SOLIDWORKS: Flatten Complex Bent Square Tubes Part II

Flatten Complex
Posted in: Mechanical Design
August 11, 2017

This is Part 2 of a two-part series on flattening bent square tubes to obtain unbent length and locations of features. Before we begin, please review Part 1 by clicking here, where the tube is prepared by removing excess curved faces with Delete Face, suppressing or deleting cuts on the ends of the tube, and using Convert Entities to capture hole locations and sizes. This article will deal with the more complex case of bends in multiple planes. This requires a modified workflow, as the Sheet Metal commands create bends that are normal to the thickness of the sheet. In this case, some of the bends in the tube would represent bending the “sheet metal” along the edge of the sheet (the bent face would be on the thin face or “edge” of the sheet). In order to control this, we will split the tube into multiple sections with each section having bends in only one plane. In the case of the tube above, it will be split into three sections using a simple Cut-Extrude.

Having already prepared the model as shown in Part 1, the next step is to cut the tube into sections. An open-contour cut is used to split the part by sketching a line across both short sections and selecting Through All-Both in the Cut-Extrude PropertyManager. It is important to leave a gap between the newly split parts, so the Thin Feature option was selected with an arbitrary value. Note: do not make the Thin Feature dimension so large that it intersects with any bends.

Now, in the same manner as in Part 1 of the series, use the Insert Bends command to convert each section into a Sheet Metal part, allowing SOLIDWORKS to process the bends. In our example, with three sections, Insert Bends was used three times.

To merge these sections together we will use a standard Boss-Extrude to bridge each of the gaps between sections.

This extrusion does not have to be cylindrical or centered as shown. However, be sure not to merge the faces of the tube sections (possible if using a rectangular extrusion) as this can cause the Flat Pattern to break.

The result is a single Flat Pattern that takes into account all bends in the model.

The final step is to make the bridge section unnoticeable. To do this, reduce the Thin Feature dimension to a small value such as 0.0001”.

Now you may add back any features that were removed at the beginning such as holes or end cuts.

And as shown in Part 1, you may also want to use a Cut-Extrude to regain the appearance of the original square tubing.

You now have an unbent tube that is ready to be detailed out in a drawing. You still have the ability to add new features along the tube as well as edit dimensions of the original bent shape. Note: if you require adding new sections to the tube that would involve new out-of-plane bends then this process should be repeated for those new sections. For more information, check out our YouTube channel, get a SOLIDWORKS 3D CAD quote or contact us at Hawk Ridge Systems today. Thanks for reading!

August 11, 2017
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