Create an angular dimension between the horizontal line and Line.5 line using the constraint tool. f. g. h. i. j.
8f
Select the Constraint icon. Select the horizontal line. Select the Line as shown. Place the dimension. Edit the angular value to [15] degrees.
8h
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8j
8g
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (16/18) 8.
Sketch solving status and corrective action. (Continued) k. l. m.
All elements of the profile are green, indicating that profile is fully constrained. Select the Sketch Solving Status icon to ensure that sketch is iso-constraint. Exit the sketcher.
8k
8l
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8l
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (17/18) 9.
Modify Axis System.2 and note change in geometry. Modify parameter of Axis System.2 a. b.
c. d.
Click left mouse button two times on Axis System.3. Change Angle from [15] to [20] Observe that the sketch geometry orients and positions itself to modified Axis System.2. The profile is still constrained to Axis System.2 Click Undo Edition icon to go back to original Axis System.2 parameters. Put Axis System.3 in Hide mode.
9b
9c
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9d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (18/18) 10. Extrude the sketch. Enter Generative Shape Design workbench and extrude the sketch. a. Click Start > Shape > Generative Shape Design. b. Click Extrude icon. c. Select Sketch.3 as Profile. d. Enter [500mm] for Limit 1 e. Select OK 10a
11. Close the file without saving it. 10b 10c
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10d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Additional Sketcher Tools
Student Notes:
Create a positioned sketch Use sketch analysis tool Create a fully constrained sketch Modify Axis System Undo changes in Axis System
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Use an Axis System
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Additional Sketcher Tools
Student Notes:
Recap Exercise 15 min
In this exercise you will open an existing part that contains a positioned sketch. You will add a flange to this sketch and constrain it fully. Highlevel instructions for this exercise are provided. By the end of this exercise you will be able to: Create a positioned sketch Use transformation tools in sketcher Use re-limitation tools in sketcher Use Equivalent Dimensions Copyright DASSAULT SYSTEMES
Create a Formula
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/5) 1
1. Load Ex4B.CATPart. 2. Edit the sketch. Access the Sketcher workbench for Sketch.1 and add a flange geometry as shown. Use transformation tools (Offset) and re-limitation tools (Break, Trim) to create geometry.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/5) Create Equivalent Dimensions for thickness parameters. Multiselect all thickness dimensions as shown, and create Equivalent Dimensions of [3mm]. By this, you can have better control on the thickness constraint.
3
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3.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/5) Create Equivalent Dimensions for inner radius. Multiselect the inner radius dimensions as shown, and create Equivalent Dimensions of [3mm]. By this, you can have better control on the inner radius constraint.
4
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/5) Create Formula for outer radius. Create a formula for each of the highlighted outer radius, Outer radius = Inner radius + Thickness. By this you can have better control on outer radius. A change in the value of inner radius and/or thickness will be reflected in outer radius.
5
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5.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/5) 6.
Create a shaft. Revolve the sketch to get a solid. 6
7.
Modify value of equivalent dimensions. Modify thickness to [4] and inner radius to [5] from Relations node of feature tree.
8.
Close the file without saving it.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Additional Sketcher Tools
Student Notes:
Create a position sketch Use transformation tools in sketcher Use re-limitation tools in sketcher Use equivalent dimensions
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Create a formula
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Additional Sketcher Tools
Student Notes:
Recap Exercise 15 min
In this exercise, you will perform the sketch analysis, and create pads and pocket. You will use the tools you have learned so far, to complete the exercise with no detailed instruction. By the end of this exercise you will be able to: Solve a sketch related problem Use the sketch analysis tool and take corrective actions Create a pad
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Create a pocket
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself
Student Notes:
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1. Load Ex4C.CATPart and create pads and pocket. Perform sketch analysis and take corrective actions.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Additional Sketcher Tools
Student Notes:
Solve a sketch related problem Use the sketch analysis tool and take corrective actions Create a pad
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Create a pocket
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Create Basic Wireframe Geometry In this section you will learn how to create wireframe elements (i.e., points, lines, and planes).
Use the following steps to create the Suspension Seat: 1. 2. 3.
