CATIA V5 Fundamentals- 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: Engine Design Intent Stages in the Process Duplicate Features Transform a Body Copy and Paste the Data Insert Data From a Catalog
Duration: Approximately 0.5 day
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Case Study: Reusing Data
Student Notes:
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The case study for this lesson is the Engine used in the Drill Press assembly (shown below). The engine is a part of the Bloc Engine sub-assembly. This case study focuses on incorporating the design intent requirements in the creation of the part.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Design Intent
Student Notes:
The engine must meet the following design intent requirements: The side fins must be created using a rectangular pattern. This avoids having to create and sketch each pocket individually.
The hole pattern must be created using a user-defined pattern. This feature can also be created as a rectangular pattern; however, a user-defined pattern will enable you to customize the hole locations.
The model must be partially created by copying pasting the features. This is one way of quickly recreating duplicate features.
The model must include features from a catalog.
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This is an easy method to retrieve data from a source that is accessible to everyone.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Stages in the Process
Student Notes:
The following steps are used to create the engine: Duplicate features. Transform a body. Copy and paste the data. Insert data from a catalog.
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1. 2. 3. 4.
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CATIA V5 Fundamentals- 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: 1. Duplicate features.
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2. Transform a body. 3. Copy and paste the data. 4. Insert data from a catalog.
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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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CATIA V5 Fundamentals- 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.
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3a
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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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1c
1d
2a
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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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9b
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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
Conf. Dep.
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Modify an instance of the pattern
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/3) You will be opening up an existing part, creating a rectangular pattern, removing some instances, exploding the pattern, and modifying some instances of the pattern.
2
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1. Open the file Ex6B.CATPart. 2. Create a rectangular pattern of Pocket.1.
1
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CATIA V5 Fundamentals- 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 Fundamentals- Lesson 6: Reusing Data
Do it Yourself (3/3)
Student Notes: Conf. Dep.
4. Explode the pattern. 5. Modify the two pockets as per the following sketch. 4
6. Save and close the file.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise Recap: Patterns
Student Notes:
Create a rectangular pattern Remove instances from a pattern Explode a pattern
Conf. Dep.
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Modify an instance of the pattern
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- Lesson 6: Reusing Data Student Notes:
Transform a Body In this section, you will understand what transformations are and how to apply them to features in a part.
Use the following steps: 1. Duplicate features.
2. Transform a body.
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3. Copy and paste the data. 4. Insert data from a catalog.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Introduction to Transformations As you create a model, you may need to occasionally move the bodies. This is accomplished using transformations. These transformations enable you to move a body by translating it along an axis, rotating it round an axis, or moving it symmetrically about a plane.
A
B
C
D
A
There are four types of transformation features: A. B. C. D.
Translate Rotate Symmetry Axis To Axis {Not covered in this course}
B
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C
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Using Transformations
Student Notes:
Transformations are used in a multi-body context. Transformations are required when you have some geometry that has been created in one location and which needs to be moved or rotated into a specific position.
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A typical example would be a body representing a standard tool set which is copied into your model and then needs to be positioned with respect to your design.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Translation (1/2)
Student Notes:
The Translation tool allows you to move a body in a linear direction. You may define the translation vector in the following three ways:
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A. Direction, distance • Moves the body along a linear direction defined by a reference, such as an edge or a plane. B. Point to point • Moves the body from one point to another. The relative position of the body with respect to the endpoint is the same, as it was with respect to the start point. C. Coordinates • Moves the body with respect to a Cartesian coordinate system.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Translation (2/2) Use the following steps to perform a Direction, distance translation:
1
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1. Select the Translation icon. 2. A warning message appears. Click Yes. 3. Define a direction by selecting an axis, line, plane or planar surface. In this example, the indicated edge was selected to define the direction. 4. Specify a distance value. 5. Click OK.
2
3
4
More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Rotation An axis and an angle are required to define a Rotate transformation.
1
Use the following steps to rotate a body: 1. Select the Rotation icon. 2. A warning message appears. Click Yes. 3. Define the Axis reference by selecting a line or axis. For example, the indicated edge was selected as the rotation axis. 4. Specify the rotation angle. 5. Click OK.
2
3
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More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Symmetry (1/2) The Symmetry option enables you to mirror a body without duplicating it. Only a single reference element is required. Any of the following may be used as a reference:
A. B. C.
A
Plane or plane surface Segment Point
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B
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Symmetry (2/2) Use the following steps to apply symmetry on a body: 1. Select the Symmetry icon. 2. A warning message appears. Click Yes. 3. Select a reference. In this example a plane was selected. 4. Click OK.
1
2
4
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3
More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Scaling The Scaling option allows to shrink or expand an entire body based on a single point as a reference. Use the following steps to create a Scaling feature: Select the Scaling icon. Select the reference point. Modify the scaling ratio. Click OK.
