This article discusses how to use SOLIDWORKS Forming Tools and some tips on how to create your own.
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 provides some forming tools to get you started. Modify existing forming tools to meet your needs, or create entirely new forming tools from scratch.
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The forming tools included with the software use an “old school” creation technique which is, to put it bluntly, outdated.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 may be 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).
The Forming Tools Folder setting is only required if using older versions of SOLIDWORKS that still used standard part files (.SLDPRT) for forming tools, as opposed to Form Tool part files (.SLDFTP), which were included with SOLIDWORKS 2020 and later.
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.
Figure 3: The Form Tool Feature PropertyManager.
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. Adding points is done after clicking the Position tab in the Form Tool Feature PropertyManager. Dimension the location of these points, or use relations to establish the desired position.
Figure 4: Adding a point adds another instance. Dimension as needed.
Obsolete Forming Tool Creation
Even though the process of creating a forming tool was updated in SOLIDWORKS 2006, the forming tools included with SOLIDWORKS still employ the pre-2006 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. If a read-only warning is shown, click the "Open Read-Only" button.
Figure 5: Examining the old process used to create forming tools.
Understanding how these old forming tools were created will help if one of the canned forming tools needs to be modified. Therefore, let’s look at a short summary of how they were modeled using Figure 5 as a reference.
- A base feature is created, typically a small plate. This is used as temporary geometry on which to place the forming tool.
- The forming tool geometry is created. A variety of features can be used to accomplish this task.
- The original base feature is removed using a cut feature.
- 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, which aids in positioning.
- If there are any faces that should be removed when the forming tool is employed, those faces must be assigned the color red with the precise RGB value of 255, 0, 0. It would have been necessary to do this with the Appearances command.
Prior to 2019, forming tools were saved as standard part files. The advent of Form Tool part files (.sldftp) was a "silent enhancement" not listed in the What's New guides.
Forming Tool Creation
Fortunately for us, creating forming tools is easier than it was. Let’s stick with the same counter sink emboss forming tool and examine the process. The first 2 steps are the same, because we still need to create the appropriate geometry and something on which to place it. Let's pick up after step 2, where the process becomes much more streamlined.
1. Click the Forming Tool command (see Figure 6) on the Sheet Metal tab of your Command Manager, or access the Forming Tool command from the Insert > Sheet Metal menu.
Figure 6: The Forming Tool command.
2. In the Form Tool PropertyManager (see Figure 7), 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.
4. Click the Insertion Point tab (also shown in Figure 7). 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.
Figure 7: Form Tool PropertyManager.
5. 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 were all standard part files at one time. 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 this article, it was 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. This is because prior to 2020, the forming tools included with SOLIDWORKS were standard part files. Sometime after, those same files included with every installation of SOLIDWORKS were Form Tool part files.
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. They are already understood by SOLIDWORKS to be forming tools due to their unique file extension. Form Tool files can be dragged and dropped from any folder location, even if they do not reside in the Design Library.
Converting Part Files to Form Tool Files
How do you save a forming tool as a Form Tool part file? Use the File > Save As command, and pick Form Tool as the file type you’re saving as.
Any part can be saved as a Form Tool part, even if it does not contain a forming tool feature. There is no warning, so be careful! A forming tool feature must be present, or an error will occur when trying to utilize the Form Tool part file.
Figure 8: Form Tool error.
Updating Old Forming Tools
If you find some of the old 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 9). 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.
Figure 9: Modernizing old forming tools.
Forming Tool Creation Tips
When creating custom forming tools, be careful not to create any curved faces (typically fillets) with an inside radius smaller than the maximum thickness material you may be applying the forming tool to. Examine the knockout in Figure 10. The large radius fillet will shrink to .036” if this forming tool is used on a part with a thickness of .050”. Using this tool on a part with a thickness of .086” (or greater) will force the radius to become zero (or even a negative value) and the forming tool may not work.
Figure 10: Be careful with inside radius values.
Take Advantage of Configurations
If your forming tool comes in different sizes, take advantage of configurations. The example in Figure 10 shows the knockout forming tool’s ConfigurationManager with 4 new configurations. These configurations will appear when the forming tool is used. Figure 11 (inset) shows the drop down list which would appear when using this forming tool.
Figure 11: Using configurations with a forming tool.
Using Split Lines for Face Removal
Are you familiar with the Split Line command? It is a great command, and very useful in a number of interesting situations. Technically, what the Split Line command does is to split a face into multiple areas. This can be extremely useful in the creation of forming tools.
For our example, let’s imagine we wanted an opening in the knockout where a screwdriver could be inserted to more easily twist out and remove the knockout. First we will create a sketch that describes the area where the opening should be (see Figure 12).
Figure 12: Creating a sketch that describes the area to be removed.
Next, access the Split Line command found in the Insert > Curve menu. In the Split Line PropertyManager, shown in Figure 13, select the face to be split. The type of split should be Projection. Check the Single Direction option if you like, but it isn’t mandatory in this case. Click OK to complete the command.
Figure 13: Using the Split Line command.
The end result is a separate face that can be selected as a Face To Remove when defining the Form Tool feature. The completed Form Tool feature is shown in Figure 14. It is worth noting there are now a total of 4 faces that will be removed when the forming tool feature is used.
Figure 14: The face created with the Split Line command.
The final image (Figure 15) shows the knockout forming tool in action, having been used on a sheet metal part. Different configurations were used. It is not apparent in the image, but there are actually small gaps between the disks of the knockouts and the rest of the sheet metal part.
Figure 15: Using the custom knockout forming tool.