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4.
Create Feature Profiles and Axis System. Create Basic Wireframe Geometry. Create Shaft and Groove Features. Shell the Model.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Reference Geometry
Student Notes:
In the Part Design workbench, you have the ability to create points, lines, and planes outside of the Sketcher environment. These elements are called reference (or 3D wireframe) geometry.
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Depending on how the part was initially created, these elements can be represented in the specification tree in two ways. If the Enable hybrid design option is selected, CATIA will place these features within the main PartBody. If the Enable hybrid design option is cleared, wireframe elements are inserted under a group called a Geometrical set. Geometrical sets contain only 3D wireframe and surface elements and not solid geometry.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Accessing the Reference Elements Toolbar
Student Notes:
The toolbar is located at the bottom of the toolbars on the right-hand side of the screen. You may need to move other toolbars to view it.
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If you cannot locate the toolbar, it may be turned off. To turn on the toolbar, click View > Toolbars > Reference Elements (Extended).
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Power Input Line
Student Notes:
Instead of selecting the icons, you can use the power input line to access the 3D wireframe tools. Type: • [c:plane] to create a plane • [c:point] to create a point • [c:line] to create a line The command can be used for many tools. It is a good way to launch functions when you cannot find the icon. To view the command, hover the mouse pointer over the icon.
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For example, placing the pointer over the Line icon displays c:Line beside the power input line.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Points Points are used to mark a location on a model. They can be used as a basis for creating additional features. Use the following steps to create a point:
1
1. Click the Point icon. 2. Select the Point Type from the menu.
2
• Many types of points can be created. The required fields vary depending on the selected type. In this example, you create a Coordinates point type.
3. Specify values as required. For a coordinate point, the X, Y, and Z distances from the reference point are required. 4. Click OK to create the point. 5. The point is added to the specification tree under the Geometrical set.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Lines (1/2) Lines are created for many purposes, they can be used to define the direction for additional geometry (solid and wireframe), or as an axis for a revolved feature.
1
2
Use the following steps to create a line: 1. Click the Line icon. 2. Select the Line Type from the menu. •
Many types of lines can be created. The required fields vary depending on the selected type. In this example, you create a Point-Point type line.
3. Specify values as required. For a PointPoint line, two points are required.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Lines (2/2) Use the following steps to create a line (continued): 4.
Click OK to create the line. The line is added to the specification tree under the Geometrical set.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Planes (1/2) Planes are used to create a planar reference in a specific location. In the Part Design workbench, they are used as sketch supports.
1
Use the following steps to create a plane:
2
1. Select the Plane icon. 2. Select the Plane Type from the menu. •
Many types of planes can be created. The required fields vary depending on the selected type. In this example, you will use the Offset from plane type.
3
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3. Specify the values as required. For an Offset from plane type, a planar surface or an existing reference plane is required.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Planes (2/2) Use the following steps to create a plane (continued…): 4. Click OK to create the plane. 5. The plane is added to the specification tree under the Geometrical Set.
4
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Recommendations for Reference Elements
Student Notes:
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In this section, you will be given a recommendation to help during the creation of reference elements.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
No Reference Elements on Solid Face (1/3) It is recommended not to create reference elements that rely on solid faces, edges or dress-up features. During the design and development of a part:
Plane relies on face and edge.
Plane will be affected if edge/face disappears
a. The solid face or edge is subject to change and can disappear. b. A planar face can later become a non-planar face. c. Dress-up features can be removed for a downstream manufacturing processes. Plane will be affected if dress-up feature is removed
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Plane relies on dress-up feature.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
No Reference Elements on Solid Face (2/3) 1
In the example shown, reference element Plane.1 is offset from the highlighted solid face. 1. 2.
3.
Plane.1
Plane.1 relies on solid face. During further design and development of the part, the profile is changed such that the highlighted solid face becomes non-planar. The reference element, Plane.1 will be affected and the design becomes unstable.
2
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
No Reference Elements on Solid Face (3/3)
Student Notes:
In the example shown, reference element Line.1 is parallel to edge of fillet. 1. 2. 3.