2 3
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1. 2. 3. 4.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Recommendations for Transformations
Student Notes:
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You will learn about the specific methods and recommendations about Transformations.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Differences in Transformations
Student Notes:
Transforming a body can be done using the Transformations tools or using the compass. How to use the compass to move items will be discussed later in the course. When you select any transformation tool, a Question dialog box will be displayed (as shown below).
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Selecting Yes will proceed to the use of the Transformations as selected. The message in the dialog box reminds you that you can also transform a body using the Compass. This is useful since you cannot use a Transformation tool to transform sketched geometry.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Scaling the Part to Define Mold “Shrink”
Student Notes:
A part gets scaled differently depending on the type of element used as the reference. If a point is used, the scaling is done using the same scaling ratio in all three directions.
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In the design of the model for an injection molded plastic part, the design part will often be scaled up, to account for material shrinkage. Depending on the material, the part may shrink by different amounts in each direction.
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CATIA V5 Fundamentals- 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: 1. Duplicate features. 2. Transform a body.
3. Copy and paste the data.
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4. Insert data from a catalog.
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CATIA V5 Fundamentals- 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 Fundamentals- 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 Fundamentals- 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 Fundamentals- Lesson 6: Reusing Data Student Notes:
Insert Data From a Catalog In this section, you will learn how to insert data from a catalog.
Use the following steps: 1. Duplicate features. 2. Transform a body. 3. Copy and paste the data.
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4. Insert data from a catalog.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Introduction to Catalogs (1/2)
Student Notes:
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Catalogs are sets of features or components which can be used as a library of information. You can retrieve these features or components to avoid recreating geometries which are frequently used.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Introduction to Catalogs (2/2) In Part mode, features can be stored as PowerCopies or user features. Conf. Dep.
A User Feature is a group of features that exists as one entity and when placed in a model, it is represented by a single feature. A PowerCopy is also a group of features that exist as one entity. However, when placed in a model the original order and the state of the features are preserved. This makes it easy to modify the features after placing the PowerCopy. .
Conf. Dep.
User Feature placed in a model
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These two are stored in the part they were created in, but also can be saved into a catalog. Instantiating the items can be done from the stored catalog or the part the PowerCopy and user feature were created in.
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PowerCopy placed in a model
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
PowerCopy (1/3) A PowerCopy can consist of a feature or group of features. It differs from a typical copy because it allows the user to address references of the copied features when pasting it into its new location. The references are controlled using inputs and parameters. Use the following steps to create a PowerCopy within a part: 1. 2.
Click Insert > Knowledge Templates > PowerCopy. The Powercopy Definition dialog box opens at the Definition tab, where you can customize the name of the PowerCopy and select the features that are to be included.
2
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Conf. Dep.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
PowerCopy (2/3) Use the following steps to create a PowerCopy within a part (continued):
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3. Select the features to include in the PowerCopy from the specification tree. As you select features, they appear on the Selected components window. Their respective references determine the inputs that are required to place the PowerCopy. 4. On the Inputs tab, you can create custom names for the inputs. Descriptive names can make placing the PowerCopy more intuitive.
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4
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
PowerCopy (3/3) Use the following steps to create a PowerCopy within a part (continued): 5.
5
6
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6.
On the Parameters tab, you can specify variable parameters. These parameter values can be made modifiable while placing the power copy. To make a parameter variable, select the parameter in the list and select the Published option. On the Icon tab, you have the ability to customize the particular type of icon, that appears next to the PowerCopy feature in the specification tree. You can also add a preview of the PowerCopy to identify the geometry.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
User Feature
Student Notes: Conf. Dep.
The process used to create user features is also used to create a PowerCopy; however, more tabs are available in the Userfeature Definition dialog box. The Outputs tab enables you to specify which feature is the main output result of the user feature. You can also add a separate feature to be included along with the main result.
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The Type tab enables you to assign a particular type to the user feature, so that it behaves like any other type, and can be searched easily in the specification tree.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Catalog Creation Once a PowerCopy or user feature is created it can be stored in the form of a catalog outside the part file in which it was created.
1
Use the following steps to create a catalog of a PowerCopy: 1. Select the PowerCopy feature in the tree. 2. Click Insert > Knowledge Templates >Save in Catalog. 3. Specify a name and location for the catalog. 4. Click OK.
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4
Conf. Dep.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Inserting Catalog Items (1/3) Once a catalog is created, its contents can be inserted into any document as long as the input requirements are met. Use the following steps to insert a catalog item:
2
Select the Catalog icon. Select the Browse another catalog icon.
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1. 2.
