CATIA V5-6R2015 Basics Part II: Part Modeling by Tutorial Books

CATIA V5-6R2015

Basics Part II

Tutorial Books

Copyright 2015 by Kishore

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Contents

Sketch-Based features are used to create basic and simple parts. Most of the times, they form the base for complex parts as well. These features are easy to create and require a single sketch. Now, you will learn the commands to create these features.

The topics covered in this chapter are:

• Pad Features
• Shaft Feature
• Pocket Features
• Reference Planes
• More Options in the Pad and Shaft commands
• View commands

Pad

Pad is the process of taking a two-dimensional profile and converting it into 3D feature by giving it some thickness. A simple example of this would be taking a circle and converting it into a cylinder.

1. Once you have created a sketch profile or profiles you want to Pad , activate the Pad command (On the Sketch-Based Features toolbar, click Pads drop-down > Pad (or) click Insert > Sketch-Based Features > Pad on the Menu).
2. Click on the sketch profile to add thickness to it.

1. On the Pad Definition dialog, type-in a value in the Length box.

1. If you want to add equal thickness on both sides of the sketch, then check the Mirror extent option.
2. Click the Preview button to view how the model would look when completed.

1. Click OK to complete the Pad feature.

While creating a Pad feature, CATIA adds material in the direction normal to the sketch.

If you want to manually define the direction in which the material will be added, then click the More button on the Pad Definition dialog. Click in the Reference selection box and select a line.

Shaft

Revolving is the process of taking a two-dimensional profile and revolving it about a centerline to create a 3D geometry (shapes that are axially symmetric). While creating a sketch for the Shaft feature, it is important to think about the cross-sectional shape that will define the 3D geometry once it is revolved about an axis. For instance, the following geometry has a hole in the center.

This could be created with a separate Pocket or Hole feature. But in order to make that hole part of the Shaft feature, you need to sketch the axis of revolution so that it leaves a space between the profile and the axis.

1. After completing the sketch, activate the Shaft command (On the Profile toolbar, click the Shaft icon (or) click Insert > Sketch-Based Features > Shaft on the Menu).
2. The sketch will be revolved by full 360 degrees.

1. If you want to enter an angle of revolution, type-in a value in the First Angle box.

1. On the dialog, click OK to complete the Shaft feature.

Project 3D Elements

This command projects the edges of a 3D geometry onto a sketch plane.

1. Activate the Sketcher Workbench by selecting a plane or model face.
2. On the Operations toolbar, click 3D Geometry drop-down > Project 3D Elements (or) click I nsert > Operations > 3D Geometry > Project 3D Elements on the Menu.
3. Click on the edges of the model geometry to project them on to the sketch plane.
4. Click OK on the Projection dialog.

The projected element will be yellow in color and fully constrained. If you want to convert it into a normal sketch element, then right click on it and select Mark.object > Isolate .

1. Complete the sketch and exit the workbench.

The Pocket command

This command removes material from the geometry by extruding a sketch. It functions on the same lines of the Pad command.

1. Draw a sketch on a plane or a model face.
2. On the Sketch-Based Features toolbar, click the Pocket icon (or) click Insert > Sketch-Based Features > Pocket on the Menu.
3. Select the sketch.

1. On the Pocket Definition dialog, type-in a value in the Depth box and click Preview .