Line.1 relies on a dress-up feature. Because of a downstream manufacturing process, the dress-up features are deactivated. The reference element, Line.1 will be affected and the design becomes unstable.
1
Line.1
2
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Create Shaft and Groove Features In this section you will learn how to create revolved features that add and remove material.
Use the following steps to create the Suspension Seat: 1. 2. 3.
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4.
Create Feature Profiles and Axis System. Create Basic Wireframe Geometry. Create Shaft and Groove Features. Shell the Model
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Creating an Axis An axis can be used as a reference to create revolved features, such as shafts and grooves (discussed later in this lesson). The sketched profile is revolved about it. An axis can also be used to create symmetrical sketched elements inside the Sketcher workbench.
2
3
4
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Use the following steps to create an axis: 1. Click the Axis icon. 2. Click to create the start point for the axis. 3. Click again to create the endpoint. 4. Using the shaft command on the profile sketch, CATIA produces a shaft using the defined axis.
1
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Dimensioning to an Axis You can define diameter and radius dimensions to an axis. This is useful while creating the profile sketches for revolved features (discussed later in this lesson). Use the following steps to create a Radius/Diameter dimension to an axis: 1. 2. 3. 4. 5.
1
3 2
Click the Constraint icon. Select the sketched element. Select the axis. Right-click and select Radius/Diameter. Click to place the dimension. 4
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Revolved Features (1/2) A revolved feature is created by revolving a 2D profile around an axis of revolution. A
In the Part Design workbench, you can create two types of revolved features: A. A shaft, which adds material. B. A groove, which removes material.
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B
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Revolved Features (2/2) Revolved features can be revolved between 0° and 360°.
A B
You can define the following limits: A. The First angle limit defines the revolution angle of the profile around the axis, starting from the profile position and orientated in the clockwise direction. B. The Second angle limit defines the revolution angle of the profile around the axis, starting from the profile position and oriented in the counterclockwise direction.
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Profile
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Axis of Revolution
Student Notes:
The axis of revolution for a revolved feature can be defined by two methods. The axis can be created inside the actual sketch containing the profile, using the Axis tool. If the axis is created inside the sketch, it will be detected automatically while defining the shaft or groove.
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If you did not create an axis in the sketch, or want to use a different axis other than the one defined in the sketch, you can define it from the Shaft/Groove definition window in the Axis selection field. Any linear element in the model (e.g., an edge of existing geometry, a 3D wireframe line, a line created in a sketch) can be used.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Shafts 2
A shaft is a revolved sketched-based feature that adds material to the model. Use the following steps to create a shaft: 1. Select the profile. 2. Click the Shaft icon. 3. If no axis is created inside the sketch, select an axis of revolution. 4. Define angle limits. 5. Click OK to complete the feature. 6. The shaft feature is added to the model.
1 3
4
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Creating Grooves Grooves are revolved features that remove material from existing features by rotating a 2D profile around an axis. The axis and the profile can be created in the same sketch or the axis can reside outside of the sketch.
1
3
Use the following steps to create a Groove feature:
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1. Select the Profile. 2. Click the Groove icon. 3. If no axis is created inside the profile sketch, select an axis of revolution. In this example, the implicit axis of the cylindrical feature is selected. 4. Define angle limits. 5. Click OK to complete the feature. 6. The Groove feature is added to the model.
2
4
5 6
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Restrictions for Revolved Features (1/2)
Student Notes:
Not every sketch can be used to create a shaft base feature. The examples shown display various sketch solutions: Axis on a profile edge:
Axis outside the profile:
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Axis cutting the profile:
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Error
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Restrictions for Revolved Features (2/2)
Student Notes:
Not every sketch can be used to create a shaft base feature. Below are some examples showing various sketch solutions (continued): Open profile:
Open profile and axis outside the profile:
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Error
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Shell the Model In this section, you will learn how to create hollow models by using the Shell operation.
Use the following steps to create the Suspension Seat: 1. 2. 3.
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4.
