Perf patterns in sheet metal?

S1mon

What is the "best" way to make a perf pattern in a sheet metal part?

And by "best", I mean something that performs well, and is robust for modifications. I'd like to avoid "finish sheet metal" if it's not 100% necessary. I also assume we want to avoid sketch patterns.

Here's a part with a hex hole pattern. We're typically having this fabbed with laser cutting, so having only whole hexes is not 100% necessary, but would be fine.

Is fill pattern still the recommendation here?

nick_papageorge_dayjob

3 years ago I was doing this for a few parts. I was running into very slow regeneration times. Some of my patterns were for EMI of high frequency and were quite small size/large qty. I found that applying the pattern to a separate part first, then bolean subtraction that part to the real sheetmetal, saved a lot of processing time.

I also found the FS's to make this simpler were more resource intense. So I would sketch qty 1 (or qty 2 if a hex pattern), and pattern them to the dummy part manually.

Also found doing this after "finish sheet metal" made a world of difference. I relented to doing it there.

Now, a couple years later, I know sheetmetal has had a lot of performance improvements. IDK if my comments are still valid.

EvanReese

You can use the Form feature, which can be made robust, but I think doing it on active sheet metal will just always be slower than otherwise. Here's an example.

https://cad.onshape.com/documents/ff2551224d4b938373bb2cd6/w/652755f027b9207bad0ded57/e/c337d16436e401aa29c41f94

S1mon

@EvanReese
I like the idea of using the form tool for some things, especially common sized vent patterns for things like a box fan.

I'm curious if Grid Extrude has been updated in a while and if there are any possibilities to make it more robust? We used it (not with form tools) on some sheet metal parts and got weird errors from Onshape about "System failed to resolve part instance display data".

EvanReese

I've not updated it in a while, and I didn't pay much attention to using it with SM at the time. If there's a certain case you can share of the failure, I'll take a look. TBH you might get my example a bit quicker by using Fill on the form tool anyway since it's equivalent to a face pattern, where mine is equivalent to a part pattern. It's more flexible, but at a cost.

bryan_lagrange

Lana has given me this feature script that works like the form feature but is for a cutout library. It works well. It was a quick feature she created and she informed me that it is not fully polished but it is a good starting point.

https://cad.onshape.com/documents/99c9155030f1cee5bc1ae577/v/4bec1a32e8b0dffbcacc2eb8/e/76e7bf34c0459088e72418eb

lana

Currently sheet metal is not suited for handling perforated designs - regeneration performance and memory use are not optimized for it. Two possible sane approaches would be formed feature or sketch in flat. I'm assuming that you want to have the perforation reflected in flat, so you need to have a representation for flat pattern which can be exported with DXF. It seems to me that building the desired piece as a formed tool is the simplest way to to achieve this. You can use Evan's Grid Extrude to build the tool and then use its face to generate the sketch of the form.

Derek_Van_Allen_BD

@lana unfortunately for our team sane approaches don't work on sheet metal cones.

For this part we did our patterns and booleans to a non sheet metal body first and did a sheet metal thicken to build the final geometry. You could also finish your sheet metal part first, do your pattern stuff, and use the Sheet Metal Model+ custom feature to take advantage of the Recognize functionality of the custom tool, though it's using the old sheet metal kernel and doesn't work on cones, hence why we had to do this. Just be careful to select the right version of the flat pattern for export.

There are probably a dozen ways to do this but to me it's a hard requirement to avoid any that break geometric parity between the 3d and 2d representations of the sheet metal. I'll happily sacrifice performance knowing that my holes are going to end up being the right shape and in the right locations. I've also banned the team from using .dxf files as a manufacturing format because there's too much ambiguity left up to the vendor due to deficiencies inherent in the format itself. Even when we send flat representations of our parts we send them as .step files because it's harder for a vendor to misinterpret the geometry and send us out of spec parts.

EvanReese

https://forum.onshape.com/discussion/comment/119424#Comment_119424

I don't think this has been made public

Derek_Van_Allen_BD

Any chance you could share that doc @bryan_lagrange ? Writing a tool that works like the form tool but that executes cut geometry is in my backlog of features to write.

bryan_lagrange

@Derek_Van_Allen_BD @EvanReese I am not the owner of the document for this feature script so I can't give permissions for it. You can send @lana a message about getting access to it.