Forming Tool Tips

In my previous blog, Forming Tools, we examined how pre-SOLIDWORKS 2006 sheet metal forming tools differ from those which can be created today. We examined how to save forming tools as Form Tool part files and what the advantages were of doing so.

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 1. 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 will not work.

Be careful with inside radius issues

Figure 1: 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 2 shows the knockout forming tool’s ConfigurationManager with 4 new configurations. These configurations will appear when the forming tool is used. Figure 2 (inset) shows the drop down list which would appear when using this forming tool.


Using configurations with a forming tool

Figure 2: 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 3).


Creating a sketch that describes the area to be removed

Figure 3: 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 4, 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.


Using the Split Line command

Figure 4: 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, and is shown in Figure 5.

The face created with the Split Line command

Figure 5: The face created with the Split Line command.


Those three tips should help in the process of creating some very useful custom forming tools. The final image (Figure 6) shows the knockout forming tool in action, having been used on a sheet metal part file. Using the custom knockout forming tool

Figure 6: Using the custom knockout forming tool.


Thanks for reading and Happy Modeling!

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