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part templates

rick_conardrick_conard Member Posts: 23
I am looking for a way to create "part templates" in Onshape.

In Solidworks, you can create part templates that allow you to start a new part with a pre-existing set of features.

Is there a way to do this in Onshape?


Answers

  • MichaelPascoeMichaelPascoe Member Posts: 593 PRO
    edited September 2
    Are you familiar with configurations and deriving parts? You can make a part or "template" and derive it wherever you like and change the configured values on the spot. You can also derive parts from other documents. 




  • shawn_crockershawn_crocker Member, OS Professional Posts: 263 PRO
    @rick_conard
    Onshape offers many options that at first glance, sometimes seem incomprehensibly different. But I have usually found them to end up actually more capable of supplying a need in a more direct manner. I would concur with @MichaelPascoe that deriving is a create way to achieve a template type workflow. The benefit to implementing a derived style of templateing is that every part you make that is built on top of the derive, does not get broken away from the derived "template". An umbelical chord is left attached and can be updated if a template level change needs to be made that you would like to easily propagate to anything that references it. Onshapes derive feature is extremely powerful and my current hyper efficient workflow wouldn't exist without it. Alas, if you truly want the SolidWorks experience inside Onshape, you can create a document with a part studio setup the way you want. Anytime you want to create a new part from the template you can right click on it and select "copy document". You will be immediatly launched into a copy of the template document.
  • rick_conardrick_conard Member Posts: 23
    Thanks very much Michael and Shawn for your replies.   I'm curious about your "hyper efficient" workflow.

    That helped me understand a lot,   and it led me to another question:     In solidworks,  we always used the part number as the filename, and thus the assembly tree showed the part number, and that was a unique number.     However, with Onshape,  what shows in the assembly (or studio) list is the "part name."  If I want exported assemblies to show the part number,  I think I have to use the "part name" property for the part number.   However,  I see that the "part name" is not a unique thing,  i.e. if I copy a part studio to a new tab in an existing document,  the "part name" is the same,  but the parts are not linked.   So, you have the same name (or number)  but different parts.

    What is your recommended way to handle part names , numbers,  and avoid possible duplicate numbers,  and if possible, have assembly exports show the part number in the feature tree?     
  • shawn_crockershawn_crocker Member, OS Professional Posts: 263 PRO
    @rick_conard
    I do not name my parts a part number. I did in SolidWorks for reasons probably similar to yours. In Onshape I take full advantage of not needing too and really just name them something short that lets me identify them for what they are quickly in the assembly. Often they are the same as what I put in the description but usually a simplified version of the description. On configured parts (almost everything) I often use a custom feature that can change the name based on other configured data. For example, all my fastener names change based on what configuration iv selected to insert. The name of a part can change within an assembly but the identity of the part remains the same so no broken things happening. This ability Onshape gives us really removes that nasty feeling that somehow one must instill logic to part numbers only to need a variation in the future that doesn't fit the format. Part numbers in Onshape do not ever need logic because of the way part names work and how configured components automatically find the part number that was assigned to it. As for my hyper efficient workflow, it's basically a wonderful setup of configured parts many that are built from derived features. In Onshape you can create a master part studio where you can design a whole bunch of parts that need to work together very fast and very messy if your just trying to getter done quick. You can then configure the studio to allow for practically any variation you will need of the things. Then you can derive the parts into there own part studio and then configure that studio to drive the configurations of the derive feature. Then everything is nice and neat even though you got to accomplish the neatness through messy "hyper" efficiency. Really I'd say Onshape allows for a workflow I tried for years to accomplish in SolidWorks but could never attain due to having to over come the new bug that popped up around the corner everytime I got close to the goal. Configurations in Onshape allow the same abilities as driveworks express minus the drawing creation. And minus the negative impact of every exported project being completely detached from the master. In Onshape it remains attached and a new variation can simply be selected rather then completely recreated and exported.

    Ps. Check you personal account settings in preferences right at the bottom. You can setup naming schemes for exported items and can have the part number automatically included in the name. If your using a paid account you should have this ability also as a global company definition as well.
  • rick_conardrick_conard Member Posts: 23
    Shawn,  thanks for your answers.     So,  it seems that it is possible to have two parts have the identical part name and part number and yet be two totally different parts.    Am I correct?    Maybe that is not a big issue but it does seem worrisome.


  • shawn_crockershawn_crocker Member, OS Professional Posts: 263 PRO
    @rick_conard
    That is right.  Can be identical.  It seems worrisome until you are in an environment where it matters like if you end up getting a professional account with release management available to govern things for you.  Once you have release management, it will not allow you to release two part numbers at the same time or will attempt to automatically create revisions of part numbers that overlap by accident.  It basically makes it near impossible to mess up your stuff (but we all know that its never going to be impossible).  At least with onshape, you know you will never be accidentally and irreparably overwriting something.  you may accidentally release something using the wrong part number which ends up revisioning something you did not intend, but everything is still there and you can push the older revision that should not have been revised, forwards to have it take precedence again.  Doesn't happen much though as the releasing environment is pretty clear about what is about to happen as long as a point it made to actually examine what its showing you.
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