Create Feature Profiles and Axis System. Create Basic Wireframe Geometry. Create Shaft and Groove Features. Shell the Model
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Shelling Shelling a feature hollows out solid geometry. The shelling operation removes one or more faces from the solid and applies a constant thickness to the remaining faces. You can also apply a different thickness to the selected faces.
Faces to be removed
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Shell
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Shelling a Part (1/2) Use the following steps to shell a model where the remaining faces have a different thickness: 1. 2. 3. 4.
Select the face(s) to be removed. Click the Shell icon. Specify a wall thickness. Select on the Other Thickness Faces field. 5. Select the wall(s) that will have a different thickness.
1
2
5
3
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Shelling a Part (2/2)
6
Use the following steps to shell a model where the remaining faces have a different thickness (continued):
7
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6. To change the thickness of the Other Thickness faces, double-click the dimension directly on the model, and specify the value. Take care to select the dimension associated with the correct direction. 7. Click OK to the Parameter definition dialog box. 8. Click OK to the Shell Definition dialog box. 9. The shell feature is added to the model.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Recommendations for Shelling
Student Notes:
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In this section, you will be given a recommendation to help during the creation of shell.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Avoid Shell with Multiple Thickness
Student Notes:
It is recommended that you avoid using shells having multiple thickness value. It is not easy to visually distinguish the shell thickness values if:
2
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1. The part is large and the shell thickness values are relatively small. 2. If the bottom face is assigned another thickness value, it is not possible to distinguish it unless the hidden lines are displayed or the distance is measured.
1
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Importance of Feature Order
Student Notes:
While shelling a model, it is important to consider the feature order. The Shell operation hollows all solid features in a model. If you do not want a feature to be shelled, it must be created after the shell operation.
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For example, when a feature containing a hole is shelled, a pipe is created. If the design intent requires a hole, the shell feature needs to be created before the hole.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Thin Features (1/2) A thin feature is created by applying a constant thickness to a profile. Pads, pockets, shafts, and grooves can all be created as a thin feature. Use the Pad Definition dialog box to define its properties: • •
A thin feature can be created with a closed or open profile. Thickness can be applied to one side or both sides of the profile.
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Conf. Dep.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Thin Features (2/2) The definition dialog boxes for pads, pockets, shafts, and grooves contain a section for defining a thin feature. Use the following steps to create a thin pad: 1. Select the Thick option. 2. The dialog box expands to display additional options. 3. Specify the thickness values. Thickness 1 defines the inside thickness, and Thickness 2 defines the outside thickness. 4. Click OK to complete the feature. 5. The feature is added to the model.
5
2
Conf. Dep.
1
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
To Sum Up
Student Notes:
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In the following slides you will find a summary of the topics covered in this lesson.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Create Feature Profiles and Axis System
Student Notes:
Lesson 2 introduced you to the basic Sketcher tools and the Sketcher environment. This lesson will introduce you to the advanced Sketcher tools. Sketcher includes the following additional tools: Re-limitation tools. Transformation tools. Project 3D element tools. Analyze a sketch using the Sketch Analysis tool.
Create Shaft and Groove Features
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A revolved feature is created by revolving a 2D profile around an axis of revolution. In the Part Design workbench, you can create two types of revolved features. The axis of revolution for a revolved feature can be created inside the sketch containing the profile, using the Axis tool. If you did not create an axis in the sketch you can define it from the Shaft/Groove definition window in the Axis selection field. Any linear element in the model can be used.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Create Basic Wireframe Geometry
Student Notes:
In the Part Design workbench, you have the ability to create points, lines, and planes outside of the Sketcher environment. These elements are called reference or 3D wireframe geometry. Depending on how the part was initially created, these elements can be represented in the specification tree in two ways. If the Enable hybrid design option is selected, CATIA will place these features within the main PartBody. If the Enable hybrid design option is cleared, wireframe elements are inserted under a group called a Geometrical set. Geometrical sets contain only 3D wireframe and surface elements and not solid geometry.
