CAD Forum

I have a part I created that has a unique feature on it that clips in to another part. I need to use the first part as a reference for the second only for dimensions and such. I can do this by importing a part in to a part and create sketch to start building the new part while using some references from the old. The problem is I cannot suppress the old part once I get the references as it suppresses the derived part.

Maybe suppression isn't the desired thing but I can't even hide the solidbody as it hides everything that is based on it.

So what is the correct way to go about doing without having to manually "copy and paste" the dimensions to make sure everything fits/connects?

I should mention that I would also like for the base part to drive the derived part. I simply do not want the base part be part of the derived parts model(so I can print them separate).

The simple answer is you should be using assemblies instead of a multibody part. There is a method you can use with multibody parts by deleting the body you don't won't later in the history. But from the sound of things you should be using the assembly method.

I assume you are quite new to Solidworks. Judging by your question I would suggest viewing some tutorial videos on this subject (and probably Solidworks in general).

Someone may be able suggest a good place to find decent quality ones. We have Alin on the forum who often makes videos for instance.

I will second Rich's advice to do this in an assembly. Having said that, delete body might be what you are looking for.

Another option: Once the sketch is created, delete relations to the original body so that it is no longer needed.

https://help.solidworks.com/2022/englis ... e_body.htm

I'll go ahead and recommend the part insert method. There's some hassle in managing the reference file in your PDM, and maybe it depends on the PDM system you are using. We use master model technique for some parts, so we are used to it.

In our office, we strictly avoid in-context relations in assemblies. For us that is a bigger problem. So in your case, if we did want to be able to update the relations, we would use the part insert method.

Dwight

Hello, and welcome to the forum. As others mentioned, editing the Part within an Assembly might be your best option, but if you still want to insert the Part into the other Part using the Delete body for the inserted Part after you're finished referencing it will fix the problem you mentioned. Since that's a separate feature in the tree nothing above it in the tree is affected by it, so you won't lose any work done before using the Delete Body feature.

(@RichGergely mentioned this method, but I thought I'd add more detail.)

Like @Dwight I use insert body and the last step is Delete/Keep Body...

My most likely use case is creating a lid for a housing. Other then thickness and hole/thread sizes everything else is referenced geometry.