Easy method for exporting sheet metal flat pattern to STEP file?

Vrmithrax

We are using Onshape for design, but when it comes to CAM we are forced to export all of our models to files that are imported into Fusion360 for processing and machining on our CNC router. Until Onshape actually gets their CAM Studio actually running and available to the general public, this is our only option currently.

Now we have a situation - we have folded sheet metal parts that need to have the flat pattern exportable so we can actually machine the part without having to run through a lot of hoops on Fusion360. We worked out how to create flat pattern drawings, but exporting to something like a STEP file seems to be lacking.

I'm used to SolidWorks, sheet metal and flat patterns are super easy there. Even Fusion360 wasn't so bad once you worked out a few of their odd choices. I really want Onshape to be similarly simple, particularly since my "work force" in this case is high school students often learning CAD for the first time, and in a time crunched production environment where there is not a lot of time to stumble around what should be a simple process. Sheet metal design is often the most elegant way to attack some designs, and I'd hate for the students to get a bad opinion of the process.

eric_pesty

A flattened sheet metal is inherently 2D, any reason you need it as a STEP? Can a 2D DXF not work in your workflow?

Otherwise you can insert a flat pattern into an assembly and export a STEP from there…

You could also use either the "flat pattern without edges" FS if you don't want the bend lines to show:
https://cad.onshape.com/documents/d075777b23239493791a6871/v/8725ed1ea47f3c78bf784922/e/dba9566c2dda32a29752e76b

Or the "Flat pattern copy" FS (although this one requires "finishing" the sheet metal model for some reason): https://cad.onshape.com/documents/4357eff2151398c89303c467/v/3bd121d14269dd21d6d52704/e/31206977c0ba652ad907d54a

nick_papageorge_dayjob

Are you cutting the flat patterns yourself? On a laser machine? DXF is what is mostly used for flat patterns in industry, not STEP. And any laser/waterjet machine will accept dxf. If you are instead sending the parts to a sheetmetal vendor, then you would send them a STEP of the fully bent part.

joshtargo

I also have my own Extract Flat FS

https://cad.onshape.com/documents/ee5fe3705045d8cf9e3fe478/w/6c8344d774ce4c4c0e00ad7e/e/2e3c34069cc7000fbe02adb9

michael_hills168

https://forum.onshape.com/discussion/comment/110626#Comment_110626

I suspect that I'm in the same situation (high school robotics competition) as Vrmithrax, so my answers to these questions likely apply. We use a low-cost Omio CNC router for everything from 1/4" aluminum (which we don't bend), to 1/16" polycarb.. I'm not the CAM guy on the team, but as I understand it, for normal 2.5D or 2D parts on our 2.5D router, we export the .step file from Onshape, load that in Solidworks and used HSM Works for CAM. For bent parts, we export the .dxf flat pattern,, import that into SolidWorks, extrude the part to the (hopefully) correct thickness, then us HSM Works for CAM. Thanks to some of the comments above, I might explore generating the .step file from OnShape to make the CAM workflow the same for bent and unbent parts.

I still have one problem: Most parts we do are 2D parts. We occasionally make 2.5D parts for countersunk holes and such. We also occasionally make bent parts. If we wanted to make a 2.5D part that was also bent, it looks like it would be a bit messy and error prone. For example, I might want to make a bent part out of 1/4" polycarb with some countersunk screw holes and a strip along the bend line thinned down to 1/16".. I could make a 1/16" sheet metal model, use one of the feature scripts above to create the flat pattern part, then extrude the non-bent areas to make them 1/4" instead of 1/16", then add countersunk holes or other 2.5D features, but I would have to add those same features to both the flat pattern part to be used for CAM, and add them to the folded part to insert into the assembly. I don't see an automated way to ensure that both versions of the part are the same initially, or after someone make changes. Does anyone know of a technique or feature script that could help with this?

Derek_Van_Allen_BD

Adding to this discussion since my company works with a ton of high mix low volume weird geometry sheet metal parts. Our workflow is to insert the flat pattern states of each part studio into an empty assembly to export each part as a .step file. No custom featurescript or insertion into a drawing tab necessary.

To answer the questions why one might do this over exporting .dxf files: the .dxf file format carries no inherent manufacturing metadata for sheet thickness, part scale, or even something as fundamental as interior geometry vs exterior geometry. That's without even considering the complete lack of industry standard layer mapping convention for notes or etches causing miscommunication between vendors and getting etches cut or cuts etched. Industry standard wisdom is to supply a drawing and communicate specifications when ordering with your laser vendor and this works when you have large quantity orders of repeated parts, but this is the era of instant online quoting via SendCutSend or OSHcut or Xometry or other online vendors. I don't work with orders of 1 of 1000, I work with orders of 1000 parts which are 1 of 1.

.STEP files are far less error prone for high mix low production volume industries and it has become our company's default export format for sheet metal parts even in the flattened state simply due to the amount of waste and error we've determined to come from the .dxf format being insufficient to communicate the true manufacturing needs of sheet goods.