Turning Parts into Assemblies, Assemblies into Parts (Part 1)

EmailFacebookGoogle+LinkedInTwitterShare

This next series of blogs from me will be about turning Parts into Assemblies and Assemblies into Parts in SOLIDWORKS

In this (Part 1) of the series, we will look at TURNING A PART INTO AN ASSEMBLY.

There are many reasons you might want to do this, the MAIN reason being something called the “Master Model” approach to modeling. Many consumer product designers do this. It is much easier to build a cell phone, or remote control, etc., as a PART file to get your form/fit/function looking good and THEN worry about “breaking up” the part into the necessary pieces to actually make the thing ! (i.e. top half, bottom half, battery door, buttons, display screen, etc.)
The great thing about this Master Model approach is then you have an ASSEMBLY (and all its individual parts) that live and breathe off of the original PART file you created. If you ever need to make form/fit/function changes you just edit the PART file and all the individual parts and the assembly would update too !!

Here’s how you do it: (there are other ways but this is the best)

Take your part file and create a SKETCH, a PLANE, or a SURFACE body that you want to use to SPLIT your part up. (can use multiple combinations of sketches, planes, and surfaces too)
Then use the INSERT–FEATURES–SPLIT command.
Select your Sketch/Plane/Surface as the “trimming tool” and hit CUT PART.
If you float around on the graphics screen you get to see what the result of the cut is going to do for you.
In the property manager under “Resulting Bodies” you will also see listed all the resulting solids that you will get from the split.
Now the important part…
If you JUST put a check mark in the box under the scissors icon, and hit OK on the command, you will just end up with a MULTI-BODY part.
If you DOUBLE CLICK in the “file name” box next to the check mark (for each body) and give it a name and location where you would like to SAVE, it will actually CREATE new parts on your hard drive representing the resultant solids !
A nice option down at the bottom of the property manager is to “Copy custom properties” from the master part to the individual parts (materials, vendor, etc.) if you would like.
Go ahead and hit OK on the command now…

In your MASTER file you DO now have a multi-body part.
BUT on your hard drive will be actual PART files from the SPLIT !
AND if you look in those part files there is a EXTERNAL REFERENCE (the “->” symbol) directly linking it back to your master model !
I.E. any changes in the master will update the parts…

Now, you could MANUALLY go make an ASSEMBLY from those individual parts, but who wants to do that !?
Look in the Feature Manager Tree of the master part. There is a SPLIT feature.
Right click on the SPLIT feature and choose CREATE ASSEMBLY.
It will go out and gather up ALL the parts that were created from the SPLIT feature and put them into an assembly with fixed relations so they won’t move ! Awesome !
(of course if you wanted to be able to move the parts in the assembly you can “float” a part and mate it into place the way you want it)

There you GO ! Turning a PART into an ASSEMBLY. WITH full associativity !

The OTHER great thing about the SPLIT feature showing up in the Feature Manager Tree of the master part is that any features you insert BEFORE the split WILL propagate down to the piece parts and to the assembly, and any thing you do AFTER the split feature will NOT.

This is a SUPER useful tool that A LOT of people can use even if you aren’t designing remote controls or cell phones. Let us know what YOU can think to use it for !

Stay tuned for Part 2 where we will show you how to turn an ASSEMBLY into a PART…