Pad

Creating a pad means extruding a profile or a surface in one or two directions. The application lets you choose the limits of creation as well as the direction of extrusion.

This task shows you how to create a basic pad using a closed profile, the Dimension and Mirrored extent options.

Open the Pad1.CATPart document.

1. Select Sketch.1 as the profile to be extruded.

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

If you launch the Pad command with no profile previously defined, just access the Sketcher by clicking the icon

available in the dialog box and sketch the profile you need.

You can now select surfaces, non-planar faces and even CATIA V4 surfaces. For more information, pleaser refer to "Pads from Surfaces".

By default, if you extrude a profile, the application extrudes normal to the plane used to create the profile. To see how to change the extrusion direction, refer to Pad not Normal to Sketch Plane.

If you extrude a geometrical element created in the Generative Shape Design workbench, you need to select an element defining the direction because there is no default direction.

Click the Pad icon

The Pad Definition dialog box appears and the application previews the pad to be created.

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

You will notice that by default, the application specifies the length of your pad. But you can use the following options too:

	Up to Next
	Up to Last
	Up to Plane
	Up to Surface

3. Enter 40 in the Length field to increase the length value.

You can increase or decrease length values by dragging LIM1 or LIM2 manipulators.

The length value cannot exceed 1 000 000 mm.

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

To know how to use the "Thick" option, refer to "Thin Solids".

The button Reverse side applies for open profiles only. This option lets you choose which side of the profile is to be extruded.

Click the Mirrored extent option to extrude the profile in the opposite direction using the same length value.

If you wish to define another length for this direction, you do not have to click the Mirrored extent button. Just click the More button and define the second limit.

5. Click Preview to see the result.

Click OK.

The pad is created. The specification tree indicates that it has been created.

A Few Notes About Pads

The application allows you to create pads from open profiles provided existing geometry can trim the pads. The pad below has been created from an open profile which both endpoints were stretched onto the inner vertical faces of the hexagon. The option used for Limit 1 is "Up to next". The inner bottom face of the hexagon then stops the extrusion. Conversely, the "Up to next" option could not be used for Limit2.

Preview

Result

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

In the following example, the sketch to be extruded is defined by a square and a circle. Applying the Pad command on this sketch lets you obtain a cavity:

Preview

Result

Before clicking the Pad command, ensure that the profile to be used is not tangent with itself.