Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Locking a released file

Dear all,

I have released a part in Onshape, and after release it is possible to make changes to this part without any warnings. I have experience working with Windchill and 3DX at two companies and in both situations the PLM/CAD systems were configured that user could not edit released files. When you select a feature and try to change a dimension you get warnings. At this stage you need to create a new revision that would get the status "in work" and you are able to make changes. 

Is it possible to configure Onshape to do the same? 

Best Answer


  • tim_hess427tim_hess427 Member Posts: 642 PRO
    All releases (and versions) are read-only. The thing that trips people up is that onshape automatically creates a new workspace for editing (whereas that would be a manual thing in windchill). No matter what you do in the workspace, previously created versions and released items will always be available with permanent links. 

    I admit its a little weird and seems to be a "design work" focused default arrangement, whereas I can see in many situations you want users to have a "retrieve released data" default arrangement. 

    I'm hoping that onshape will work on something, even if its something like a "view only" interface, or a way to automatically open the latest version/revision of a document rather than the most recent workspace. 
  • Dennis_VarkevisserDennis_Varkevisser Member Posts: 13 PRO
    Hello Tim, 

    Thanks for your reply. I am still struggeling with my way of working within Onshape. When I was just moddeling I made around 10 parts and drawings within one Document. This worked quite okay. I had for instance all parts of an subassembly and the subassembly + drawings in one document which gave a nice overview. But once I start to use releases and revisions this Document approach start to show some disadvantages: If I release one drawing and part and want to show the correct drawing so I can send it to a supplier I need to do the following:
    - Point the drawing to the released part using "change to version"
    - Now my drawing is still showing a "in progress" watermark. because the drawing itself is the Main version and not the release version.
    - Now I have to select to show the released document. this status is for the complete document so for all parts and drawings included.
    - If I want to work on another drawing that has a different status I need to change the status again also showing the watermarks on all drawings. 

    To overcome the above workflow I now only make 1 component documents just containing 1 part and its drawing. 
    What is your approach on this?

    Best regards,
    Dennis Varkevisser
  • Dennis_VarkevisserDennis_Varkevisser Member Posts: 13 PRO
    Thanks for these tips Tim!
  • shawn_crockershawn_crocker Member, OS Professional Posts: 334 PRO
    I don't let myself get too worked up over where and how. Properly tracking changes is the job of the document control system not the user in my mind. Onshape has certainly done a magnificent job of nailing that down. What some people may forget or be unaware of is you can pin down references. A typical thing I do, is create all the parts for an assembly in one part studio which ends up in its own document. I then create an assembly linking to all those parts. Now, what used to bother me, was if I changed the part studio but only one part of in the studio was affected, the assembly should want to update all the parts to the newer version. If the assembly was released, many parts would have there rev bumped redundantly. What I do now is pin the assemblies references and selectively update just the part I know changed. When releasing now only the one parts rev gets bumped. One rule I usually do follow for configured product models is having only one tab per document associated with the top level assembly and generally keep all drawings out of those documents. Because its configured, I'm wanting to be able to keep everything drivable by the top assembly. If other tabs were in the same document, I would have to start replacing components the are not changing with releases which would break the documents configurability.
Sign In or Register to comment.