Creating a Form Tool for Sheet Metal Parts

There are two different methods to create a form tool. I’ll be creating a very simple Emboss tool with an open face (which means that particular face will be removed from the sheet metal part when this form tool is applied).

Old School Method (can be used with older version also):

1. Start a new sketch on Top Plane.
2. Start a rectangle of any size.
3. Add an equal side relation between any two perpendicular sides (optional).
4. Give dimension to any of the side (optional). I have given 2 in as the linear dimension. This will fully define the sketch.
5. Now click on Extrude Boss/Base feature on the feature tool bar or Insert > Boss/Base > Extrude.
6. Extrude in any direction to any thickness. I have used .1 in as extrude thickness and click OK  to exit the command.
7. Start another sketch on the top face.
8. Draw a circle any where on the face.
9. Give a dimension as per requirement of tool size. I have used .5 in as diameter of the circle.
10. If required you can define the position of the circle to make the sketch fully defined though this is not required.

11. Extrude to the height you want for the tool using Extrude Boss/Base feature. I have extruded to .2 in height.
12. Now click on Fillet/Round feature on the feature tool bar or Insert > Features > Fillet/Round.
13. Add a fillet of .1 in on the selected edge (ref. picture).
14. Now start a new sketch or use the same sketch used for creating the rectangular base and do a cut extrude. I have used the same sketch. Sometimes it is good/easy to create a new sketch and use it.

15. Select sketch1 from the feature manger tree and click on Extrude Cut feature or Insert > Cut > Extrude.
16. Using any option i.e. Blind, Up to surface or Vertex, cut away the rectangular base.
17. The final shape will look like as shown in the picture.
18. Start a new sketch on the highlighted face (ref. picture).
19. Click on Convert Entities feature or Tools > Sketch Tools > Convert Entities.
20. A fully defined sketch will get created on the selected face.
21. Click OK to exit the sketch command. Now rename the sketch. To do this, select the Sketch in the feature manager tree and press F2 on the keyboard (shortcut for rename) or Select the sketch, pause and then again select to start the rename option.
22. Rename the sketch to Orientation sketch.
23. Now add colors to the faces to define the form tool. Right click (RMB) on the face, click on appearances and then click on Face to start the appearance mode.

24. Add color in this manner. Stopping face: Cyan color, Faces to Remove: Red Color and rest all faces Yellow color.
25. Now it is the time to save the form tool in the proper location.

26. Click on File > Save or Save as (in case you’re editing an older form tool).
27. Browse to the location where you want to save the tool (you can save either in the forming tool folder under design library or create a new folder in case you want to share the form tool over a network). Give a proper file name (I have used Dia .5 X .2) and select Form tool under File type. I have created a new folder under forming tool folder in design library with the name “My tools” to save/store the new form tools.
28. Save the file and you’re done.

New Method (Available from SW2007 onwards):

1. Repeat steps 1 -17 as discussed above. You might not require creating a base in some shapes. You need a base only if you need a fillet at the bottom.
2. After you have create the shape required, go to Insert > Sheet Metal > Forming Tool or click on Forming Tool feature on the sheet metal toolbar.
3. Select the required face as Stopping face.
4. Select the required face(s) under Faces to remove.
5. Click OK to exit the command.

6. The required colors will be added to faces as per the selection and a sketch with the name Orientation sketch will be added on the stopping face.
7. Save the files as described in steps 26- 28

We’ll see how to use the form tool, mapping the file location so that it can be shared over a network in another post.