1
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Inserting Catalog Items (2/3) Use the following steps to insert a catalog item (continued):
4
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3. Locate the catalog file that contains the PowerCopy you want to place. 4. Select Open. 5. Open the catalog (e.g., PowerCopy). 6. Open the chapter (e.g.,3 inputs). 7. Double-click the PowerCopy.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Inserting Catalog Items (3/3) Use the following steps to insert a catalog item (continued): 8. The Insert Object dialog box opens. The inputs required to place the PowerCopy are listed and a preview of the previous reference is displayed. 9. In this example, the required reference is a surface. Select the corresponding face on the model. 10. Click OK.
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CATIA V5 Fundamentals- 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 Fundamentals- 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:
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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. 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. 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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A
B
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Transform a Body Transformations are used in a multi-body context. Transformations are required when you have some geometry that has been created in one location and which needs to be moved into a specific position. These transformations enable you to move a body by translating it along an axis, rotating it round an axis, or moving it symmetrically about a plane. The Scaling option allows to shrink or expand an entire body based on a single reference. In the design of the model for an injection molded plastic part, the design part will often be scaled up, to account for material shrinkage.
Translate
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Rotate
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Symmetry
Scaling
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CATIA V5 Fundamentals- 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:
Copy the hole
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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 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.
Paste on the flank
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Insert Data From a Catalog
Student Notes:
Catalogs are sets of frequently used features or components which are stored as a library of information. You can retrieve these features or components to avoid recreating geometries. Catalogs can be built of two types of features: A. User Feature is a group of features that exists as one entity and when placed in a model, it is represented by a single feature.
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B. PowerCopy is also a group of features that exist as one entity. However, when placed in a model the original order and the state of the features are preserved. This makes it easy to modify the features after placing the PowerCopy.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Reusing Tools Transformations 1
Translate: moves a body in a linear direction
2
Rotate: rotates a body around a selected axis
3
Symmetry: mirrors a body without duplicating it
4
Mirror: duplicates selected features across a reference plane to create mirror effect
Patterns 5
1 2 3 4
Rectangular Pattern: creates array of selected features in linear directions 5
6
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7
8
Circular Pattern: creates array of selected features in radial directions User Pattern: creates array of selected features using locations defined in an existing sketch of points Scaling: shrinks or expands an entire body based on a given ratio
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7
8
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise: Part Transformation and Catalog
Student Notes:
Recap Exercise 15 min
In this exercise, you will use the transformation techniques learned in this chapter to manipulate a robot hand part. The PartBody will be transformed relative to the part origin. You will also add features from other models using the copy and paste and catalogs. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a part symmetry Create a part rotation Create a part scale
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Cut and paste a feature between two parts Add a feature from a catalog
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/9) 1. Open the file Ex6D.CATPart. Start this exercise by opening an existing part that contains a model of a right robot hand. a. b. c. d.
1a
Click File > Open. Browse to the exercise file directory. Select Ex6D.CATPart. Click Open to open the file.
2. Perform a Symmetry operation. Use the Symmetry tool to create a left hand from the existing part. Use the ZX plane as the symmetry plane.
2a
a. Click the Symmetry icon. b. Click Yes from the dialog box that asks whether you want to keep the transformation specifications.
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2b
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (2/9) 2. Perform a Symmetry operation (continued). c. Right-click on the reference field of the Symmetry Definition dialog box and select ZX Plane. d. Click OK to complete the symmetry.
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2c
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (3/9) 3. Perform a Rotation operation. Rotate the left robot hand to point the thumb upwards.
3c
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a. Select the Rotation icon. b. Click Yes if you want to keep the transformation specifications. c. Right-click on the Axis field of the Rotate Definition dialog box and click X Axis. d. Type [180deg] for the rotation angle. e. Click OK to complete the rotation.
3a
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (4/9) 4. Copy and paste a feature from another model. Open another part and copy the mounting pocket feature. Paste it into the current model.
4b
a. Click File > Open and select the file Ex6Dreference.CATPart.
b. From the specification tree, select the Pocket.1 feature and click Copy from the contextual menu. c. Switch windows and make Ex6D.CATPart active. d. Select the mounting surface of the robot hand and click Paste from contextual menu. e. Click the Update icon to see the copied feature.
4d 4d
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4e
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (5/9) 5. Perform a Scale operation. Double the size of the robot hand using the Scale tool.
5a
a. Select on the Scale icon. b. Select the coordinate system origin as the scaling reference. c. Type [2] for the scaling Ratio. d. Click OK to complete the Scale.
5b
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5c
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (6/9)
6a
6. Insert a feature from a catalog. Open an existing catalog that contains a hole feature. Place the hole feature onto the robot mounting surface by selecting the prompted references. a. Click the Catalog icon. b. Click the Open icon and browse to the exercise files folder. c. Select MountingHoles.catalog and click Open. d. Double-click on PowerCopy in the catalog window e. Double-click 3 inputs. f. Double-click MountingHoles and a Insert Object dialog box opens.
