CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Reusing Data
Student Notes:
In this lesson, you will learn how to create parts by reusing existing data instead of creating new features.
Lesson Contents:
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Case Study: Sprocket Design Intent Stages in the Process Duplicate Features Copy and Paste Data Create the Published Elements
Duration: Approximately 0.5 day
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Case Study: Reusing Data
Student Notes:
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The case study for this lesson is the Sprocket used in the Front Suspension and Engine assembly shown below. The Sprocket is a part of the Powertrain sub-assembly. The focus of this case study is the creation of a features that incorporate the design intent for the part.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Design Intent (1/2) The Sprocket must meet the following design intent requirements: The outer diameter must be 125mm. Create a profile of the sprocket teeth with outer diameter of 125mm.
The inner diameter must be 110mm.
A
Create a profile of the sprocket teeth with inner diameter of 110mm.
The number of teeth of sprocket must be 36. Create a circular pattern with 36 number of instances.
The mounting hole (A) must have a diameter of 30mm.
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Create a main profile of the sprocket with inner diameter of 30mm.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Design Intent (2/2) The Sprocket must meet the following design intent requirements: The three mounting holes (B) must have a diameter of 5mm and be spaced at predefined angles around the central axis.
C
Create a hole of diameter 5mm and a pattern with angular spacing of 80 and 70 degrees.
A
The mounting hole (C) must have a diameter of 11mm. Create a hole of diameter of 11mm.
Publish axis of hole A, hole B and rear face of the sprocket.
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Use Publication to publish these elements.
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B
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Stages in the Process
Student Notes:
The following steps are used to create the Sprocket: 1. Create shaft. 2. Create pocket 3. Create circular pattern. 4. Create groove. 5. Create fillet. 6. Create hole.
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7. Publish geometry.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Duplicate Features In this section, you will understand what duplicate features are and how to create them within a part.
Use the following steps to create the Sprocket: 1.
Copy Paste Create the Published Elements
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2. 3.
Duplicate Features.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Introduction to Duplicating Features CATIA allows the creation of various types of features; however, some features occur multiple times in a model. In order to avoid creation of each feature individually, duplication tools are used. Two types are discussed in this lesson:
A B
A. Mirror • If you create one half of a symmetrical part, then using the Mirror tool you can duplicate the opposite side.
B. Pattern
Mirror
Rectangular pattern
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• Using Patterns you can create several identical features from an existing one, and simultaneously position them on a part.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Mirror While designing parts, it is better to identify areas of symmetry before you start making the model. This enables you to plan and reduce the amount of work needed by only building half of the part, then using the Mirror tool to build the other side. You can also mirror individual features.
1
2
Use the following steps to create a mirror feature: 3
2
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1. Select the Mirror icon. 2. Select a datum plane or planar surface which defines the plane of symmetry. 3. Click OK.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Patterns CATIA allows you to define three different types of patterns within the Part Design workbench: A. Rectangular pattern B. Circular pattern C. User pattern
A
B B
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A
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Rectangular Patterns (1/2) 1
Rectangular patterns are linear and can be created in two directions. 2
Use the following steps to create a rectangular pattern: 1. Select the Rectangular Pattern icon. 2. Select the feature to be patterned. In this example, a pocket is selected. 3. Select the Parameters type from the list, to define how the instances of the pattern are defined.
4
a. There are four Parameters options to define a pattern.
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4. Click inside the Reference element field and select a reference (i.e., an axis, plane, line, planar surface) to define the first direction of the pattern.
4
3a
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Rectangular Patterns (2/2) Use the following steps to create a rectangular pattern (continued):
5
5. Select Second Direction tab and define the pattern in this direction using the same steps. 6. Click OK.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Circular Patterns (1/3)
Student Notes:
1
Circular patterns are radial and defined about an axis. The axis reference can also be defined by an edge or a normal vector of a planar surface or datum plane. 2 Conf. Dep.
Use the following steps to create a circular pattern: 1. Select the feature to be patterned. In this example, a pad is selected. 2. Select the Circular Pattern icon. 3. Select the Parameters type from the list, to define how the instances of the pattern are defined. a. There are five Parameters options to define a pattern.
