Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.
First time visiting? Here are some places to start:- Looking for a certain topic? Check out the categories filter or use Search (upper right).
- Need support? Ask a question to our Community Support category.
- Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
- Be respectful, on topic and if you see a problem, Flag it.
If you would like to contact our Community Manager personally, feel free to send a private message or an email.
Composite Parts - how to use them?
I'm experimenting with using a composite part to represent a molded part with insert molded threaded inserts. We started with an assembly, but because no one in the supply chain ever orders the plastic part without the inserts, it started to seem like it would make sense to use a composite part.
A few things are a bit strange:
A few things are a bit strange:
- I added two (of the same) inserts using the Point Derive FS. At first they didn't have their material set, so I set one to brass, and the second insert didn't pick up the material setting. I went to the part studio where the insert was created, and set the material, and then both inserts picked up the correct material. Is there a better way to manage this?
- With an open composite, the mass properties work in the part studio, but in the next level assembly, the BOM reports "no value" for the mass. I tried a closed composite, but that made things worse. Then there was no material defined in the part studio (and I assumed it would treat the composite as a single material, if I assigned it)
0
Comments
As for how materials are handled for derived parts, what you describe is the behavior I'd expect. I'd plan on setting materials at the original part studio level. In this case, the studio with the insert.
At least now you can set an assembly to hide it's sub-parts so it's less of a tradeoff to create this as an assembly for something like this (other than needing two tabs).
Yes. It's a bit odd. It seems more like what was happening in Solidworks land. "Let's add some kinda useful functionality, but don't think it all the way through."
Unless we're just working on science fiction, all of our parts have mass. In my case, one of our product's key metrics is overall weight, so it's nice to track the mass of everything. I'm sure we're not unique.
Your reminder of the subassembly options really seals this in for me for now. Until the BOM "no value" mass oversight (bug) gets fixed, we'll stick with assemblies, but our BOM and naming will treat it more like a part.
My understanding of the closed composite behavior is that it's more useful for things where you have a ton of parts (e.g. a PCBA import) and want to simplify the load on Onshape by creating one dumb part. I'm sure there are other interesting uses, but that's the one place I've found it helpful.
If you think of a closed composite is basically as an alternate to a boolean union (for when an boolean union wouldn't work because of disjointed bodies and non-solid entities). Then it sort of makes sense that the mass would be set for the whole thing uniformly.
The open composite is a bit of a weird one actually but it's the equivalent to a multi-body part in other CAD systems. What can be a bit confusing is that when you go to use it you have to be careful to not insert just a sub-part.
It's almost like we would need a 3rd option that hides all the parts but retains the mass/appearances. However at this point it's basically an assembly (but without creating a new tab)...
A good example of a dilemma is for models of sealing washer that we use on some our assemblies: a piece of SS steel with a rubber gasket bonded to it: it's nice to have a configured model so you can swap size easily, and also nice to be able to show them in their "raw" (exploded views for example) and "squished" (to see where the bolt actually ends up after assembly) configurations.
Right now if I want the correct mass I need to keep the composite "open" but then you might grab the wrong thing when inserting them. If it's closed, then it's easy but you have to manually set the mass for each configuration.
If it's an assembly then you have to know to look for an assembly when inserting so it's not ideal either...
Having to know what to look for when inserting into an assembly is a bit awkward for composites as well. I kinda feel like the insert dialog should default to all parts/composite parts/sketches/assemblies and allow you to uncheck things to filter. I found myself momentarily confused why my composite part wasn't showing up in the insert part dialog at first.
You already have parts, composite parts, sketches, surfaces, flat patterns, why not have just one more of assemblies rather than have them in a different "header". Good question about the default but it should probably include parts, composites and assemblies and then you could turn them off as needed to refine.
Actually I just notice if you deselect all filters (i.e. deselect the part filter that is checked by default from the part studio header) it shows everything (I've always "added" the things I was looking for by clicking on them)!
I would prefer "all filters off" to be the default but I also understand why it would be nice for "beginners" to only see parts when they go to insert something in an assembly so I'm not sure...
The bizarre thing is that in the part studio, the mass property tool works just fine on a composite part, but somehow it goes missing in the assembly BOM. It shouldn't require any custom features, just a fix from Onshape.