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Sheet metal and Derived feature.
robert_stiles
Member Posts: 147 PRO
in General
Hello -tricky one here...
If I had a sheet metal part defined in a parts studio. I brought that in to another parts studio using derive, at a given configuration which is differnt to defaults, along with other instances of that parts studio with differnt configurations, and other parts studios also with sheet metal definitions, can I collect all the variations of the sheet metal out put? unfolded?
Please don't suggest assemblies. Until onshape enables feature script within assemblies, there is no way we can bring all the parts studios into an assembly.
(at least, if it did work in assemblies, I would have to create an assembly just for the sheet metal output, and have a replica parts studio to do all the other things our feature scripts need to do)
Any suggestions gratefully received. Thanks
If I had a sheet metal part defined in a parts studio. I brought that in to another parts studio using derive, at a given configuration which is differnt to defaults, along with other instances of that parts studio with differnt configurations, and other parts studios also with sheet metal definitions, can I collect all the variations of the sheet metal out put? unfolded?
Please don't suggest assemblies. Until onshape enables feature script within assemblies, there is no way we can bring all the parts studios into an assembly.
(at least, if it did work in assemblies, I would have to create an assembly just for the sheet metal output, and have a replica parts studio to do all the other things our feature scripts need to do)
Any suggestions gratefully received. Thanks
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You can do multiple derive ins of different configurations of the same source (you can pick the configuration in the derive in feature), but when you derive in a sheet metal part you just get the solid so you won't get flats right away...
You'd have to "convert" them again to sheet metal (just need to use a "thicken" with correct thickness and bend radii, etc...), which you might be able to automate with featurescript...
You might also be able to use the "unfold" feature to create "flattened" configurations of the parts before you derive them in.
I'm assuming you want to nest these afterwards using featurescript?
The unfold feature you have pointed me to in your reply is just to pinpoint the unfold code so I can adapt it in one of our custom features right? Its not actually supposed to do anything as a feature tool as it is there? because it doesn't do anything!!! Thanks though, this is a very useful start point.
The nesting... currently we use an external nesting once we have the dxfs out. Our dxfs have multiple layers, for multiple tool operations, and we need to control grain direction and priority, etc. One day we might have a process that runs in onshape, but its a little way down the list. If you are interested, after some long investigations, we settled on nestfab for now. Its very good - https://www.nestfab.com
Another question please. Why when I run the finish sheet metal part feature, I can only select one part? It seems to close out the sheet metal operations on the all the sheet metal parts in the parts studio, not just for the single part I choose to select in this feature? I get that purpose of the feature is to close out those specific sheet metal operations, just as the create sheet metal part starts them. (We have a similar thing, we call book ends on some of our features), but... what's the point in being able to select one part? is it doing anything else to that part I've not realised? either it should be able to select multiple parts, or it should not need a part at all, and just be a close out book end. Otherwise its a bit confusing.
Thanks
The "unfold" has worked for me before so I'm not sure what's going on...
I guess my other question would be why you need the flats to all be in the same part studio as it seem like a cumbersome step to take (but I don't know what you are trying to achieve...).
If you are running featurescript, could you not just run it on multiple parts rather than require bringing them in? If that doesn't work I would look at bringing the parts together in the featurescrip rather than manually deriving them into a single part studio...
for deriving multiple configurations of the same part (or multiple parts) you can use Ilya's Super Derive feature
3 years later, and I've come up against this problem again. Sheet metal is not an area of onshape I spend much time with. Any updates on how I can solve the original problem? i.e. getting the data out of derived sheet metal parts with out rebuilding them?
@robert_stiles , Derive now has the option to "preserve active sheet metal models" so you should be able to derive a bunch of them into a part studio and have all the sheet metal related data, hopefully that helps?
Although that still won't give you all the flats in one place (they will be under different sheet metal "drop downs" in the flat view…
There is this FS that creates a "flat without edges" that might be useful (at least to "steal" some of the code)? https://cad.onshape.com/documents/d075777b23239493791a6871/v/8725ed1ea47f3c78bf784922/e/dba9566c2dda32a29752e76b
Going back to your earlier comments, I can't imagine it would be difficult to create a FS that allows "finishing" multiple sheet metal features at once… Just a wrapper for the "native" one that just applies it to all your selections…
Finish sheet metal now accepts multiple selections and can handle multiple sheet metal models.
