SOLIDWORKS Sheet Metal vs Body Convert Part Creation Method

Article by James Swackhammer updated May 9, 2019


In this article I am going to make a very basic sheet metal box with two different creation techniques to determine which is more efficient, delivers more accurate results, and looks better. Before you jump to conclusions thinking which method is better, you might be surprised by the outcome. Stay tuned for the results.

The two different creation methods are:

  1. Making the box using the body (boss extrude) with various support features, then using convert to sheet metal.
  2. Fully modelling the part using sheet metal tools.

Method 1: Convert to Sheet Metal

Start off by making a sketch 12″ x 12″ (start plane doesn’t matter here) and extrude mid-plane 12″ to get a cube. Next we need to make a 0.25″ fillet on the bottom 4 edges. A shell feature is needed after the filler and keep the wall thickness to 0.125″. This is starting to look like a sheet metal box, right?

Box model shelled

Box model shelled

We need one last feature and that is Convert to Sheet Metal command located in the sheet metal tab. In here we want the thickness to be (again) 0.125″ the bend radius to be 0.125″ and use the Collect All Bends button. This button will grab all the sides and produce any rip edges that are needed. Here’s the interesting part, before you hit the check on this command, scroll down to look at the other options. There are corner types to consider. For this demo I selected Corner Butt and took the smallest I could get without errors for Default Gap at 0.010″ and Overlap at 0.50. One last item is choose a material, I took Plain Carbon Steel. This part is complete, save and put aside so we can compare with the next one.

Measuring the gap

Measuring the gap

NOTE: Without the radius the convert to sheet doesn’t work. Also something to note: the radius must be bigger than the metal thickness to work as well.

Method 2: Creating Sheet Metal

Start off by making a sketch on the top plane (most sheet metal parts should be drawing on top plane) and draw the same 12″ x 12″ square. Instead of extruding, use the Base Flange/Tab and make the thickness 0.125″.

The next and final command we need to use is the Edge Flange. Select the 4 edges you filleted in the last part. The selection doesn’t matter if it is the top or bottom edge, what does matter is the direction and height. I chose 12″ blind up (Y direction).

Sheet Metal Part

Sheet Metal Part

My flange position is material inside to maintain the 12″ outside dimension. I made my best radius the same 0.125″ and the gap distance 0.0001″. Please note that this isn’t the smallest, but is the smallest that would be practical for most sheet metal parts. The last thing is to change to the same material type (Plain Carbon Steel).

Gap measurement

Gap measurement

Part Comparison

Now we have two parts that are “exactly” the same, right? Let’s dive into this further:

Mass Properties

Doing Mass Properties on both parts will tell a different story. The sheet metal part I created is 24.593 lbs and the converted part is 24.564 lbs. The difference is so small, which means we can call it equal. Let’s give a point to each.

  • Method 1 Score = 1
  • Method 2 Score = 1


Taking a look at the work flow to complete each part, it seems there is an easy winner. The sheet metal part uses less features, takes a shorter amount of time and requires little effort to create the part. The bodies part needs more design intent to create. Knowing that, the future bend radius and material thickness dictates how the part is made otherwise you will end up with errors or warnings.

  • Method 1 Score = 1
  • Method 2 Score = 2

Physical appearance

The last test is the physical appearance. Just a quick scan and rotating the parts, everything seems fine, but zoom in closer on the corners. On the converted part you get a weird twisted edge. This occurs in any type of relief you do and yes, a corner relief or treatment can be placed in, but that is yet another step and another feature.

Corner for converted part

Corner for converted part

The sheet metal corner has a better and more organic look to it. The last physical check is the flat pattern look. Analyzing both flats and the corners are again, the most noticeable item here with the same outcome as before.


Sheet Metal Part Corner

Sheet Metal Part Corner

  • Method 1 Score = 1
  • Method 2 Score = 3

Our conclusion: creating a Sheet Metal Part is the winner

Making a sheet metal part rather than converting a part to sheet metal works out better in the long run. This works for most cases and this isn’t saying ‘don’t design a part using the bodies method and converting’, but you’ll typically get a better looking and easier to make product using the sheet metal commands.

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James Swackhammer

James is a SOLIDWORKS Technical Support Application Expert based in the Javelin Oakville head office