Reusing Parts

tlewis3348 · February 2017

When I use SolidWorks to create small standalone assemblies, I generally store all my files in a single folder dedicated to that assembly. This is generally fine because I'm not going to be reusing those parts elsewhere. However, this approach can become problematic when I am using the same parts in multiple different assemblies. If I were to have a copy of that part for each assembly, I would end up with countless copies of each. This not only results in extra space being used on the server, but also significant problems if the supplier updates the part. As a result, I have created a database of parts where each part is stored according to its description rather than according to its use in a given assembly. As a result, any time I want to add a specific part to an assembly, I merely need to find it in the database.

I say all that to say, although I haven't used OnShape much, I get the impression that it is well suited for building small assemblies where parts aren't reused extensively. I know that a part (or assembly) can be moved to a new document or added from an existing document. However, the closest thing that I see that would allow me to accomplish what I'm talking about is to have a single document with multiple levels of folders storing parts in folders according to their description. Then I would be able to grab parts from that document for every assembly I create. However, when I go to grab a part from that document in a separate assembly (by selecting Insert parts and assemblies --> Other documents), the resulting dialogue does not show the folder hierarchy I created in the document. Furthermore, I noticed I can tag my documents, but those tags aren't exposed when I'm looking for something in the insert dialogue.

Ultimately, I'm not sure whether I'm just missing something, or if I'm trying to use OnShape in a manner that it was not intended to be used. So my question is, what is the best strategy for managing parts that will be getting reused in multiple different assemblies in OnShape? Is this something that OnShape can handle?

bradley_sauln · February 2017

This is where the power of our linked documents come into play. The most important thing to remember is to keep an open mind because we are not a file-based system. That means that the workflow will be different from what you are used to (which is the folder structure you've described). Here are two links to get you started:
https://www.onshape.com/cad-blog/tech-tip-how-to-use-linked-documents

http://www.solidsmack.com/cad/onshape-linked-documents-do-more-than-you-think/

Once you've gone through these, let me know if you want to discuss further.

The structure will be to create a team and you can call it a "Parts Library" and within that team, have documents for your components. I have documents by part type. When using Linked Documents you also need to utilize our versioning.

konstantin_shiriazdanov · February 2017

In the future they have no way but add the functionality of standart part libraries, and this functionality could also be used for user components. But before OS team have to manage with basic functionality, which is still not full

carl_von_ayres · February 2017

What your talking about is a user library and is something that onshape handles well. What i do this create a label 'Library', then for each type of standard part I create a document (i.e. one for switches, another for MCBs, etc) and assign them all the label 'Library'. From the front page i can select my library label for quick access and when i am working in a assembly you can click insert 》 other documents 》 library (in a recent update they added user labels to the bottom of the list) where there is then a list of all my library documents.
You can also build up your library later after your first couple of projects by right clicking on parts or assemblies in the document list and select move to new document (this will move the parts for future use and inserts of linked copy into your original document). This allows you to work in a local document and only when you want to reuse parts move them to your library.

Hope this help

Hopefully its clearer with pic, below is on my homepage with the Library label:

Image: https://us.v-cdn.net/5022071/uploads/editor/ba/s5dxm3h7883t.jpg

In my assembly, I select inset then other documents and you can see the my labels at the bottom:

Next you click on the label and it brings up my library documents

Finally I select the part or assembly that I want to link into my current document [as these are multi-body parts I normally bring them in as a assemble with the part no attached to the assembly]

Image: https://us.v-cdn.net/5022071/uploads/editor/5z/b1xfuqwx500w.png

One final tip, when you are importing a lot of models it is a good idea to create a temp document for importing and tidying up the model before you move it to your library. Otherwise your libraries will become >100Mb quite quickly and slow the loading.

bradley_sauln · February 2017

carl_von_ayres said:

What your talking about is a user library and is something that onshape handles well. What i do this create a label 'Library', then for each type of standard part I create a document (i.e. one for switches, another for MCBs, etc) and assign them all the label 'Library'. From the front page i can select my library label for quick access and when i am working in a assembly you can click insert 》 other documents 》 library (in a recent update they added user labels to the bottom of the list) where there is then a list of all my library documents.
You can also build up your library later after your first couple of projects by right clicking on parts or assemblies in the document list and select move to new document (this will move the parts for future use and inserts of linked copy into your original document). This allows you to work in a local document and only when you want to reuse parts move them to your library.

Hope this help

This is a great workflow @carl_von_ayres

jochen333 · February 2017

Thats similar to what i do.

I have a document called Standard/DIN-ISO-Parts, where i put all purchased and non-altered parts (DIN is similar to your ANSI).

Then another document where i save all company related parts, whether altered Standard-parts or on-purpose built parts that i need on several places.

That works like a charm.

owen_sparks · February 2017

I too like this workflow.

For common parts I'll be writing a featurescript that does pretty much what the existing derive feature does but pre-populated with some menu structures for my most common parts and families and with the addition of a "derive here" option to save having to transform it into place.

Owen S.

carl_von_ayres · February 2017

Using featurescript to create standard parts is also a excellent idea, I plan to do this for DIN rail and trunking but its slow going.

jason_li079 · February 2017

I created a library file too, but look like the part property is not go through to the BOM, when I generate a BOM for the assembly. Do you guys have the same problem?

stevehess · March 2017

@carl_von_ayres

Very nice yet simple use of Onshape linked docs and labels. Thanks for posting.

Reusing Parts

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