6d
6b
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6e
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6f
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (7/9) 6. Insert a feature from a catalog (continued). g. Select the robot hand mounting surface as the Holeplacementface reference. h. Select the z axis as the vertical reference. i. Select the top circular edge of the mounting surface as the circular reference. j. Toggle the reference direction on the circular reference by clicking on the green arrow.
6h
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6i
6g
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (8/9) 6. Insert a feature from a catalog (continued). k. Click OK to finish placing the catalog hole. l. In the catalog window, double-click on the MountingHole feature again and place another hole on the other side of the robot mounting surface. m.Select on the robot hand mounting surface as the Holeplacementface reference. n. Select the z axis as the vertical reference. o. Toggle the direction of the z axis by clicking the green arrow.
6m
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6n
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (9/9) 6. Insert a feature from a catalog (continued…). p. Select the bottom circular edge of the mounting surface as the circular reference. q. Toggle the reference direction on the circular reference by clicking on the green arrow. r. Click OK to finish placing the catalog hole. s. Select Close on the catalog window.
6p
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7. Save and close the file.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise Recap: Part Transformation and Catalog
Student Notes:
Perform a symmetry on a part. Copy and paste a feature from another part. Perform a rotation on the part. Scale the part.
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Place a feature from a catalog.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise: Patterns Modifications Recap Exercise
Student Notes:
Conf. Dep.
10 min
In this exercise you will modify an existing pattern by exploding and removing instances. You will also copy and paste one of the exploded instances and make changes in the copied feature. High-level instructions for this exercise are 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 the copied features
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself (1/3) In this exercise, you will open an existing part file and manipulate instances of a pattern.
1
1. Open Ex6Econeholder.CATPart. Open an existing part file using the Open tool and investigate the features in the specification tree. 2
2
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2. Edit the pattern and remove instances. 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 will also remove references for the fillet feature. Select Edgefillet.10, select Edit, and click OK to remove the missing references. Click OK on the Edge Fillet definition dialog box.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Do it Yourself (2/3)
Student Notes: Conf. Dep.
3. Explode the pattern. Explode the pattern and notice that the fillet and shell features that were created after the pattern are not deleted.
3
4. Copy and paste an instance. Copy Pad.2 and paste it into the same part. 5. Modify the copied instance. Edit the sketch of the copied pad and move the sketch to the centre of the part. Change the pad length to [100mm]. 5
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Do it Yourself (3/3)
Student Notes:
6. Add a draft and fillet to the instance. Add an [8 degree] draft and [5mm] fillets to the copied instance. 7. Save and close the part.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise Recap: Patterns Modifications
Student Notes: Conf. Dep.
Remove pattern instances Explode pattern Copy and paste a pad instance Modify the copied pad
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Create a draft and fillets
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise: Pattern and Catalog
Student Notes:
Recap Exercise 30 min
In this exercise you will create a phone model. 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 pattern Remove instances of a pattern
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Insert a feature from a catalog
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do it Yourself
Z
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X
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Exercise Recap: Pattern and Catalog
Student Notes:
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Create a pattern Remove instances of a pattern Insert a pocket feature from a catalog
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Case Study: Reusing Data
Student Notes:
Recap Exercise 35 min
You will practice what you have learned by completing the case study model using only a detailed drawing and hints as guidance. In this exercise you will create the case study model. Recall the design intent of this model: The side fins should be created by a rectangular pattern The hole pattern should be created by a user pattern The model should be partially created by copying and pasting features
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The model should include features from a catalog
Using the techniques discussed so far, create the model without detailed instructions.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Do It Yourself: Drawing of the Engine (1/3)
Student Notes:
The following steps offer useful hints to guide you through the creation of the engine part: 1. Open CaseStudy.CATPart. 2. Create a rectangular pattern for the side fins.
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3. Create a user pattern for the hole pattern.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data Student Notes:
Do It Yourself: Drawing of the Engine (2/3) The following steps offer useful hints to guide you through the creation of the engine part (continued): Conf. Dep.
4. Create copies of Pad.3, Pad.5 and Hole.1 one after the other and paste them one by one into the model. 5. Move the pasted features into a separate body by selecting the features, and selecting Insert In New.. from the contextual menu.
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6. Translate the body to a distance of [40] in the X direction.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Do It Yourself: Drawing of the Engine (3/3)
Student Notes:
The following steps offer useful hints to guide you through the creation of the engine part (continued):
7. Insert data from the supplied CaseStudy.catalog.
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8. Reorder the catalog Shaft feature to occur before Pocket.4 in order to apply the pocket feature to the catalog geometry.
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CATIA V5 Fundamentals- Lesson 6: Reusing Data
Case Study: Engine Recap
Student Notes:
The side fins should be created by a rectangular pattern The hole pattern should be created by a userdefined pattern The model should be partially created by copying and pasting the features
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The model should include features from a catalog
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