Edit Parts with Other Parts - Welding Groove

You can fit parts together in an assembly.

For example, a standard welding groove can be added between sheet metal parts with the Boolean function.

An example of editing with parts.

1. The starting point is an assembly model, which includes the following:
   • Jig part

     

   • Finished plate section modeled with the Jig.

     

2. Select the context-sensitive function New Part, and name the part.
3. Select the context-sensitive function Copy Surface.

   Copy a Face

4. Select the Tangential Shelling search.
   
5. Select the surface.

   

6. Select Confirm.
7. Define the properties in the Copying a Face dialog box.
   • In is selected.
   • Select To Volume.
8. Click OK.
9. Define the properties in the Surface Chain Data dialog box.
   • Change to Sheet Metal Part is selected.
   • Define the sheet thickness.
   • Select the material by clicking the Select button.
10. Click OK.
11. Exit the part modeling mode. Select Confirm.

    You can hide the Jig part to see the new part in more detail. Select the part and press the H key.

    

12. When nothing is selected, select the context-sensitive function Boolean.
13. Define in the Boolean dialog box.
    • Operation Subtract.
    • Offset Value - In the example, the offset value defines the welding groove. Enter the value. The welding groove is a smaller volume than the plate part.
    • Select Only the Biggest Volume Stays.
    • Editable Parts - Select the part to be edited. Click the Add button and select a part from the model. Select Confirm.

      

    • Tool Parts - Select the the tool part. Click the Add button and select a part from the model. Preview by clicking the Apply button. Select Confirm.
14. Click OK.