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Shell the Model Shelling a feature hollows out solid geometry. The shelling operation removes one or more faces from the solid and applies a constant thickness to the remaining faces. You can also apply a different thickness to the selected faces. While shelling a model, it is important to consider the feature order. The Shell operation hollows all solid features in a model. If you do not want a feature to be shelled, it must be created after the shell operation.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Additional Sketcher Tools Operation 1
2
Relimitations: trim or extend the existing sketched geometry
1
Transformation: modify existing sketcher geometry 2
3
3D Geometry: project the existing 3D elements onto the sketch plane
3
Tools 4
Sketch Analysis: help to resolve problems with a sketch 4
Knowledge 5
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6
Formula: create Relationships between Dimensions
5
Equivalent dimensions: equates all selected parameters to a value
6
Tools 7
Axis System: used to define local coordinates
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Additional Part Design Tools Reference Elements 1
Point: creates a point in 3D space
2
Line: creates a line in 3D space
3
1 2 3
Plane: creates a plane in 3D space 4
Sketch-Based Features 4
5
6
Multi-pad: creates several pads in one operation
5
Multi-pocket: creates several pockets in one operation Shaft: helps to resolve problems with the sketch
6
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Dress-Up Features 7
Shell: removes one or more faces from the solid and applies a constant thickness to the remaining faces
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Shaft and Groove
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a simplified sprocket part by creating a revolved feature using a point, line, and sketch. Then a reference plane will be used to create an additional feature. By the end of this exercise you will be able to: Create a wireframe geometry Create a shaft feature Create a groove feature
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Create an edge fillet
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/9) 1. Create a new part. Create a new part file.
1d
a. Click File > New. b. Select Part from the list of document types. c. Select OK. d. Enter part name [Ex4D] e. Click OK.
2. Create a point. Create a point by entering coordinates. This point will be used as a reference to create a line The line is then used as the axis of revolution for a shaft feature.
1e
2a
2b
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a. Click the Point icon. If you can’t find the icon, enter [c:point] in the power input line. b. Change the point type to Coordinates. c. Enter [-4mm] for the Y value and leave all other inputs as default. d. Click OK to create the point.
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2d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/9) 3. Create a line. Create a line in the X axis direction using the created point.
3a
a. Click the Line icon. If you can’t find the icon, enter [c:line] in the power input line. b. Change the Line type to PointDirection. c. Select the Point.1 that was created previously. d. Contextual menu in Direction field and click X Axis. e. Select the Infinite End Point option for the Length Type. f. Click OK to complete the line.
3b 3c
3d
3e
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3f
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/9) 4. Create a sketch. Create a sketch that will represent the profile for a simplified sprocket. a. Right-click on the PartBody and select Define in Work Object. This ensures that any features that are created are added to the part body and not the geometrical set. b. Select the Positioned Sketch icon. c. Select the XY plane as the Reference. d. Select Origin Type as Projection point and select Point.1 as Reference. e. Select orientation type as Y axis. f. Use the Profile icon in sketcher to create the lines and arcs.
4b
4c
4d
4e
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4f
4a
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/9) 4. Create a sketch (continued). 4g
g. h. i. j.
Create an axis vertically along the V axis. Select the Constraint icon. Select the left vertical line. Select the axis. Right-click and select Radius/ Diameter from the pop-up menu. k. Left-click to place the diameter dimension. l. Create two construction circles and apply tangency constraints. m. Finish dimensioning and constraining the sketch as shown.
4h
4l
4l
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4m
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/9) 5. Create a shaft feature. Create a revolved feature using the sketch and line created previously.
5a
a. Click the Shaft icon. b. Select Sketch.1 previously created as the profile selection. c. Select inside the Axis Selection field and select Line.1. d. Make sure the first angle is [360deg] and the second angle is [0deg]. e. Click OK to complete the shaft.
5d
5b
5c
5c
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5e
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (6/9) 6.
Create a sketch. Create a sketch that will be used as the profile for a groove on the simplified sprocket. a. b. c. d. e.
Click the Positioned Sketch icon. Select the XY plane as the sketch support. Select origin type as Projection point and Point.1 as Reference. Select orientation type as X axis. Click the Profile icon in sketcher to create the lines.
6a
6b
6c
6d
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6e
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (7/9) 6.
