Mating Fins to a Rocket Fuselage.

tom_hannon

My are designing and building rockets using OnShape.  They have designed the cylindrical fuselage and the fins that attach to it.  The three fins need to be mated to the fuselage in an assembly much like the fletchings would be attached to shaft of an arrow.  We are not having any luck finding a good, efficient way to mate the fins to the fuselage, evenly spaced at 120 degrees apart.  Does anybody have a suggestion?

wayne_sauder

@tom_hannon
Mate 1 fin using a mate created in the parts studio, if using multipart part studio then use the circular pattern.

wayne_sauder

@tom_hannon
Or just insert and group then use the circular pattern.
https://cad.onshape.com/documents/24b325853be5547a6434fc24/w/a368e19f79a45faff9698216/e/c29c936e9cc7b6e9ac6db780

dave_franchino

I'm struggling with Onshape mates as well - particularly the inability (I think) to access part features in assembly mode and therefore the lack of access to planes and axis which in Solidworks were useful tools.  Pragmatically this has meant I need to have a geometry feature on the part to mate to - whereas there seem to be plenty of situations where I'd like to mate to a construction element as opposed to a geometric feature. I can find ways around this but they all seem like really bad cobbles. Am I missing something here?

pmd

@dave_franchino - you can also insert sketches from a Part Studio into an assembly. This is frequently used to bring in a simple vertical line (e.g.) for the centre of a circular pattern.  Make sure you rename the sketch to something meaningful so easy to pick when inserting it.

You can also place one or more mates onto a Part in the Part Studio (don't forget to rename them to something meaningful...) and then these mates come over into the assembly and can be used to simplify mating.

john_mcclary

dave_franchino said:

I'm struggling with Onshape mates as well - particularly the inability (I think) to access part features in assembly mode and therefore the lack of access to planes and axis which in Solidworks were useful tools.  Pragmatically this has meant I need to have a geometry feature on the part to mate to - whereas there seem to be plenty of situations where I'd like to mate to a construction element as opposed to a geometric feature. I can find ways around this but they all seem like really bad cobbles. Am I missing something here?

That is one of the key differences between Onshape and other parametric CAD.

Onshape does not rely on the feature tree outside if it's own context. (The part studio it was created) since you are able to model multiple parts in one studio in relative position, rather than a having each part in it's own part studio centered on the origin. So default planes and axis are irrelevant except for the first part you draw in the studio. If a plane/axis/or vertex is needed outside of the part studio, then add a mate connector and bind it to that part.

On mate connector in a part studio takes over the job that would otherwise have been (3) planes, (3) axis, and (1) reference vertex.
much more powerful and less cluttered than expanding a part's tree in an assembly and digging out one of those options from a list...

By not relying on the construction geometry of the part studio, that also means that you mate to the relevant geometry of the part itself. Which means ANY imported part is mated the same was as ANY native Onshape part.

So, you can draw a part in SolidWorks, Import it into Onshape, mate it in an assembly. Modify the part in SolidWorks, update the import in Onshape, and it will still be mated correctly.

This also means Onshape doesn't care HOW the part is modeled. As long as the finial part is correct. Whereas SolidWorks is able to read the hole feature and make a derived pattern in an assembly (which is nice, except you have to mate to the seed feature, so you end up mating, patterning, then re-making the mate..) Onshape's replicate doesn't care if you used a pattern or separate features, it will pattern to all circles that size on that face. Where SW you will need to have that design intent figured out while you model the part.