Pocket

Creating a pocket consists in extruding a profile or a surface and removing the material resulting from the extrusion. The application lets you choose the limits of creation as well as the direction of extrusion. The limits you can use are the same as those available for creating pads. To know how to use them, see Up to Next Pads , Up to Last Pads , Up to Plane Pads, Up to Surface Pads.

This task first shows you how to create a pocket, that is a cavity, in an already existing part, then you will edit this pocket to remove the material surrounding the initial profile.

Open the Pocket1.CATPart document.

Select the profile to extrude, that is Sketch.2.

About Profiles

You can use profiles sketched in the Sketcher or planar geometrical elements created in the Generative Shape Design workbench (except for lines).

You can create pockets from sketches including several closed profiles. These profiles must not intersect.

You can select diverse elements constituting a sketch too. For more information, refer to Using the Sub-Elements of a Sketch.

Instead of selecting profiles, you can now select surfaces created in the Generative Shape Design workbench, non-planar faces and even CATIA V4 . To know how to create a pocket from a surface, refer to Pads or Pockets from Surfaces.

Click the Pocket icon

The Pocket Definition dialog box is displayed and the application previews a pocket.

If you launch the Pocket command with no profile previously defined, just click the icon

to access the Sketcher and sketch the profile you need.

You can define a specific depth for your pocket or set one of these options:

	up to next
	up to last
	up to plane
	up to surface

If you wish to use the Up to plane or Up to surface option, you can then define an offset between the limit plane (or surface) and the bottom of the pocket. For more information, refer to Up to Surface Pad.

To define a specific depth, set the Type parameter to Dimension, and enter 30mm.

Alternatively, select LIM1 manipulator and drag it downwards to 30.

If you are not satisfied with the profile you selected, note that you can click the Selection field and select another sketch.

Clicking the icon

opens the Sketcher. You can then edit the profile to modify your pocket. Once you have done your modifications, you just need to quit the Sketcher. The Pocket dialog box reappears to let you finish your design.

By default, if you extrude a profile, the application extrudes normal to the plane used to create the profile. To specify another direction, click the More button to display the whole Pocket Definition dialog box, uncheck the Normal to sketch option and select a new creation direction.

If you extrude a geometrical element created in Generative Shape Design, you need to select a direction.

		To know how to use the "Thick" option, refer to "Thin Solids".
		Optionally click Preview to see the result.
	4.	Click OK to create the pocket. The specification tree indicates this creation. This is your pocket:
	5.	Double-click Pocket.1 to edit it. As the application now lets you choose the portion of material to be kept, you are going to remove all the material surrounding the initial profile. The option Reverse side lets you choose between removing the material defined within the profile, which is the application's default behavior, or the material surrounding the profile.
	6.	Click the Reverse side button or alternatively click the arrow as shown:

	7.	The arrow now indicates the opposite direction.
	8.	Click OK to confirm. The application has removed the material around the profile.

A Few Notes About Pockets

The application allows you to create pockets from open profiles provided existing geometry can trim the pockets.

If your insert a new body and create a pocket as the first feature of this body, the application creates material:

Pockets can also be created from sketches including several profiles. These profiles must not intersect.

In the following example, the initial sketch is made of eight profiles. Applying the Pocket command on this sketch lets you create eight pockets:

The 'Up to next' limit is the first face the application detects while extruding the profile. This face must stops the whole extrusion, not only a portion of it, and the hole goes thru material, as shown in the figure below:

Preview

Result

When using the 'Up to Surface' option, remember that if the selected surface partly stops the extrusion, the application continues to extrude the profile until it meets a surface that can fully stop the operation.