Create a sketch (continued). f. g. h. i.
j. k. l.
Create an axis horizontally along the H axis. Click the Constraint icon. Select the top vertex. Select the axis. Right-click and select Radius/ Diameter from the contextual menu. Left-click to place the diameter dimension. Project the element of Sketch.1 and make it a construction element. Finish dimensioning and constraining the sketch as shown.
6g
6k
6k
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6l
6f
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (8/9) 7.
Create a groove feature. Create a revolved feature using the sketch and sketch axis. a. b. c. d.
7a
Click the Groove icon. Select Sketch.4 created previously as the profile. Make sure the first angle is [360deg] and the second angle is [0deg]. Click OK to complete the groove.
7c
7b
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7d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (9/9) 8.
Create two fillet features. Create edge fillet feature on the edges of groove feature. a. b. c. d. e. f. g.
Close the file without saving it.
8d
8b
8c
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9.
Click the Edge Fillet icon. Select an edge of Groove feature. Enter [10mm] as Radius. Click OK to complete the fillet. For second fillet, select other edge of Groove feature. Enter [10mm] as Radius. Click OK to complete the fillet
8a
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Shaft and Groove
Student Notes:
Create a wireframe geometry Create a shaft feature Create a groove feature
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Create a fillet feature
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Fillet and Chamfer
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a new part. Using shaft, pockets, fillets and chamfer, you will construct a damper assembly cap. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a shaft Create a pocket Create an edge fillet
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Create a chamfer
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (1/5)
Student Notes:
1. Create a new part file. Create a new part file called [Ex4E.CATPart].
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2. Create a shaft feature. Create the profile shown to construct a shaft feature.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (2/5)
Student Notes:
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3. Create a pocket feature. Create the profile shown to construct a pocket feature.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (3/5) Create a pocket feature. Create the profile shown to construct a pocket feature. Enter depth = [28mm].
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4.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (4/5) Create an edge fillet. Create an edge fillet on one edge as shown (radius = 2mm).
6.
Create a chamfer. Create a chamfer on 2 edges as shown (length = 2mm and angle = 45deg).
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5.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (5/5) Save and close the part.
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7.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Fillet and Chamfer
Student Notes:
Create a shaft feature Create a pocket feature Create a fillet feature
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Create a chamfer feature
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Shaft and Groove
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a part that contains features taught in this and the previous lessons. You will use the tools learned in this lesson to complete the exercise with no detailed instructions. By the end of this exercise you will be able to: Create a shaft feature Create edge fillets Create internal and external groove features Create a pocket feature
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Create a reference point and line Create a cone-shaped groove feature
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself
Student Notes:
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1. Create the following spool part.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Shaft and Groove
Student Notes:
Create a shaft feature Create edge fillets Create internal and external groove features Create a pocket feature Create a reference point and line
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Create a cone-shaped groove feature
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Wireframe Creation
Student Notes:
Recap Exercise 15 min
In this exercise you will create and manage wireframe geometry for a suspension control arm. You will use the tools learned in this lesson to create points, lines, and planes. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a point Create a line
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Create a plane
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/7) 1.
Load the part and prepare the environment. a. b.
2.
Load Ex4G.CATPart from the database. Define Geometric Set “SuspensionArm” as the working object.
Create a point and change properties. Create a point, a. b. c.
Click the Point icon. Select the type as On Curve. Select PinAxis as curve and [0.5] as ratio and click OK.
1b
Change name of the point to CradleArmMount. d. e.
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1b
2c
Right-click on the point created > Properties > Feature properties. Change the feature name to CradleArmMount and click OK. Copy Graphic properties of existing point using Painter.
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f.
2b
2c
2c 2e
2f
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/7) 3.
Create a point and change properties. Create a point. a. b. c.
3a
Click the Point icon. Select the type as Coordinates. Select the coordinate values as shown and click OK.
3b 3c
Change name of point to UpperBallJoint. d. e.
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f.
Right-click on the point created > Properties > Feature properties. Change the feature name to UpperBallJoint and click OK. Copy Graphic properties of existing point using Painter.
