Configuration variables vs configurations?

S1mon

Is there a way to build a part studio using configuration variables, and then have a list of configurations to choose from (not an infinite variety)?

For example, let's say I have a part called "box" which is simple cube extrusion. I set the #sideLength as a configuration variable with a default of 50mm and a range of 10mm to 100mm. Then I want to have a "small", "medium" and "large" sizes (let's say 10mm, 30mm, and 90mm for #sideLength).

Other than going back in and getting rid of the configuration variable and just configuring a regular variable, is there a way to do this? I like the flexibility of configuration variables, but I also like the idea of having a simple list of configs to choose from. Is this something I can do with a derived part?

eric_pesty

I've done this quite a bit. I call it the "infinitely configurable master" model.
The best way I have found is to create a second part studio and "derive" the first one, then configure some lists that have specific values for the config variables. The nice thing too is that it can help with revision management (or even avoid having to create versions) by having this one configurable model used to create a set of "standard" parts where you don't need to modify the master to create a new "standard" one.

Here's an example I created a while back with different way to "narrow down" the configuration options of such a "master" model (see "standard sizes" part studio that's basically your use case):
https://cad.onshape.com/documents/d2d3382aa18189471db96624/w/bfdb4819bc7e743e462a92ad/e/257db9494bc229d5216ec85f

S1mon

@eric_pesty

THANK YOU. I was about to try derived models as my next step to see if this is indeed how it works. Your example makes the power and flexibility of this very clear.

I have to say that configurations in Onshape are incredibly powerful in ways that I haven't seen in other CAD systems. Maybe I haven't investigating the alternatives enough recently.

eric_pesty

No worries, you were on the right track with deriving and I happened to have an example ready to go from a previous discussion!

And yes this works very well and we have used it successfully a number of times for things like:
- Pop rivets we have a master model and then derive that in to create different sizes that we can show in the both "unformed" and installed (in different thickness materials).
- Families of electrical terminal blocks/headers etc.
- Rubber grommets instead of downloading a various STEP files
- Electrical contacts like ring or fork terminals
- Etc

My biggest complaints with configurations in Onshape are the fact that you can't make two configurations of something appear as a single item (in BOMs of for releases), and the fact you can't prevent "incompatible" combinations of inputs. Other than that it quite flexible and really easy to use (and maintain, which was always a huge pain in SolidWorks where you spend half your time having to double check and fix broken configurations...)

S1mon

eric_pesty said:

My biggest complaints with configurations in Onshape are the fact that you can't make two configurations of something appear as a single item (in BOMs of for releases), and the fact you can't prevent "incompatible" combinations of inputs. Other than that it quite flexible and really easy to use (and maintain, which was always a huge pain in SolidWorks where you spend half your time having to double check and fix broken configurations...)

Agreed about the missing things in Onshape, and about the pain of Solidworks configs. I spent more time maintaining Solidworks configs than I did using them. Using configs with inserted models (equivalent of derived) was very flaky. 

chadstoltzfus

We also have adopted this "templated" style of building configurations. As a business, it's immensely helpful for maintenance. It's a lot easier to add a specification change to a master template and run a macro (or API) to update documents using that template instead of going into 100+ configurations, adding a new config option, and configuring potentially differently structured feature trees. Then again, we do use configurations a little bit differently than how most businesses do. 

That being said if you care about the order of the configuration parameters, moving them up and down the list can be annoying if you create a new parameter in the template and need to add a parameter to multiple configurations. This became so much of a pain point that we actually developed JS code that we can copy and paste into the console in the inspector and with some tweaking, will move the config parameters using a programmatic loop. 

I ended up doing a user group presentation on some of the powerful hidden functionality of configurations, maybe I should make a YouTube video on it sometime. 

EvanReese

chadstoltzfus said:

I ended up doing a user group presentation on some of the powerful hidden functionality of configurations, maybe I should make a YouTube video on it sometime. 

Please do!

shawn_crocker

I use the derive method usually as well. I make a configured master studio that potentially has lots of parts. Then I derive each part into its own studio so that it can have its own set of configuration inputs that are suitable to that specific part. I don't like using parts from a configured multipart studio because everytime you insert a part into an assembly, you potentially has loads of inputs to consider when possibly only one input actually has a geometric impact on that particular part. Onshape configs are a life save for the type of designing we do.  Sheet metal products that are majorly made from standard parts and assemblies with a few customized options sprinkled in.

julian_julian372

This was the example on mastering configurtions i was looking for.

onshape needs to incorporate this post / example into there configurations tutorials. 

romeograham

We've settled on this method as well - doing "design" work in a configured part studio, deriving each configuration into its own part studio tab - and then releasing from there. This makes it much easier for casual viewers of the document (say, project managers or other engineers that are not designing these parts) to see what each part is. Then, these parts are used in assemblies and drawings.
This means that the trail of breadcrumbs from a top-level assembly goes through these clean, simple part studios (with a single part) down to the messy, configured, multi-body design Part Studio. 
Also much easier to move parts / tabs / drawings in & out of documents, since they already live in their own tab.
You'll need to add any sketches you want in your drawings to the single part studio tab (since they won't show up in a drawing even if you derive them in to the part studio).