Creating Multi-Pads

You can extrude multiple profiles belonging to a same sketch using different length values. The multi-pad capability lets you do this at one time.

Note: Depending on your role, you may not have access to this functionality.

Before you begin: To perform this task, create a sketch made of seven closed profiles similar to the one below.
See Also
About Pads
Creating Pads
Using the Sub-Elements of a Sketch
Location of Sketches in the Tree (Hybrid Design)
  1. From the Model section of the action bar, click Multi-Pad .
  2. Select the sketch that contains the profiles to be extruded.
    Important: All profiles must be closed and must not intersect. In case a profile would be open, the app would not take it into account.

    The Multi-Pad.xdialog box appears and the profiles are highlighted in green. For each of them, you can drag associated handles to define the extrusion value.

    The arrow normal to the sketch indicates the proposed extrusion direction. To reverse it, you need to click it.



    The Multi-Pad Definition dialog box displays the number of domains to be extruded.

  3. In the Domain column, select the serial number for the respective profiles to be extruded..
  4. In the Lim 1 and Lim 2 columns of the respective domain, enter the length values in respective directions.
  5. You need to repeat the operation for each extrusion domain by entering the values of your choice.
    Tip: For complex sketches, the Preview button proves to be quite useful.
  6. Optional: In the Direction box, select the reference element to change the direction of extrusion.
  7. Optional: Select to switch the direction of extrusion.

The multi-pad (identified as Multi-Pad.x) is added to the tree.