Export for sheet metal bending (Solidworks) problem

I researched forum for problems related to sheet metal bending - found similar problems, but couldn’t figure solutions or real causes to the problem I just encountered.

I sent a simple model (exported as step) to fabricators for flat sheet metal bending. When opening my model in SolidWorks, all sorts of errors are reported and they are not able to get a flat sheet from it. I tried to model it in several different ways:

  • extruding the profile curve into surface, then offsetting it 1mm to solid,
  • offsetting a 2 rail surface,
  • loffsetting a lofted surface,
    no success. I’m attaching a sample - stp file exported from Rhino. Any ideas?
    test_loft_sldw.stp (65.6 KB)

I think the problem here is that is made form a single surface instead of dividing it in flat and curve surfaces
you have the command _DivideAlongCreases with the option SplitAtTangents=yes

Hi Diego,

thanks for your input. I’ll try this option as well and send it to fabricators. I’m out of my whits though - because the fabricators said before, that the problem is, they get separate surfaces instead of solid one.

They need to be able to Join up the model in SolidWorks to be able to do anything with it, with the arcs and flats as separate surfaces in the solid to be able to unroll it.

My question would be why not just unroll it in Rhino? Unless there have been a ton of features added to SW in the last few years they’re not going to get a more precise result, to do that the model has to be rebuilt using Sheetmetal features(a comical thing to watch on an assembly of the slightest complexity, let me tell you, they’re not as nice to use as the normal modeling tools,) to be able to set the bending allowances.

It appears Rhino and SolidWorks are just not compatible - not for this sort of metal sheet bending, anyway. I got feedback from the fabricator and SW user who I sent test files to. It appears no matter how I model it or export it from Rhino, they can not use it. I’m most baffled that SW can interpret exported files I sent in such a different way. It does not even recognize arcs and straight surfaces.Thank you, Jim, for clarifying it for me with "not as nice to use as the normal modeling tools:)) - I’m sticking with Rhino anyhow and the community in this forum, which is awesome. Thanks!

Here’s a thought: I’m sure many working with Rhino came across that sort of compatibility problem with SW. Is it always such a hurdle? It’s mind boggling to think to have to rebuilt entire model due to such incomprehensible incompatibility issue. Would it not be possible to have a standardized format that would work across all 3d programs? I’m only guessing, but I would of thought that the input for simple geometry such as arcs, lines and geometric surfaces should be possible to standardize. I would of thought everyone might benefit.

@hereiam - I split up your object at tangents as described by @DiegoKrause and reexported as Step - SW seems to like it just fine, though I confess I do not know how to use the sheet metal bit at all… I used Feature Recognition on the way in and that seems to have made a valid SW tree.

Without feature recognition, Import Diagnostics heals some edges it doe not like

unroll.stp (128.5 KB)

I did notice the file tolerance is pretty large - I’m not sure how SW handles that. (.01 meters)


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For SolidWorks to be able to unroll a sheetmetal model it has to be built using parametric sheetmetal features. There are lots of things you CAN do with Rhino geometry in SolidWorks, sheetmetal is a particular, oddball specialized thing. You can’t even unroll a non-sheetmetal native SolidWorks model, nevermind an import.

If you model the mid-surface in Rhino you can unroll it there, and that will be good enough for many purposes. For higher precision needs I do that to get a quote and send 3D of the exact result I want and the fabricators have to figure out what to do to get it–which is a bit of a black art that can vary from machine to machine, so it’s not frankly the end of the world that they have to rebuild it, let the experts handle it.

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You can do this, but what I found to be working best is to do the conversion on a surface model rather than on the thickened part. SolidWorks is very picky about Surfaces being flat and fillets being tangent though. One of the flat surfaces in your file was not flat after splitting the tangents (also not marked planar in Rhino) and the attached 180 degree bend was not tangent to the adjacent surfaces. Attached is a SW model exported from the outer surface, then converted to sheet metal in SW
test_loft_sldw_repaired.zip (92.4 KB)

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btw: after repairing your surface in Rhino and offsetting in Rhino, it appears to be convertible to SW sheetmetal as well I just found:

test_loft_sldw_repaired2.zip (108.6 KB)

this is the Rhino file that I used to export it:
test_loft_sldw_repaired.3dm (736.6 KB)

I think too that this is something you need to take a look at. I believe SW normally uses 0.0001 as tolerance.

Thanks fro the files. I only opened the sldprt file in SolidWorks and this is what it shows. Is that how it’s suppose to look?

yes. SW normally has quite low quality mesh preview. Nothing wrong with the geometry itself. You can increase display quality in your document settings if you want

Fusion 360 has a sheet metal module that I imagine is pretty similar to the one in SW although I suspect it is much easier for a newbie to grasp (and afford!) I’ve managed to learn a bit using the Fusion sheetmetal tools and put some stuff out for bid to the fabricators and they have had no problem with the results. I do my initial design in Rhino and import it into Fusion and then just fold and flange away with their tools to wrap around my Rhino stand in so to speak. I’ve never been a big fan of AutoDesk but they got a lot right with Fusion in many ways. I sure wish I could copy/paste both ways between the two!

Here is a simple bracket from a much more complex assembly to give you an idea.

MTN 9T 3pc Tread BracketSolid .3dm (251.8 KB)

This was an more ambitious item exported back into Rhino after being developed and ‘flattened’ to a DXF for laser cutting in Fusion.

Mai Ta’i Nui 9 Tread Dimpled v10 Welded.3dm (2.0 MB)