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3d 3e 3f
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/7) 4.
Create a line and change the properties. Create a line. a. b. c. d. e.
Click the Line icon. Select the type as Point-Point. Select Point1 as LowerBallJoint. Select Point2 as UpperBallJoint. Select other parameters as shown and click OK.
Change name of line to BallJointAxis. f. g.
4b 4c 4d
4e
Right-click on the line created > Properties > Feature properties. Change the feature name to BallJointAxis and click OK. Copy Graphic properties of existing line using Painter.
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h.
4a
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4g
4h
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/7) 5.
Create a line and change the properties. Create a line. a. b. c. d. e.
Click the Line icon. Select the type as Point-Point. Select Point1 as CradleArmMount. Select Point2 as LowerBallJoint. Select other parameters as shown and click OK..
Change name of line to ControlArmAxis. f. g.
5b 5c 5d
5e
Right-click Right on the line created > Properties > Feature properties. Change the feature name to ControlArmAxis and click OK. Copy Graphic properties of existing line using Painter.
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h.
5a
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5g
5h
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/7) 6.
Create a point. Create a point. a. b. c. d.
6a
Click the Point icon. Select the type as On Curve. Select ControlArmAxis as curve and [0.65] as ratio and click OK. Copy Graphic properties of existing point using Painter.
6b 6c
6c
Create this point ControlArmAxis
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6d
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (6/7) 7.
Create a plane. Create a plane. a. b. c.
8.
Create a line. Create a line. a. b. c. d. e. f. g.
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Click the Plane icon. Select the type as Through three points. Select the parameters as shown and click OK.
Click the Line icon. Select the type as Angle/Normal to curve. Select ControlArmAxis as Curve. Select the plane created in above step as support. Select the point created in step 6 as Point. Select the Angle, Start and End parameters as shown and click OK. Copy Graphic properties of existing line using Painter.
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7a
7b 7c
8a
8b 8c 8d 8e 8f
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do it Yourself (7/7) Close the part without saving it.
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9.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Wireframe Creation
Student Notes:
Create a point Create a line
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Create a plane
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Features from Wireframe
Student Notes:
Recap Exercise 20 min
In this exercise you will open an existing part that contains a sketch. You will use this sketch to create pads, fillets, and holes feature. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a pad Create a fillet
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Create a hole
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/13) 1.
Load Ex4H.CATPart from database. 1
2.
Create a pad. Create a positioned sketch on YZ plane of AxisSystem.1 and create a pad with length 1 of [15mm] and length 2 of [19mm].
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2
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/13) Create edge fillets. Create an edge fillet feature. Select the two edges of pad and apply fillet of [5mm].
3
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3.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/13) Create a pad. Create a positioned sketch on YZ plane of AxisSystem.2 and create a pad with length 1 of [30mm] and length 2 of [25mm].
4
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4.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/13) Create edge fillets. Create an edge fillet feature. Select the two edges of pad and apply a fillet of [5mm].
5
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5.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/13) Create a pad. Create a positioned sketch on Plane.2 and create a pad with length 1 of [15mm] and length 2 of [10mm].
6
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6.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (6/13) Create edge fillets. Create an edge fillet feature. Select the four edges of the pad and apply a fillet of [9mm].
7
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7.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (7/13) Create edge fillets. Create an edge fillet feature. Select the two edges as shown and apply a fillet of [25mm].
8
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8.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (8/13) Create a pad. Create a positioned sketch on XY plane of Axis System.3 and create a pad with length 1 of [22mm] and Mirrored Extent.
9
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9.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (9/13) 10
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10. Create edge fillets. Create an edge fillet feature. Select the two edges of pad and apply a fillet of [3mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (10/13) 11
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11. Create a pad. Create a positioned sketch on Plane.2 and create a pad with length 1 of [15mm] and mirrored extent.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (11/13) 12
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12. Create variable edge fillets. Create a variable edge fillet feature. Select the two edges of pad. Radius values are 5mm and 10mm. Create a variable edge fillet feature. Select the four edges as shown. Radius values are 5mm, 8mm, 10mm.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (12/13) 13
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13. Create edge fillets. Create an edge fillet feature. Select the two edges as shown and apply a fillet of [8mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (13/13) 14.
