Converting your multi-body part to an assembly is a simple process, here's some tips and tricks to make sure you are successful!
In today's tech tip, we will be discussing how to convert your multibody part to an assembly. If you want a little background on multibody parts, check out our original guide here: Multibodies - Only a Stone's Throw Away
We will be discussing some more advanced techniques; such as saving the multibody part out as an assembly as well as a short discussion on external references.
First off, we have a sheet metal part. This part is made of three individual bodies, which you can see underneath the "Cut List" tab. You may notice there are two "folders" containing three bodies. In the case you have duplicate bodies created by mirrors, this can happen.
Saving Bodies as Parts
First, we will begin the Save Bodies command. You can perform this on any part, right click the "Cut List" (or "Bodies", if not Sheet Metal or a Weldment) Folder. Select Save Bodies.
Inside of the Save Bodies command, we will begin selecting and renaming our bodies. First, check on all the bodies you'd like to save. In my case, I want to save all three. By default, it will name the file as the last feature used to create it.
Let's rename those. To do this, double click on the Title of each body. This will bring up a save dialog box where you can give it a name.
Now that those are named reasonable names, I would like to direct your attention down to the "Create Assembly" box. I unchecked Consume cut bodies here. If you leave this on, your bodies will disappear from the part.
A very important note: do this when you have finalized your design.
You will be unable to edit the "SplitParts" like you would from the original multibody part (full of sheet metal bodies). It is highly recommended that the Save Bodies command is the last thing you do. They will import similarly to "dumb solids" (like a .STEP, or .X_T), meaning they have no features; just the geometry. You can still use normal commands to create new features, you will be unable to edit existing ones.
Saving Out as an Assembly
This box allows you to export the multibody part into an assembly. Be careful here. You can do this; but you are beginning to create external references. We will get into that later.
We are going to go ahead and create an assembly with this file. Press the Browse Button, and give your assembly a new name.
Hit the check mark, and everything should process. If you have a lot of bodies, this can take time. The new assembly should open by default, you may just need to tab over to it. Let's move over to the assembly. Notice how the new parts, all have external references.
Breaking External References
You can keep these intact, however, I don't recommend it for this method. Break the references by right clicking the Assembly and selecting External References.
Select Break All.
Broken references will display as ->x
Converting Back to Sheet Metal
Now that the references have been broken (if you chose to do so), you can feel free to edit these parts. You may have noticed, that these are no longer Sheet Metal parts. We can go back into each part and convert them again. You can do this right from the assembly utilizing "Edit Component".
Then convert it back. Repeat this process for the other bodies.
And just like that, you have an assembly made of sheet metal parts!
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