While working on a sheet metal part, it may become necessary to flatten your part before making further changes to your geometry. Intuitively, you might want to activate the “Flatten” command in Solidworks to flatten your sheet metal onto a single sheet to make your cuts on, however you'll probably run into some issues with this. Solidworks generally considers two types of sheet metal features: Formed Features and Flattened Features. Formed Features are features that can be seen in the bent/formed state of the geometry, while Flattened Features are features that ONLY show while the flat-pattern is active. Therefore, Solidworks won’t actually propagate any edits on the flat-pattern of your part to the bent state of your sheet metal.
Let's see what happens when we make edits using the Flatten feature versus using the Fold/Unfold Feature:
Using the Flatten Feature
Here, we flattened the part and created a cut-extrude while the part is in its flattened state. When we unflatten the geometry, we get the following behavior:
The cut is suppressed along with the flat-pattern feature. This is because Solidworks is designed to differentiate between formed features and flat-pattern features by considering everything above the “Flat-Pattern” feature as a formed feature and everything below the “Flat-Pattern” feature as a flat-pattern feature.
Using the Fold/Unfold Features
Now let's try using the “Unfold” and “Fold” commands. You can find these commands on the sheet metal toolbar:
The “Flatten” command is essentially an automation of the “Unfold” and “Fold” commands, but with the “Unfold” and “Fold” commands, we can flatten the part, create features, and then fold the part back up without losing any of our edits.
To begin, we’ll unfold one of the edge flanges in our sheet metal geometry by choosing the bottom face as our fixed face and the edge flange’s bend as the bend to unfold:
After we click “ok”, we receive the following result:
We then draw our cut-extrude as shown below:
Notice how the cut-extrude is now ABOVE the “Flat-Pattern” feature in the feature tree. This means that this cut-extrude will still be shown when we refold the part back to its original configuration.
Next, we use the Fold feature, the same parameters for fixed face and bends to fold are chosen:
Here we can see that the cut-extrude was correctly propagated back to the folded state, as we originally desired. Since all formed features are preserved when entering our flat-pattern state, our cut should also appear in our flattened state:
The hole created using the Unfold/Fold features was correctly propagated to the flattened state as we expected. This is the correct workflow to use whenever you need to make edits to a flattened piece of sheet metal, but still want to see those changes in its formed state.
If you’re still having trouble propagating edits in your flattened state to your formed state, feel free to call Hawk Ridge Systems Technical Support at 877.266.4469 (US) or 866.587.6803 (Canada).