SOLIDWORKS, 3D CAD, Tech Tips

Design Sheet Metal Fast with the Convert to Sheet Metal Feature

By Justin Lingerfelt on July 15, 2016

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Want to get that sheet metal design going more quickly? Utilizing "Convert to Sheet Metal" can help.

Are you more of a visual learner? Scroll to the bottom for a step-by-step video of this tutorial.

Click the images to enlarge. 

Simple Shape

Step 1: Start with a simple shape. This shape can either represent the overall size of your part or the internal volume. In this example, a block with an extrude is created to represent the overall size of the part.

 

 

Step 2: Click the "Convert to Sheet Metal" icon located on the Sheet Metal tab of the Command Manager.

Convert To Sheet Metal

 

 Gauge Table

Step 3: The first option in the PropertyManager is a check box to use a gauge table. You can use a gauge table or manually enter a thickness in the next section. In this example, the box is checked to use a gauge table and the drop down menu is used to select the table.

 

 

Step_4.pngStep 4: Under "Sheet Metal Parameters" choose a face to fix (pictured in Step 3). SOLIDWORKS will bend all flanges from this face. Choosing a face parallel to either the front or top plane that represents either the front or bottom of the part will affect the flat pattern.

Next, choose your gauge using the drop down menu or enter a thickness manually. The "Reverse Thickness" check box controls whether the sheet metal will be inside or outside the geometry. You want the thickness on the outside if your geometry represents the internal volume.

In this example, it is cleared. The "Keep Body" option will keep the geometry after the Sheet Metal part is created. This is useful if you want a way to measure the internal volume of the part.

"Override Thickness" allows you to manually set the thickness if you chose to use a gauge table. "Override Radius" controls the bend radius. 

 

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Step 5: Select the edges that will be bends. The order in which this is done is very important. Always start from the "Fixed Face" first. In this example, all four edges for the fixed face are selected.

 

 

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Now, select the secondary bends. There are two in this example. The bends will be highlighted in pink by default and the gaps in purple. SOLIDWORKS automatically fills out the "Rip Edges" box. That is why order of selection is important.

 

 

 

 

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Continue selecting edges in the order in which they are bent in relation to the fixed face. In this example, there are two more tertiary bends and one fourth bend. You can double click on the callouts to override the gaps and bend radius of each flange. If you don't see the callouts, make sure to check the box "Show Callouts" -- one check box for each section (Bend Edges, Rip Edges and Rip Sketches).

 

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Step 6: At the bottom of the "Convert to Metal" PropertyManager is where you can control the Corner Defaults, Bend Allowance and Corner Reliefs.

 

 

 

 

 

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Final Step: Click the check mark at the top of the "Convert to Sheet Metal" Property Manager. You will notice you now have a Cut List folder, Sheet Metal folder, and Convert Solid feature.

Right clicking on the "Sheet Metal" folder allows you to change the gauge, default bend radius, Bend Allowance and Corner Reliefs.

Right clicking on the "Convert Solid" feature allows you to add or remove bends and rips plus change the fixed face.

This tutorial was also created in video format!

 

Learn more about sheet metal with our On-Demand Webinar: Sheet Metal Tips and Tricks!

Sheet Metal Tips & Tricks