Part studio with multiple states for suppressed features

florian

Hi,

I couldn't get my head around what would be the best way to create multiple part states. E.g.

1. Rapid manufacturing (With machining offsets)
2. Final part after machining
3. Customer version for STEP export leaving out the stuff that make us special

As I am in a rapid manufacturing made-to-order business I want to do the following:

• Have a few documents for each customizable part
• Save a version when the we have a baseline design
• Branch that design for a new customer order and change variables (ideally upload, use a form etc…)
• Create three states of that design (see numbered list above) and export an STL (for step 1) and PDF for simple machining (2) and another PDF and STEP for the customer (3).
  
• Improve the general design in the main branch and save a new version to branch from in the future.

It gets difficult, when I get to the states section. All that is necessary in 90% of all cases is the suppress feature function. I would like to save the states of the features I suppressed and the rollback bar position. Moving around features might break some stuff, but that could be restricted to the main state. Then you could create a drawing by choosing the state that you'd like to import. Same with your STEPs. Maybe even export to filename document - part_name - state.filetype

How would you do it in our cloudy-onshape-rapid-x world?

Other approach:
I could create three versions => That is very manual and if the customer wants one dimension changed I'd have to branch again or create more versions.

Looking forward to your ideas!
Flo

ilya_baran

If I understand correctly, what you are asking for is called "configurations" in other CAD systems and they are on our TODO list.  In the meantime, there are workarounds.  Branching and merging, as you point out, is one.  Another that I shudder to suggest (since it offends my software engineer aesthetics  ) is to make use of variables and expressions as follows:

Suppose you define a variable "state" at the top of your feature list and you set it to 0, 1, or 2.  Then, say, if you have an extrusion whose depth you want to be 4, 3, or 4.5 mm depending on the state, you can enter [4 mm, 3 mm, 4.5 mm][#state] into the depth field of that extrusion.  If you would like to suppress the extrude in state 2 instead, I don't know how to do that, but you can make it fail (which will have the same effect except it will turn red) by writing [4 mm, 3 mm, 1 deg][#state] (or something similarly invalid as the 3rd item).  Note that to be able to commit an invalid input, you will need to have the state variable set to a number where the feature is valid (so you would be able to commit the prior expression if #state is 0 or 1 but not 2).  This trick will also not work to "suppress" features that don't have an input where you can type an expression (like Delete Face or Split).

To simulate the effect of selective rollback (e.g., you have a main state and then some manufacturing features), you can have the main state in one part studio and have a derived part studio that has the manufacturing features.

To reiterate, we will have configurations, but for the time being, some ugly cleverness can save time...

3dcad

@ilya_baran
Wow, so we have 'case' function in variables! This is huge, almost like poor man's configurations..
I did not know about this, did I miss something or is this hidden feature without proper documentation?
Same thing goes for round -command revealed in forum some time ago.. is there more of these?

ilya_baran

I don't believe this construction is currently documented -- but the round function is -- see: https://cad.onshape.com/help/#numeric-fields.htm. We'll continue to improve the documentation, like the rest of the system.

andrew_troup

@3dcad: it's cleverly hidden away    at
https://cad.onshape.com/help/#numeric-fields.htm
under the (slightly misleadingly titled) category
"Accepted unit keywords", which is collapsed by default.

andrew_troup

Thanks very much, @ilya_baran -
I'm sure you have made some card-carrying geek users very very happy. 
I'll post a link to your ingenious suggestion in the "Powerful Workarounds" thread.

florian

ilya_baran said:

If I understand correctly, what you are asking for is called "configurations" in other CAD systems and they are on our TODO list.  In the meantime, there are workarounds.  Branching and merging, as you point out, is one.  Another that I shudder to suggest (since it offends my software engineer aesthetics  ) is to make use of variables and expressions as follows:

[…]

To reiterate, we will have configurations, but for the time being, some ugly cleverness can save time...

Thank you for the answers. configurations is what I meant. Couldn't even remember the German word in pro/e. The list thing is really neat. I'll stay with a bit more manual feature suppression, as I have to enable some booleans. I don't want to make that part fail 10 features earlier as a "feature".

3dcad

andrew_troup said:

@3dcad: it's cleverly hidden away    at
https://cad.onshape.com/help/#numeric-fields.htm
under the (slightly misleadingly titled) category
"Accepted unit keywords", which is collapsed by default.

As I'm not a big fan of 'help documentation' if it's not linked with new feature - I would have never gone there without this post.
Thanks.

I still hope that help get's more integrated into UI so that people like me could get the information without crawling through tabs and digging under collapsed headers.
I like tooltips, if you know what you are doing and move fast only small one appears, if you stop for a while to think bigger one opens with more information. Maybe there could be 3rd stage with even more information and videos on how to use certain feature.    

andrew_troup

@3dcad
I hear you. One particular reason to dislike collapsed headers is that the browser's "Find" will not find words buried under them, such as "round" in the instance discussed above.

I am a fan of authentic simplicity. Synthetic simplicity: not so much.

andrew_troup

Cross-fertilising from another post: a workaround, for those who want to save time digging for nuggets of Onshape's documented functionality
(an acknowledged subset of the actual functionality - but I personally think it would be immature to expect otherwise, particularly in beta)

The entirety of (uncollapsed!) Help can be viewed, or downloaded, from 

https://cad.onshape.com/help/PDF/Onshape.pdf

(Thanks to @john_rousseau for posting the kosher link in another connection)

If the pdf is viewed from a web browser, the rudimentary "Find" (on this page) will locate the "round" function
but it finds that text string within longer words, making things a bit more laborious than if the (latest) pdf is downloaded and the much more powerful search capabilities of, say, an Adobe Reader are brought to bear

lougallo

A quick illustration...



https://cad.onshape.com/documents/e85ffca120784e42ac86c80d/w/69b20e3da3024bb0adbb59ef/e/e086e68f386d4a5e8da35234

andrew_troup

Nice demo, @lougallo

@ilya_baran 's excellent explanation already won my heart, but the reality is actually less unwieldy still than I imagined.

Even in this quite potent example, where some features change size while others are effectively suppressed.

florian

Just a quick update on another possiblity to do configurations as I need them (configs for customer, rapid-prototyping, manufacturing):

• Create your base geometry (sometimes a split might be needed at this stage)
• Derive the needed parts for a certain config into a part studio
• Model away with the derived parts (booleans are your friend)