4
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4. Click inside the Reference element field and select the direction reference (an axis, plane, line, planar surface). In this example the face of the pad is the reference element.
3a
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Circular Patterns (2/3) Conf. Dep.
Use the following steps to create a circular pattern (continued): 5. Specify the number of instances and angular spacing. 6. Click OK to create the pattern.
5
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Circular Patterns (3/3)
Student Notes: Conf. Dep.
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The Crown Definition tab allows the feature(s) to be patterned in a radial direction as well as around an axis. There are three Parameters options to define the crown.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
User Patterns (1/2) User patterns use an existing sketch of points to define the location of the instances. Use the following steps to create a user pattern: 1. Select the feature(s) to be patterned. In this example, the stiffener feature is patterned. 2. Select the User Pattern icon. 3. Pick a sketch of points to define the instance positions.
1
2
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
User Patterns (2/2) Use the following steps to create a user pattern (continued): 4. Click OK.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Recommendations for Patterns
Student Notes:
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In this section you will find information regarding pattern creation.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exploding a Pattern
Student Notes: Conf. Dep.
After a pattern is created, individual instances may need to be modified such that, they are independent from each other and the original source feature. The instances of the pattern can be separated into individual features using the Explode option.
1
Use the following steps to explode a pattern: 1. Select the pattern in the specification tree. 2. Right-click. 3. Select object > Explode…
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Removing Individual Instances in a Pattern
Student Notes:
When you create a pattern, CATIA gives you the option to remove individual instances before the pattern is completed.
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While the Pattern definition window is open, click on the center points of the instances that you do not want to keep. To activate an instance you have removed, click on its center point again.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Keep Specification When you pattern a feature, the pattern instances appear identical to the original feature. Use the Keep specifications option to maintain the design intent of the original.
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In the example below, the pad is created with the Up to Surface depth option. If the Keep specifications option is not selected, the pattern instances retain the state of the original feature during pattern creation.
Without the option set
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With the option set
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Contextual Menus As mentioned in previous lessons CATIA has contextual menus. Here are some examples available when creating Patterns: A. You can create a line or plane to define Reference Direction of a pattern using the contextual menu on the Reference element.
A
B. You can define the spacing of the pattern by creating a formula using the contextual menu on the Spacing.
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B
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise: Patterns
Student Notes:
Recap Exercise 30min
In this exercise, you will create a part that will contain a circular and a user pattern. The part will be mirrored to create a symmetrical model. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a circular pattern Create a user pattern
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Create a mirror feature
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/10) 1. Create a new part. To create a new part file select Part from the New dialog box. a. b. c. d.
Click File > New. Choose Part from the New dialog box. Click OK. Accept the default file name and click OK.
2. Launch the Sketcher workbench. Sketches are created in the Sketcher workbench. It is accessed by choosing a sketch support and selecting the Positioned Sketch icon.
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a. Select ZX plane as the sketch support. b. Click the Positioned Sketch icon.
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1b
1c
1d
2a
2b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Do it Yourself (2/10)
Student Notes:
3. Sketch the profile. This sketch is used as the profile for a shaft feature. a. Select the Profile icon. b. Sketch and constrain the profile as shown below. c. Exit Sketcher.
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3b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (3/10) 4. Create a shaft. Use the sketch as the profile for a shaft feature. a. b. c. d.
4b
Select the sketch created in step 3. Select the Shaft icon. Specify [360] for the First angle. Click OK. 4c
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4d
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (4/10) 5. Create a hole. Using a hole feature instead of a pocket gives you more flexibility in terms of type and thread definition. a. Select the Hole icon. b. Multi-select the surface and the edge as shown. c. Set the depth to Up to Next. d. Specify [16mm] as the diameter. e. Select the Type tab and set to Countersunk. f. Specify [4mm] and [50deg] for the depth and angle. g. Click OK.
5a
5b
5c
5e
5d
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5f
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5g
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (5/10) 6a
6. Create a hole. Create a simple hole that will be patterned later. a. b. c. d. e.
Select the Hole icon. Select the surface shown. Set the definition as shown. Constrain the position sketch as shown. Click OK.
