How to create a symmetric mate?

jason_29

Coming from Solidworks, it's possible to do a host of mates that references planes.  Doing so is powerful for the placement of certain parts in an assembly.  For example, Let's say I want to create a frame from three components to make an "H".  Imagine that the two vertical elements are already there.  Placing the horizontal element so that it's in the center doesn't seem to be possible without explicitly calling out the dimension for offsetting that mate.  This is undesirable, as it defeats the purpose of parametric design.  It's desirable to define a symmetric mate, this way when the dimensions of other parts change, it doesn't matter for the placement of this element.  However, I'm new, and there's a good chance I'm missing something.  Could someone offer some wisdom?

Jason

philip_thomas

@j47c - thank you for your question. This is an easy one. Insert a mate connector and select the 'between' option. This places a mate connected at the midway point between the two faces. The other question that comes up a lot when SolidWorks users try Onshape relates to layout sketches. Yes you absolutely can use layout sketches in Onshape. Create the sketch in a part studio and hang mate connectors off the critical points. Once inserted into the assembly, you simply hang the needed components off them. Here is a webinar that I did covering all of this - https://www.onshape.com/videos/twio-mate-connectors    Good luck!

traveler_hauptman

A couple quick points:

1) Onshape is very much a work in progress. I would expect symmetric mates to show up eventually. Until then you'll have to find a workaround.

2) If you are not already designing most of your parts in the same part studio, you should give it a try. Having parts of a frame correctly resize and reposition based on the layout of the parts as a whole is pretty straightforward within a part studio.

jason_29

Right.  I've picked up on that as a good technique and have gotten pretty far with it.  When I have to work with external CAD, though, this seems to break down.  Onshape, symmetric mates, please? - Jason

jakeramsley

Symmetric constraints are something that we are working on.  In the meantime, you can create mirror geometry which will essentially have the same constraint on it.  If you want a line to go across the line of symmetry, you can make a midpoint on the line and set it coincident to the mirror line.  

3dcad

@j47c Creating 'mates' by dimensioning stuff in part studio doesn't actually connect/mate part to another. If you take that part studio to assembly, you can freely move all the parts and if you wan't to keep them on place you can select all and use 'Group'.

philip_thomas

@j47c - thank you for your question. This is an easy one. Insert a mate connector and select the 'between' option. This places a mate connected at the midway point between the two faces. The other question that comes up a lot when SolidWorks users try Onshape relates to layout sketches. Yes you absolutely can use layout sketches in Onshape. Create the sketch in a part studio and hang mate connectors off the critical points. Once inserted into the assembly, you simply hang the needed components off them. Here is a webinar that I did covering all of this - https://www.onshape.com/videos/twio-mate-connectors    Good luck!

jason_29

Thanks, @Philip Thomas!  This is precisely what I was looking to accomplish.

dan_engerer

traveler_hauptman said:

A couple quick points:

1) Onshape is very much a work in progress. I would expect symmetric mates to show up eventually. Until then you'll have to find a workaround.

2) If you are not already designing most of your parts in the same part studio, you should give it a try. Having parts of a frame correctly resize and reposition based on the layout of the parts as a whole is pretty straightforward within a part studio.

Stop giving excuses for Onshape. It's supposed to be a professional program, I'm paying good money for it. It was presented as the Solidworks killer. Now it needs to act like it, not be a perpetual "work in progress"

kevin_fitzpatrick

I went crazy trying to figure out how to create a symmetric mate especially since you can't add planes to an assembly.  Then, it dawned on me that you could just create a surface and use a mate connector to "planar" mate to the surface.  Badabingbadaboom!

check it out.
https://cad.onshape.com/documents/5c47f8bc2aa1fe06e9c0409a/w/919638bbf74d167bf9fa4df8/e/dc612af0478a9c3baba157eb 

steve_cohen

Do you need the surface?  Couldn't you just create the mate connector where you want it?

TimRice

@steve_cohen
Yes you could use the plane of a mate connector.