SOLIDWORKS Sheet Metal – Another way to Create Flat Patterns

Article by Mike Walloch updated April 18, 2023

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For SOLIDWORKS parts to meet the requirements to use Sheet Metal features they must follow three rules. Actually being made of metal isn’t one of them. They must be thin-walled parts with a uniform thickness, have bends at the corners, and be capable of being flattened.

Dropping an anvil on the part doesn’t count for that last point. It must be able to be folded and unfolded, bend by bend. So, in the example shown below the folded metal part and the cardboard box are candidates for SOLIDWORKS Sheet Metal features, but the stamped copper part is not.

If you need to calculate the flat pattern in SOLIDWORKS Sheet Metal for a part that does not have quality for normal Sheet Metal features, SOLIDWORKS Premium has a tool, Surface Flatten, which can help. But you have to know how to use it in this situation to get useful results. Our workflow will involve Surface Modeling tools.

First, we’ll use Offset Surface to create a surface body we can flatten. Then we’ll make our flat pattern by using Surface Flatten on that body, and then Thicken on the flattened surface body to make it a proper 3D representation of our flat stock.

For this example, we’ll use the stamped 1/8” thick copper part shown above. Normally a SOLIDWORKS Sheet Metal part would calculate the appropriate inside surface and k-Factor for each individual bend. But in this case, we’re creating a surface body representing a theoretical ‘neutral plane’ somewhere inside the stock, where stretching and compression of the material during the stamping process is balanced. Assuming we’re using the right k-Factor, this should give us a flat pattern that’s close enough to the real-world part to be within our desired tolerance range.

The first thing we need to do is use Offset Surface to create a surface body at 45% of the material thickness measured from the ‘inside’ of the part, which in this case is .05625”.

Now we can hide the solid body to make the new surface body easier to work with.

We can use Surface Flatten to create another surface body. The tool meshes the selected faces to be flattened with triangles, similar to using shell elements in an FEA simulation. To get the most accurate results we want small triangles in the mesh, so turn the ‘Accuracy’ slider all the way up to High. This will take longer to process, but unless the part is extremely complex it still won’t take long. (I’ve turned off the mesh preview in the image below to make it clearer.)

Now we can hide the previous surface body and look at the new surface body created by the Surface-Flatten feature. Assuming we used the right k-Factor to find the average neutral plane for this part, we now have an accurate representation of our flat stock, except for the lack of thickness.

Now we can use Thicken to turn the flat surface body into a 1/8” thick solid body, a 3D representation of our flat stock.

Toggling Between Formed & Flattened

In a SOLIDWORKS Sheet Metal part, we can easily toggle between the formed and flattened versions of the part. Using the alternative method described above we can’t do that in the same way. However, we can do it using either Configurations or Display States.

With the Configurations option you can create a derived configuration of the part with the Surface-Offset, Surface-Flatten, and Thicken features unsuppressed. Suppress them in the parent configuration. The downside to this option is configurations add considerably to the file size, and switching between them requires a rebuild of the model.

Using Display States instead will add very little to the file size. Since Display States deal only with graphics, switching between them does not require a rebuild. Just have one Display State where only the original solid body is shown, and another where only the flattened solid body is shown. Not only does this method provide a performance boost over a new configuration, it’s also a little easier to set up.

Conclusion

SOLIDWORKS provides us with a massive toolset which can meet almost any modeling need, including creating a flat pattern in SOLIDWORKS Sheet Metal. Individual tools do have their limitations, of course. When you run into those limitations, an alternate modeling technique will often fit the bill.