6b
6e
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6d
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (6/10) 7. Create a circular pattern. Create a circular pattern of the hole feature.
7b
a. b. c. d. e.
Select the hole feature. Select the Circular Pattern icon. Specify [4] for the number of instances. Specify [90deg] for the angular spacing. Click inside the Reference Element field and select the shaft face as the reference element. f. Click OK.
7c 7d
7f
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7e
Conf. Dep.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (7/10) 8a
8. Create a sketch. Create a sketch of points that will be used as a reference for a User Pattern later.
8b
a. Select the Positioned Sketch icon. b. Select the surface to define the sketch support. c. Create and constrain three points as shown. d. Exit sketcher.
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8c
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (8/10) 9. Create a pocket. Create a pocket to define the feature that will be duplicated with a user pattern. This could have also been created using a hole feature. Select the Positioned Sketch icon. Select the surface. Create and constrain the profile. Select the Pocket icon. Set the following pocket definition Click OK.
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a. b. c. d. e. f.
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9a
9b
9d
9f
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (9/10) 10. Create a user pattern. Use the sketch of points to define the location of the pockets. a. b. c. d.
10b
Select the pocket. Select the User Pattern icon. Select the sketch of points. Click OK. 10c
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10d
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (10/10) 11. Create a mirror feature Mirror the entire part to create a symmetrical model.
11a
a. Select the Mirror icon. b. Select the YZ plane. c. Click OK. 11c
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12. Close the file without saving it.
11b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise Recap: Patterns
Student Notes:
Create a circular pattern Create a user pattern
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Create a mirror feature
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise: Patterns
Student Notes:
Recap Exercise 15 min
In this exercise you will practice creating and manipulating patterns. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a rectangular pattern Remove instances from a pattern Explode a pattern
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Modify an instance of the pattern
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/3) Load Ex6B.CATPart from database.
2.
Create a rectangular pattern of Pocket.1.
1
2
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1.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Do it Yourself (2/3)
Student Notes:
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3. Remove the following instances from the pattern.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (3/3) 4. Explode the pattern. 5. Modify the two pockets as per the following sketch. 6. Close the file without saving it.
4
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise Recap: Patterns
Student Notes:
Create a rectangular pattern Remove instances from a pattern Explode a pattern
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Modify an instance of the pattern
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise: Patterns
Student Notes:
Recap Exercise 25 min
In this exercise you will use the newly acquired skills to create a part containing a circular pattern. You will use the tools used in the previous exercises to complete this exercise with no detailed instructions. By the end of this exercise you will be able to: Create a new part
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Create a circular pattern
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Do it Yourself
Student Notes:
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Create the part as shown below:
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise Recap: Patterns
Student Notes:
Create a new part
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Create a circular pattern
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Copy-Paste In this section, you will understand how to duplicate features by copying and pasting them within a part.
Use the following steps to create the Sprocket: 1.
Duplicate Features.
3.
Create the Published Elements
Copy Paste
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2.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Copy and Paste Data (1/3)
Student Notes:
Features can also be duplicated by copying and pasting them within a part. The pasted feature is identical and completely independent of the original feature. Use the following steps to copy and paste: Select the feature to be copied. Right-click. Select Copy.
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1. 2. 3.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Copy and Paste Data (2/3) Use the following steps to perform a copy and paste (continued): 4.
4
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5. 6.
Select the PartBody in which the feature has to be pasted. Right-click. Select Paste. As mentioned earlier, the feature which is pasted is a duplication of the original feature. The placement on the model is also the same as the original feature. Therefore, its position needs to be modified.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Copy and Paste Data (3/3) Use the following steps to perform a copy and paste (continued): 7. 8. 9.
Double-click sketch.3. Modify its position. Exit Sketcher.
7
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Create the Published Elements In this section, you will learn what published geometry is and how to create it.
Use the following steps to create the Sprocket: 1. 2.
Create the Published Elements
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3.
Duplicate Features. Copy Paste
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Introduction to Publishing Geometry
Student Notes:
Publishing geometrical elements is the process of making geometrical features available to different users. Although not essential, publishing geometry and parameters in a skeleton model is suggested to help control the external references created.
