If you take advantage of SOLIDWORKS sheet metal functions, forming tools can be very useful. Forming tools represent features created with stamping or punching operations, and are part of your Design Library (see figure 1). SOLIDWORKS gives you some forming tools to get you started, but you can create your own or modify existing tools to meet your needs.
Figure 1: Accessing Forming Tools in the Design Library.
The forming tools included with the software use an “old school” creation technique which is, to put it bluntly, outdated. We will look at how to update these tools in a moment. If you wish to use forming tools as is, it is necessary to make SOLIDWORKS aware which folders in the Design Library contain forming tools. To do this, right click the Forming Tools folder in your Design Library and make sure the Forming Tools Folder selection in the menu is checked (see Figure 2). It should be checked by default, but it’s always best to make certain.
Figure 2: Setting the Forming Tools Folder option.
To use forming tools, use the same drag and drop technique you would use to insert anything from the Design Library. Drop the forming tool onto a planar face, then use the Form Tool Feature PropertyManager to adjust parameters, such as rotation angle and which side of the part the tool punches into. We won’t go into detail regarding these parameters, as they should be fairly straightforward.
Locating the forming tool is very similar to locating holes using the Hole Wizard. Like the Hole Wizard, points can be placed wherever additional copies of the forming tool should go. Dimension the location of these points, or use relations to establish the desired position. Locating or adding additional points is done by clicking the Position tab (not pictured), found at the top of the Form Tool Feature PropertyManager.
Obsolete Forming Tool Creation
For this article, we will focus on updating forming tools, as well as creating your own. Earlier, I mentioned that the forming tools provided by SOLIDWORKS were created using an “old school” technique. To show what is meant by this, let’s open the counter sink emboss forming tool, found in the forming tools\embosses folder. (This can be done by right clicking the forming tool in the Design Library and selecting Open.)
Figure 3: Examining the old process used to create forming tools.
It’s not in our best interest to completely understand exactly how these old forming tools were created, but it helps to have a general understanding. Therefore, let’s look at a short summary of how it was done. Refer to Figure 3 when reading the summary.
1. A base feature is created, typically a small plate. This is used as a place to put the forming tool on.
2. The forming tool geometry is created. A variety of features can be used to accomplish this task.
3. The original base feature is removed using a cut feature.
4. A sketch is created on the bottom of the final geometry and Convert Entities is used to create what is referred to as a “locating sketch” (not shown). This is the sketch that appears when dropping the forming tool onto a part so it can be located.
5. If there are any faces that will get removed when the forming tool is employed, those faces must be assigned the color red with the precise RGB value of 255, 0, 0.
Fortunately for us, the process of creating a forming tool is much easier now, and has been since SOLIDWORKS 2006. Let’s stick with the same counter sink emboss forming tool and examine what the process is like now. The first 2 steps are the same, because we still need to create the appropriate geometry, but after step 2, the process becomes much more streamlined and user-friendly. Check out this Tech Tip from Mark for a quick video of these steps.
Figure 4: The Forming Tool command.
1. Click the Forming Tool command (see Figure 4) on the Sheet Metal tab of your Command Manager.
2. In the Form Tool PropertyManager (see Figure 5), select the stopping face. This is the face that will butt up against your sheet metal part.
3. Optionally, select any faces that will get removed when using this forming tool.
Figure 5: Form Tool PropertyManager.
4. Click the Insertion Point tab (also shown in Figure 5). A point will be present on the stopping face of the forming tool geometry. Think of this as the “handle” the forming tool will be held by as it is dropped onto a part. It is also the point you will dimension in order to position the forming tool. Use standard dimensions or relations to locate the point where you want. Click OK when finished.
Your forming tool is now complete; however there is still one more task to accomplish if you wish to have the greatest amount of flexibility when using forming tools.
Forming Tool Files
The forming tools included with SOLIDWORKS are all standard part files. Did you know there is a special file type just for forming tools? They are known as Form Tool part files and have a file extension of .SLDFTP. These files have a special ability.
Earlier in the blog, I mentioned it is necessary to set the Forming Tools Folder option in the Design Library (refer back to Figure 2). If this is not done, SOLIDWORKS is not aware the folder contains forming tools, and the forming tools will not work. When using Form Tool part files, it is not necessary to keep them in a special folder designated as a Forming Tools Folder. In fact, Form Tool part files can be stored anywhere. Since they are already understood by SOLIDWORKS to be forming tools, due to their unique file extension, they can be dragged and dropped from any folder location.
How do you save a forming tool as a Form Tool part? Use the File > Save As command, and pick Form Tool as the file type you’re saving as.
Updating Those Old Forming Tools
If you find some of the canned forming tools useful, but would like to update them, the process is quite simple. Once you’ve opened the forming tool, delete the orientation sketch and the final cut-extrude that removes the original base feature (see Figure 5). Once that’s done, use the Form Tool feature command to create the forming tool, and save the results as a Form Tool part file. That’s it!
Happy Modeling!