Thanks, Interesting. We are using our own (now quite complicated) derive super feature, and I've ask Sam to look at introducing that "preserve active sheet metal models" as an option within it. Hopefully not that hard (but its doing even more than Ilya's super derive!)
@lana yes thanks, I did see this had matured. Thanks.
Ok, so its not very easy to add this to our feature script apparently. Something to do with that functionality not being extend down all the functions enough, a top level thing within the derive feature? We might add it in the future, but we have no resource to look at this right now.
My next idea is to make suppress the sheet metal parts, retain any surfaces or geometry in the product that is derived in, and remake the sheet metal parts in that studio from the retained geometry.
I know, someone will say, thats not the intended workflow in onshape, parts should be put together in an assembly… But that's just not how our derive chain system works.
However, just to check I'm not missing a trick here, please can I ask about assemblies. Lets say I had a sheet metal part (defined in another document), with lots of configurations, and I bring that in to an assembly with other parts. What happens then? What's the work flow to get the sheet metal flat pattens out? you can't do in context modelling, because there is no sheet metal properties carry through? and if there is data there, how do I get it out? (I must admit that when I tried this, I was going via another parts studio… is it that step that strips out the sheet metal data?)
Thanks
@robert_stiles at our company we've been adopting a workflow where we'll derive all of our sheet metal components into a single export part studio where we use the default derive feature with sheet metal contexts enabled to bring the flat patterns in with the derived folded parts. Then we'll apply a custom mass-flattening feature to copy the flat pattern bodies of the sheet metal contexts into the 3d space and delete the originals, grouping the components into composite parts with similar thicknesses/materials so we can right click export the composites and export as .step files in zip folders. (.step instead of .dxf because we don't trust vendors with .dxf files)
I'm actually not a huge fan of this workflow in its current state because the only time we actually want to flatten our parts is when there's rolled geometry on a sheet, which our main vendor can't flatten at the moment with their unfolding engine. We prefer to send everything in the folded state because there's way more manufacturing information captured in the 3d representation of the sheet metal than the flat pattern. I would like to have a selective query that flattens only parts with rolled faces but I haven't figured out how to bake that into the flattening script yet due to lacking a sheet metal attribute that defines a rolled face as actually being rolled. Additionally we end up in a spot where we might have 20+ derive features in our export studio and it would be helpful to have a multi-derive feature that drags all of the sheet metal parts in at once.
It's better document control than the assembly method though, which is why we started doing it. Previously we were just dragging in the 3d or flats into an assembly and exporting from there, but because assemblies don't let you featurescript there was no way to apply material groups or names to parts with that workflow unless you already had it set up in your part studios.
@Derek_Van_Allen_BD Using the assembly method, you had already flattened/unrolled the sheet metal when you bought it into the assembly? or is there a way to export flattened sheet metal from the assembly I have not found yet?
Our problem, I think, is simply the fact we have not enabled the sheet metal contexts in our adapted derive feature (and for whatever reason, adding this now seems to be more complex than I thought). I could use the Onshape native derive, but ours has so much in it now, controlling project wide materials, merging parts, driving geometry from regions we define in a General Arrangement sketch etc etc, its probably simpler to re-make the sheet metal parts in the final parts studio from a set of driving geometry parts. If I'm smart with that driving geometry, its not so bad… but still annoying because its something we will have to do every time.
I think it would be best (for us) if Onshape could go and fetch that sheet metal data from the studio it is defined in, even with a refresh, pointing at a version, it would not have to be live updates. Sometimes though, that might be 3 derive chains deep.
@robert_stiles when you insert sheet metal parts into an assembly you can instead insert their flat patterns. Super quick way to get stuff sent out but it removes all of the nice featurescript stuff I've got built into our export tool.
They added "Preserve Active Sheetmetal" checkbox to derive a while back
That should keep everything you need
I use it for a "start part" for our sensor brackets that bolt to Unistrut.
they all start with this, and I just add flanges to make the final part.
In this example, it's configured so I can set the sheet-metal thickness and bend radius at the time of derive
it even keeps properties and mate connectors as well