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Best Workflow for Symmetric Assemblies
![steve_cohen](https://cad.onshape.com/images/placeholder-user.png)
I'm working on an assembly that has planar symmetry without mirroring, i.e. all the parts on the left are the same on the right, with each part the same distance from the center as its twin. I tried linear patterns, but every distance is different, and I need to change two different dimensions to move both parts. Symmetry is not easily preserved.
I can just make two instances and offset a fastened mate for both from a central mate connector, but then when I move one side, I have to find the other side and change that mate too. I can't use variables to make them consistent, since that is not available in assemblies, but at least the distances are the same.
Is there a better way?
And is there a better way to simulate a central plane?
I can just make two instances and offset a fastened mate for both from a central mate connector, but then when I move one side, I have to find the other side and change that mate too. I can't use variables to make them consistent, since that is not available in assemblies, but at least the distances are the same.
Is there a better way?
And is there a better way to simulate a central plane?
0
Best Answer
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steve_cohen Member Posts: 27 EDU
I think the answer might be what John said.
Layout sketches (in a PartStudio) can have symmetry, and can then be inserted in to an assembly. The symmetrical parts can then be mated to the sketch in the assembly. One dimension moves both parts, keeping them symmetric. It is a little awkward, but it works.
Even better would be a way to make planes symmetric in a part studio.0
Answers
then use a transform/copy in the part studio using two adjacent points.
or use those points to create mate connector offsets.
After creating the parts on the left, use Transform by XYZ and check Copy parts.
When using configurations you can adjust the parameters and toggle on and off
https://cad.onshape.com/documents/77baa8153589a7fc5f289829/v/f34206305bd673c93758b47b/e/181cb871f3008e6b885df46a
it lets you take a measurement of pretty much anything, then saves the result in a variable
But you could make an in-context reference
Could you please explain the process from beginning to end? Thank you for your patience.
If you just want something like a global variable:
Create a blank featurescript,
// Global variables here
setVariable(context,"NameOfVar", 7);
};
Then you insert that featurescript at the top of every partstudio that you want to reference that global variable #NameOfVar
you can do all of your calculations in the featurescript and store all of your variables there if you like.
Then output the results using setVariable();
You can have as many as you like.
---------------------------------
Otherwise, you can create a layout sketch:
Make a partstudio that contains layout sketches that you can mate to
all your calculations would be done in this part studio, then derive this layout sketch into any partstudio/assembly that you want to attach to.
Dose that make any sense?
Here is a video from Onshape showing how it works
https://www.youtube.com/watch?v=Rvu9763-2I4
Layout sketches (in a PartStudio) can have symmetry, and can then be inserted in to an assembly. The symmetrical parts can then be mated to the sketch in the assembly. One dimension moves both parts, keeping them symmetric. It is a little awkward, but it works.
Even better would be a way to make planes symmetric in a part studio.