Pro/rNGINEER Wildfire Tips & Tutorial (Pro/E Wildfire 4.0, Wildfire 3.0, Wildfire 2.0 and 2001)

TUTORIAL: Create Form Feature using Die

TUTORIAL: Create Form Feature using Die

Version: 2001, Wildfire, Wildfire2.0, Wildfire3.0

Dies uses boundary plane and seed surface to specify the form geometry. Form feature is created when the specify form geometry interface with the Sheetmetal part. Using dies, you are able to create convex or/and concave form feature.

Pro/ENGINEER Sheetmetal die form

Below is an example of how the die form feature is created in Pro/ENGINEER.

>> Click to download the tutorial files .

1. Open the file named sm_bracket_2mm.prt

Pro/ENGINEER Sheetmetal die form

2. From the Sheetmetal toolbar, pick the Create From icon Pro/ENGINEER Sheetmetal form icon. The menu manager will now appear on the top right corner. Choose Die in the menu manager and pick Done.

Pro/ENGINEER Sheetmetal form menu manager

3. Next, choose the die that you are going to use and hit the Open button. For this case, we are selecting die_02.prt

Pro/ENGINEER Sheetmetal die open

4. A new window contains the die model and the Form Placement dialog box appear. You are now required to define the die location. You should notice that the form placement dialog box is similar to the assembly placement dialog box. So, you can use the assembly constrain (Automatic, mate, align, insert …) to define the die location.

Pro/ENGINEER Sheetmetal die

Pro/ENGINEER Sheetmetal form placement

5. For this tutorial, you can use the default location constrain default placement to place the die. Hit the preview button and you should get the preview as shown below. After that, hit the OK button to confirm the placement.

Pro/ENGINEER Sheetmetal die form

6. Die is not using the entire geometry to create the form feature. We need to define the form geometry by using the boundary plane and seed surface options. Images below indicate the selection for boundary plane and seed surface.

Bound Plane: The boundary plane is the surrounding surface to the die geometry.

Pro/ENGINEER Sheetmetal die form
Boundary Surface

Seed Surface: The seed surface can be any section of the die geometry.

Pro/ENGINEER Sheetmetal die form
Seed Surface

After the selection, hit the preview button. Your form feature is created and it should looks like this.

Pro/ENGINEER Sheetmetal die form

7. (Optional) To exclude surfaces; double click the exclude surf in the form dialog box.

Pro/ENGINEER Sheetmetal die form

Pick the surfaces which you want to exclude (press and hold ctrl to do multiple select).

Pro/ENGINEER Sheetmetal die form
Exclude Surface

The form feature after the exclude surface should looks like this.

Pro/ENGINEER Sheetmetal die form is an independent website providing tips and tutorials for Pro/ENGINEER users.
ProENGINEER version covered: ProE 2001, Wildfire, wildfire 2.0, Wildfire 3.0 and Wildfire 4.0
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