copy a sketch/features from one part studio to another still not possible in 2020?

glen_dewsbury

Yes I agree, you're missing the zen. You can use the derive function across documents. You'll want to identify a master document with the initial sketch then use it any where you like. Not sure why you want to copy and paste from document to document when you can use existing sketches and parts from any document. Unless your getting too complicated to track in one document you can work with multiple part studios and assemblies inside one document. If what your working on is not to complex you can build all parts in one studio and then put together an assembly for motion study or multiple uses of the same part.
https://cad.onshape.com/documents/2679577427d13b4e8513a641/w/1e9edde7e2cde1617682453f/e/40c61813a15e5397d9823bc8
https://cad.onshape.com/documents/296a16ab7f5422287828dd13/w/808473937c84e0aa22c65eb3/e/d1bb6caef4acf06943a1fd14
Having a separate document for every part you make is pretty old school and was because it was a requirement for older CAD systems.

eric_pesty

There are other ways to deal with this too, you could have a simple part that is just the Tenon and "derive it in" to any existing part (locate with a transform or use the "super derive" to place it directly). You can then boolean add it or remove to create the geometry in your new part. I don't see a need for bringing just the sketch/feature for this use case.

nick_papageorge073

timothy_kolar said:

...snip....

However, for me a small bowl, a benchtop vice, and the plastics for a set of soldering "helping hands" all belong in different documents with their own sets of variants.  Putting all of them in the same document as variants of one another doesn't seem right to me, but it's possible I'm missing the zen of this. 

I have the feeling from what you wrote that you have everything you ever modeled in onshape in one document, perhaps even one part studio, even though they are not related to each other. Is that correct?

If that's the case, you are definitely doing it wrong. One document per "product". One part studio per "subassy collection of parts". One "subassy" for each part studio. Then one "top level assy" for the collection of subassy's. That will get you on the right track. As the complexity of the "product" increases, you would split it even further than this, but in the beginning this is appropriate.

nick_papageorge073

timothy_kolar said:

I may have missed the resolution to this, but here is my use case for copying parts of sketches between Part Studios.  I'll be first to admit there's an easy workaround, but copy and paste would be the obvious solution.

I have a wide variety of parts that serve many different purposes, but they are modular -- you can connect any one of them to another.  It would be very convenient to paste the mortises and tenons between them.   Once again, the parts are not variants of one another, they just share a single small element.

Today, for example, I am taking a part that was not originally modular and converting it.  Copying just a mortise and a tenon to the new part would make it easy to guarantee compatibility.

To help visualize, here is an example of a center piece with mortises on the top and left and tenons on the bottom and right.  You could easily build a grid out of these pieces.

In a case like this where there is a common interface between otherwise unrelated parts, you can model the interface by itself, and then bring it into every place you need it.

In this case have one part studio that has a shape representing the mortise and the tenon. Nothing else in that part studio. (Ps did you mean sliding dovetails).

When you want to apply that common interface to a new part, derive it inside the part. Then use "point pattern" to place it at all the locations it needs to go to. Then use boolean to ether union it for the male or subtract it for the female shape. You could make all 4 dovetails in this part in a couple minutes once you get familiar with the process. If the fit is not good between male and female, you would adjust it in the original part studio, and then when you update each part, it will get the new clearances.

nick_papageorge073

@timothy_kolar

Here is what I was describing above. Its robust, because if you find out you have a fit issue when you manufacture the parts, changing it in one place will change it for each of your modular blocks. I did have to add a few steps to get the rotation of each dovetail correct. IDK if there is a more efficient way of doing that. This document uses two custom features, super derive and point pattern. Both comes in super handy on many projects.

https://cad.onshape.com/documents/031a5e33b26fb624a173277a/w/ad8f1b327f71709a55f20dce/e/e07777c5f6928226de965ab5?renderMode=0&uiState=6367d83ee993db6c1c7677e6

eric_pesty

Here's a much simpler way of doing it adding mate connector to the dovetail parts and using the "transform pattern" feature:



https://cad.onshape.com/documents/c7971a04ce49f973b601aa5f/w/57799bf154d78f0f0314ea3d/e/972005ef692f2eb073fa3a5f

timothy_kolar

I have the feeling from what you wrote that you have everything you ever modeled in onshape in one document, perhaps even one part studio, even though they are not related to each other. Is that correct?

The opposite actually.  But before I learned of the wonder that is Super Derivations I couldn't find a way make sure identical elements matched dimensions across different documents.  Copy and paste between documents would not have been ideal, but it would have beat doing it manually as I have been.

However, Super Derivations solve this problem way, way, better than copy and paste ever could.  This was meant to be a minor comment about a possible cut-and-paste use case but has turned into a sublimely educational experience.

timothy_kolar

eric_pesty said:

There are other ways to deal with this too, you could have a simple part that is just the Tenon and "derive it in" to any existing part (locate with a transform or use the "super derive" to place it directly). You can then boolean add it or remove to create the geometry in your new part. I don't see a need for bringing just the sketch/feature for this use case.

Super Derivations completely obliviate my putative use case while simultaneously solving correctly a problem I've been working around for too long.  Thank you so much for pointing them out!

asko_kauppi

timothy_kolar said:

However, for me a small bowl, a benchtop vice, and the plastics for a set of soldering "helping hands" all belong in different documents with their own sets of variants.  Putting all of them in the same document as variants of one another doesn't seem right to me, but it's possible I'm missing the zen of this. 

My 2c. I see Document as the unit of versioning (and branching). This is nicely described somewhere in the Onshape tutorials.

Thus, if the "bowl, bench top vice, and the plastics" don't share a life cycle, they should obviously not be in the same document, either.