14
Face3 Face2
Face1
Close the part without saving it. Hide Axis system and Geometric Set.1. Close the part.
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15.
Create holes. Create a simple hole of diameter [35mm] on face1. Create a simple hole of diameter [20mm] on face2. Create a countersunk hole of diameter [30mm] on face3 and countersunk depth of [3mm].
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Features from Wireframe
Student Notes:
Create a pad Create a fillet
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Create a hole
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise: Shell and Holes
Student Notes:
Recap Exercise 20 min
In this exercise, you will create a Spare wheel mount, that contains features learned in this and previous lessons. You will use the tools learned in this lesson to complete the exercise with no detailed instruction. By the end of this exercise you will be able to: Create a pad Create a pocket Create a chamfer Create a fillet
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Create a shell Create a hole
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (1/9) Create a new part file. Create a new part file called [Ex4I.CATPart].
2.
Create a pad. Create a positioned sketch on XY plane and create a pad with length 1 of [350mm].
2
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1.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (2/9) Create a chamfer. Create a chamfer on two edges. Enter Length 1 as [150mm] and Angle as [45deg].
4.
Create a pocket. Create a positioned sketch on YZ plane and create a pocket of depth Upto next.
3
4
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3.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (3/9) Create a fillet. Create an edge fillet on three edges. Select the edges as shown and apply a fillet of [500mm].
6.
Create a pocket. Create a positioned sketch on a plane 350mm offset from XY plane and create a pocket of depth [300mm].
5
6
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5.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (4/9) 7.
Create fillets. Create edge fillets as shown. a. b.
8.
Create an edge fillet of [25mm] on one edge. Create an edge fillet of [55mm] on one edge.
Create a pad. Create a positioned sketch on a plane 350mm from XY plane and create a pad of length Upto next and offset [10mm].
7
7a
7b
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8
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (5/9) 9.
9
Create fillets. Create edge fillets as shown. a. b.
c.
Create an edge fillet of [100mm]on two edges. Create an edge fillet of [20mm]on one edge. Select edge to keep as shown. Create an edge fillet of [20mm]on one edge.
9a
9b
Edge to keep
Edge to fillet
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9c
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (6/9) 10.
11.
Create a pad. Create a positioned sketch on a plane 350mm from YZ plane and create a pad of length [30mm] and Mirrored extent.
10
Create Tritangent fillets. Create two tritangent fillets as shown.
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11
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (7/9) 12. Create fillets. Create edge fillets as shown. a. b.
Create an edge fillet of [8mm]on one edge. Create an edge fillet of [10mm]on one edge.
12
12a
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12b
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (8/9) 13. Load Ex4I_Step14.CATPart from database. Close the existing part without saving it and load Ex4I_Step14.CATPart.
14
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14. Create a shell. Create a shell of 1 mm thickness.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features Student Notes:
Do it Yourself (9/9) 15. Create a simple hole of diameter 80mm.
15
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16. Close the part without saving it.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Exercise Recap: Shell and Holes
Student Notes:
Create a pad Create a pocket Create a chamfer Create a fillet Create a shell
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Create a hole
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Case Study: Additional Features
Student Notes:
Recap Exercise 20 min
In this exercise you will create the case study model. Let us recall the design intent of this model: The axis of main flange must be at 5 degree from Z axis. The main flange must be at 12 degree from horizontal plane. One large hole of diameter 50mm must be created for Pillar clearance. The thickness of Seat must be 4 mm.
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There must not be any sharp corners.
Using the techniques you have learned so far, create the model without detailed instructions.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Do It Yourself: Create the Suspension Seat
Student Notes:
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Create the model using the drawing provided here.
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CATIA V5 Automotive - Chassis Lesson 4: Additional Features
Case Study Recap: Suspension Seat
Student Notes:
Create a reference geometry. Create an axis system. Create a sketched geometry. Create shafts. Create fillets. Create a pocket. Shell the model.
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Create a hole.
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