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Publishing elements are not just used when applying the skeleton method. Consider using published elements anytime you want to control external references.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Why Publish Geometry?
Student Notes:
Publishing geometry has many benefits such as: •
• •
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•
To label geometry and give it a name that can be easily recognized (particularly in the case of publishing edges, faces, etc.) To make particular geometry easier to access from the specification tree. To control external references. An option is available that lets you only select as external reference only the published elements. To ease replacement of one component of the assembly by another. Published elements that have the same names are automatically reconnected. Without published elements, you would have to reconnect them one by one.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
What Kind of Geometry Can be Published?
Student Notes:
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Many types of geometries can published : •
Wireframe features (points, lines, curves, planes)
•
Whole sketches
•
Bodies (PartBody, other body)
•
Part design features (pad, pocket, hole etc.)
•
Generative Shape Design features (extrudes surfaces, offsets, joins etc.)
•
Free Style Design features (planar patches, curves etc.)
•
Sub elements of all geometrical elements (faces, edges, vertices etc.)
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Published Elements in the Tree Published elements can identified in the specification tree.
A B
Ca Cb
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A. The tree displays names of published elements under the components Publication node. B. The green gear on a component icon indicates that the component has been designed using external references. C. When a published element is used, it is denoted in the external references node. a. Elements that are updated are denoted by the letter P in a cyan color. b. Published elements that are not synchronized are denoted by a P in a yellow circle.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Publishing Geometry (1/2) Use the following steps to publish geometry:
1
1. Activate the components that contains the geometry to be published. 2. Click Tools > Publications. 3. Select the geometrical element to publish. 4. The selected geometry is added to the publications window.
4
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Publishing Geometry (2/2) Use the following steps to publish geometry (continued): 5. To rename the published elements, select in the row with the element to rename to activate it. Select in the field again to edit the name. 6. Repeat step 3 to 5 to publish other elements. 7. Click on OK to validate. 8. The published elements are displayed under the publication node of the components.
5
6
7
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Changing a Published Element If necessary, the geometrical element referenced by a publication can be replaced using the following steps: 1. 2. 3. 4. 5. 6. 7.
1
Activate the component containing the published geometry to be replaced. Click Tools > Publications. Select the publication to replace. The current geometrical element highlights on the model Select the replacing geometrical element. Select Yes from the Replace Element dialog box. Click OK to close the publications dialog box.
3
7
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4
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
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 6: Reusing Data Student Notes:
Duplicate Features In order to avoid creation of each feature individually, duplication tools are used. Two types of duplication features: A. Mirror: While designing parts, it is better to identify areas of symmetry before you start making the model. This enables you to plan and reduce the amount of work needed by only building half of the part, then using the Mirror tool to build the other side.
A
B. Pattern: Using Patterns you can create several identical features from an existing one and simultaneously position them on a part. Three different types of patterns are: i. Rectangular patterns are linear and can be created in two directions.
B
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ii. Circular patterns are radial and defined about an axis. iii. User patterns use an existing sketch of points to define the location of the instances.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Copy and Paste the Data Features can be duplicated by copying and pasting them within a part. The pasted feature is identical and completely independent of the original feature. To copy and paste, you can use any one of the following techniques:
Paste on the flank
Click Copy then Paste in the Standard toolbar Select Edit > Copy then Edit > Paste Press Ctrl+C and then Ctrl+V Right-click then select Copy and Paste, or
Copy the hole
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In the geometry area or the specification tree, press and hold down the Ctrl key and drag the selection and drop in the geometry area or the specification tree.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Create the Published Elements
Student Notes:
Publishing geometrical elements is the process of making geometrical features available to different users. Publishing geometry and parameters in a skeleton model is suggested to help control the external references created. The benefits of using publishing geometry are as given below: Label geometry to give it a name that can be easily recognized (particularly in the case of publishing edges, faces, etc.). To make particular geometry easier to access from the specification tree. Control external references. An option is available that lets you only select as external reference only the published elements.
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Easy replacement of one feature of the part with another.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Main Tools Transformation Features 1
Mirror: duplicates one side of a symmetrical part about a given reference plane.
2
Rectangular Pattern: creates a linear pattern in two directions.
