Break In-Context References

sean_blanchard

Is there a simple way to break the link of in-context references? For instance, if I create a rectangular extruded block in a parts studio, then decide to create another extruded block from the existing face of the first block; using the project/convert tool in the sketch environment. Is there a way to break the link of the project/converted sketch, without deleting the sketch?



There is a similar feature within Autodesk Inventor called "Adaptivity" which allows the user to toggle on and off, removing the reference from an existing in-context part. Or, breaking the link all together.

lougallo

@sean_blanchard I moved this out of the improvement area since it seems more of a question.  Remember our context are not dynamically updated so there is less need to break them.  You are not going to force update like most cad packages do.  They are essentially locked until you need to update.. if you never update they basically stay the same.

billy2

@sean_blanchard

Just delete the external reference and the "in context" relation is gone. Look for purple things in a sketch which marks external constraints. Purple is external. Also, re-route external "up to" references to local.

I constrain to match external geometry, delete the constraint and add dimensions all the time. It's a good way to use "in context" and it's also a good way to manage "in context".

philip_thomas

And of course, the question that begs to be asked is "why do you want to delete the references?".

billy2

Are you asking me or is this in general?

philip_thomas

@billy2, i was asking @sean_blanchard

sean_blanchard

@philip_thomas in other CAD platforms, sometimes you want to break the link to the reference geometry to prevent unnecessary/unexpected changes. Therefore, I use the geometry to help construct the desired geometry, and break the link, when I've completed constructing the new part.

john_mcclary

You will need to delete your references manually like Billy2 said.

But what Onshape staff is telling you is, you don't have to...

The way Onshape in-context works. You can make something in-context. then delete the whole assembly. and that part will still be unchanged. 
There is no auto-update. So if you move or change something in the assembly, then nothing will happen to your part.
Until you manually right click the part and choose update and then also choose WHICH context to update.

You have so much more control in Onshape's in-context that breaking becomes an unnecessary step. Breaking should be considered a "work around" that other CAD systems have beat into your head as "The way"

Otherwise the easiest way is to just delete the context right in the part studio. 


as you can see after deleting the context is broken, and the geometry is un-changed


But any edit will need to still be manually defined, as you can see it remembers the last known good context, but deleting the reference will kill it for good

philip_thomas

@sean_blanchard - Totally agree. In other cad applications, the unchecked propagation of changes was something that we knew was a problem (after all, most of us worked on SolidWorks) - and wanted to fix this in Onshape.
Our solution was linking to versions-or-revisions (either in the same document or across documents) - that way, you get to choose whether you want to update to any newer version/revision and even if you do and later decide that that was not what you wanted, you are free to roll back to any previous (or newer) version/revision. This totally sidesteps the need to break external references and prevents that blown-up-assembly-tree problem  
Please let me know if you have any questions on how to take advantage of this amazing capability

sean_blanchard

@john_mcclary and @philip_thomas Thank you for the feedback. This information was truly helpful.