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Don't Get Shortsheeted - Multibody Sheet Metal Parts

Vince Farrell

By Vince Farrell

When I mention the word “multibody”, I hope it doesn’t bring up the bowling dream sequence in The Big Lebowski because that’s an out-of-body experience. A multibody part is a part in SOLIDWORKS that is made up of multiple solids and/or surfaces within the same part file. These bodies can be touching or not touching, but if they aren’t touching, then they are separate bodies by default. You can make multibody parts using various modules within SOLIDWORKS, but this article will focus on creating multibody sheet metal parts within the sheet metal module.

Making a multibody sheet metal part is easy and useful. Some reasons you would make this type of part is if you are working with different gauges and different materials of sheet metal within the same part. Also, if the bodies are within the same part, if you change a dimension or relation of one part, everything will change accordingly. This insures that your parts fit together when you are done with your design.

Here’s an example of what a multibody sheet metal part looks like. This is a router table with a top and 4 legs:

Sheet Metal Part

In this example, the router table is AISI 304 material while the legs are AISI 306. Also, the legs and the table top are different gauges. Let’s step through how you would create a part like this.

I’m going to start at the step where the table top was created as a single body. To summarize, this was created as a profile sketch, extruded as a Base Flange/Tab, and then Edge Flanges were added to the sides. There’s also some holes added to the part:

 

Sheet metal

From the feature manager tree, we can see that there is one body in the Cut list, and one sheet-metal feature, as expected since this is a single body part. I’m going to start a sketch on one of the inside faces that will be the profile of one of the legs:

Designing

Note that the view has been sectioned so that we can make dimensions and relations to the profile of the table. Now I will revolve the profile about the long side 90 degrees:

 

Sheet Metal

By default, SOLIDWORKS will want to merge this new feature with the table top since they are touching (remember the first paragraph of this article?) I don’t want it to do this since I want a separate body, so make sure that the Merge result box is unchecked. Now if we look at the Cut list folder, there are 2 bodies. I can also isolate the body I want to work on by right clicking the name in the Cut list folder and clicking Isolate:

SOLDIWORKS Design

The icons are different since the first body is a sheet metal body and the second body is a solid body. Next, we convert the solid leg to sheet metal by clicking the Convert to Sheet Metal button:

At this point, we can choose to use the same gauge as the table or change it:

Solidworks Design

After the conversion and exiting the Isolate, we now have two separate pieces:

Sheet Metal

We can add different materials to each (right click on the body in the Cut list, and if you look down at the bottom of the Feature Manager tree, you can see we have two separate flat patterns:

Sheet metal

If you hit the Flatten button in the Command Manager, it will only flatten the first body, so you will need to actually unsuppress the flat pattern feature for the other body, or right click on the body and select Flatten. Now with a couple of Mirror operations, we can use that first leg to create 3 more legs. SOLIDWORKS might add these bodies to a new Cut list, so just select them and left click and drag them into the Cut list you want them to be in.

Sheet Metal

That’s it! If you would like to see a video on this, please click on this link. Good luck on your sheet metal designs and thanks for reading!

For further assistance, please contact our HawkSupport team at 877-266-4469(US) or 866-587-6803(Canada) and support@hawkridgesys.com.

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