3
Circular Pattern: creates a pattern in a circular manner about specified axis. Insert in New Body: projects the existing 3D elements onto the sketch plane.
2 3 4
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4
1
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise: Features Duplication
Student Notes:
Recap Exercise 15 min
In this exercise, you will modify an existing pattern by exploding and removing instances of a pattern. You will also copy and paste one of the exploded instances and make changes to the copied feature. Detailed instruction for this exercise is provided. By the end of this exercise you will be able to: Explode a pattern Remove instances of the pattern Copy and paste features
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Modify copied features Publish an axis
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/6) 1.
Search and Load the part. Load Ex6D.CATPart from database.
2.
Remove instances of a pattern. Remove some of the instance of the pattern. a.
b.
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c.
2a
Edit the pattern and remove two instances of the pattern by clicking on the pattern instance dots. Note that the fillet feature will fail because it was created after the pattern feature. Removing instances of the pattern also removes references for the fillet feature. Select Edgefillet.10, select Edit, and select OK to remove the missing references. Select OK to the Edge Fillet definition dialog box.
2b
2
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2c
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (2/6) 3.
Explode the pattern. Explode the pattern to separate the instances. a. b.
3a
Right-click on RectPattern.1 > RectPattern.1 object > Explode. Notice that the fillet and shell feature, that were created after the pattern, are not deleted.
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3b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (3/6) 4.
Copy and paste an instance. Copy Pad.2 and paste it in PartBody. a. b. c.
Right-click on Pad.2 > Copy. Right-click on PartBody > Paste. The new pad appears last in the feature tree.
4a
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4b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (4/6) 5.
Modify the sketch of copied instance. Edit the sketch for the copied pad and move the sketch towards the middle of the part. Edit the sketch of pasted pad to
5a
enter a sketcher workbench. a. Change horizontal dimension to [200mm]. b. Exit sketcher.
6.
Modify the pad length. Edit the copied pad and change the pad length to [100mm]. a. b.
Edit the pad. Change Length1 to [100mm] 6b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (5/6) 7.
Add a draft to the instance. Create a draft feature on the pad. a. b. c.
7a
Click Draft icon. Select Pad face as a fact to draft and a suitable neutral element. Enter Angle value as [8degree].
7b
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7b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Do it Yourself (6/6) 8.
Add an edge fillet. Create an edge fillet on the drafted pad. a. b. c.
Click Edge Fillet icon. Select the face as shown. Enter Radius value as [5mm].
8a
8
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8b
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise Recap: Features Duplication
Student Notes:
Remove pattern instances Explode the pattern Copy and paste a pad instance Modify the copied pad Create a draft and fillets
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Publish an axis
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise: Wireframe and Publication
Student Notes:
Recap Exercise 10 min
In this exercise you will create wireframe geometry for a piston and publish it. You will use the tools you have 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 wireframe geometry Change properties of elements
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Publish elements
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Do it Yourself
Student Notes:
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1. Load Ex6E.CATPart from database and create the wireframe geometry (shown in dark blue color) using this drawing. Rename and publish these elements.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Exercise Recap: Wireframe and Publication
Student Notes:
Create wireframe geometry Change properties of elements
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Publish elements
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data Student Notes:
Case Study: Reusing Data Recap Exercise 35 min
In this exercise you will create the case study model. Let us recall the design intent of this model: The outer diameter must be 125mm.
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The inner diameter must be 110mm. C
The number of teeth of sprocket must be 36. The mounting hole (A) must have a diameter of 30mm. The three mounting holes (B) must have a diameter of 5mm and be spaced at pre-defined angles around the central axis. The mounting hole (C) must have a diameter of 11mm. Publish axis of hole (A), hole (B) and rear face of the sprocket.
A
Using the techniques you have learned so far, create the model without detailed instructions.
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B
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Do It Yourself: Create the Sprocket
Student Notes:
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Create a part using the drawing provided here and publish geometrical elements.
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CATIA V5 Automotive - Chassis Lesson 6: Reusing Data
Case Study Recap: Sprocket
Student Notes:
Create a shaft Create a pocket Create a circular pattern Create a groove Create an edge fillet Create a hole
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Publish the geometry
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