An opinion on Onshapes mating system

Paul_J_Premakumar

Hi Vishwarath,

 We have some tutorials : https://www.onshape.com/videos/using-mate-connectors  and https://www.onshape.com/videos/assembly-mates . If there is anything in particular you'd like to see covered, feel free to leave a comment. 

koen_van_niekerk599

How come I can use almost every Onshape modeling tool at first try (coming from a SolidWorks background), But after WEEKS I still do not understand the assembly / mate -creation paradigm. It is just really, really unintuitive. 

I always take care setting up my parts with nice symmetric construction planes. I want to be able to mate to these planes these in an assembly and to Axis.

The reason? It allows me to quickly build and assess a fully functioning assembly / mechanism without having to create all the geometry (like hinges) that are required for your "real-world" mates. If I want a hinging constructoin, I should not need to model the whole hinge first... 

bryan_lagrange

@koen_van_niekerk599 go through a tutorial on creating and using mate connectors. Makes assembling so much easier.

https://learn.onshape.com/courses/all-the-ways-to-use-mate-connectors

https://learn.onshape.com/courses/all-the-ways-you-can-use-mate-connectors-in-onshape

S1mon

Mates in Onshape were definitely one of the harder things to wrap my head around coming from Creo and Solidworks. That said, I mostly prefer Onshape’s mates now because there are so many fewer clicks.

If you’re building a lot of parts in a part studio where there’s no functional geometry yet, you might find Multi Mate Connector useful. 

https://cad.onshape.com/documents/5d8da63844bedebe5cff72b1/v/cfcff754d7bed39f9aca3ea6/e/11dcab8f665add80b9aced0a

You can easily add mate connectors to a bunch of parts in one step and then use those for whatever mates you want in your assembly.

The other thing that takes some getting used to is the lack of planes in the assembly. You can either fix a single key component when you insert it at its default location or you can mate that key component to the origin, or what I often like to do - create an assembly mate connector at the origin and mate parts to that. If you don’t do that, your assemblies can float around in space.

In any case keep in mind that fix only really has meaning at that assembly level, group mates will continue to do their thing when you have a subassembly in another assembly, but fix is only relevant at that assembly level. All assemblies are always “flexible” in Onshape - to use the Solidworks terminology. Group mates can be a little tricky because higher level assemblies’ group mates will override lower level assemblies’ group mates. In the higher assemblies, if you are grouping things from lower assemblies, just pick one key component out of a group.

eric_pesty

@koen_van_niekerk599
I agree with others that the mate system takes time to get used to because it's more "different" from SW than other parts...

That said, it's definitely worth persevering as I suspect you will end up liking it better. In your example of having a hinge mate without the actual hinge, it's actually much better in Onshape. The easiest way is to create explicit mate connectors in your parts, and with a bit of planning ahead it become really simple and you will start adding an extra feature in a sketch specifically for that but there are a couple other options as well. 

Depending on what you are designing, designing several parts in the same part studio also streamlines everything quite a bit as you can just insert and group things that don't move relative to each other or easily add reference mate connectors exactly where you need them. The multi mate connector mentioned by @S1mon is definitely super useful for that.

One thing to keep in mind is that you can insert sketches or construction surfaces in assemblies and mate them so if you have a layout sketch that shows your hinge axis you can dump that in your assembly and use it directly. You can also use reference sketches for parts you don't have modeled yet so it's very flexible

You can also apply offsets to mates in the assembly as well as edit each implicit mate connector that forms the mate (although unfortunately you have to create the mate first so it takes a bit of back forth and I wish they added an option to do it from the mate dialogue but I digress), which provides a lot of flexibility.

One area that I find is not very well explained is "offsets" in mates. The key thing to know when you are adding an offset to a mate is that the selection order matters: the offset is applied in the direction of your first pick (the offsets are going to be in the x,y,z of your first selected mate connector), and also gets applied to the first selected. What it means is that if you are mating a "floating" part to an already constrained one, pick a mate connector on the floating one first and things will behave in a more intuitive way.

The lack of planes in assemblies is a bit disconcerting at first but whenever I go back to SW now I am amazed at how much time I spend expanding and collapsing parts looking for the right planes and scrolling past all the part features etc... The cleaner assembly tree is actually really nice!

Another huge benefit to the Onshape system is that it is so much easier to troubleshoot broken mates because you have less than 1/2 as many and don't end up with the typical conflicts between a planar and axis being in "opposite alignments", not to mention that things don't randomly flip around like they do in SW.