Importing Complex Contours/Surfaces

[strugglebus_mechanic]

Hello, I'm using Inventor 2025, attempting to import a model that was exported from Rhino. This is a model of a wall that I'm attempting to slice up to create individual slats. The end goal is a "dimensional wood slat wall". I've been using Inventor for years but am now realizing my knowledge of importing and surfaces is lacking.

I've been learning some nuances about surface tools - stitching, patching, and trimming - but after stitching  cannot manipulate the solid in any way. I can't select a surface to extrude, thicken, or remove.

Thank you for your help, I've been on the forum, youtube, and chatgpt for a while now and can' seem to find the fix.

[EvellinDichev]

I am not sure is it going to be the perfect solution for you, but once you make it solid, try to  export it once again in stp, and then open it and work on it.
I had done it  tons of time, and it always worked out perfectly.
Probably not the best solutions, but it works 😄

[johnsonshiue]

Hi! Please share your attempt (ipt). It will be easier to see where the problem is and propose a better workflow.

Many thanks!

[strugglebus_mechanic]

Attached! Thanks.

[strugglebus_mechanic]

It's a solid idea but I still can't modify it's geometry after "re-importing". I can use it to set a plane and I can project its geometry to a sketch but it fails to actually build on it or cut into it.

[johnsonshiue]

Hi! Many thanks for sharing the file! The issue with the model is that the surface has only one face. But the geometry is extremely complicated. I don't think there is any command in Inventor that can edit this import surface. I suspect you can split the surface into multiple pieces. That is probably the most you can do.

Thanks again!

[SBix26 · Accepted solution]

I think there's something wrong with the geometry.  I was actually able to place a Hole feature, even with a countersink, but calculating it took several minutes. 

Inventor could not split the body using the XY plane, but I was able to create a 3D sketch and create two intersection curves, one on the top face and one on the bottom using the XY plane.  The interesting thing I found was that the two curves crossed each other, so this geometry is definitely not right.

Update: I managed to separate the two faces by using Copy Object to Surfaces, then deleted the top face (the one with minimal contour) as well as the repaired composite.  I then created a workplane close to the surface and extruded the outline To Next, making it a solid body, sort of like a large carved sheet of plywood.  This is now editable using all the normal tools, so I set about splitting it into planks using a pattern of workplanes (see below).

The attached file is Inventor 2025 format.

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Sam B

Inventor Pro 2025.1.2 | Windows 11 Home 23H2

[johnsonshiue]

Hi! Another workflow to consider is to convert it to Freeform. Go to Freeform panel -> Convert -> pick the face -> set the precision to 0.01in for each direction.

The resultant Freeform surface could be very complicated. But you may be able to tweak it.

Many thanks!

[EvellinDichev]

Can you send it to me as a step file, I will try to fix it :).
I have couple of ideas to test on.

[strugglebus_mechanic]

Impressive! I recombined the bodies and slatted the feature as planned. Updated model attached.

I still don't understand how you separated the two faces. That interfering geometry was stopping me from trying any of my usual tricks.

Also kind of crazy, after slatting the feature, the exported .stp file ballooned out to 756 MB! So that's why only an .ipt is attached.

[strugglebus_mechanic]

much appreciated! .stp in the original post, thanks!

[strugglebus_mechanic]

thank you for your time and effort!

[SBix26]

Knowing what I know now about the file, here is how I would do it when opening the .stp file originally:

Choosing Individual surfaces instead of Composite I do not get two interfering surfaces, I only get one surface:

This eliminates the problem, allowing manipulation of the surface or conversion to a solid by thickening or extruding To Next.  I don't know why the Composite option creates two surfaces and Individual creates only one.  Perhaps Inventor's conversion tool is a little buggy?

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Sam B

Inventor Pro 2025.1.2 | Windows 11 Home 23H2

[strugglebus_mechanic]

works perfectly! I circled back with the original model creator and showed him the conflicting geometry. He was able to remove the interfering surfaces before exporting, which saved me that step and helped him learn too.

thanks again!

[mgrenier1]

I'm having a similar issue when importing dwg or dxf file of more artistic stuff(vectorized jpeg images of animals or other stuff like that are a great example). The file will take hours to import and every following operations takes forever to complete.

It's been like this since I started using Inventor back in 2017 and has been an issue with every new version every year.

Is there a way to optimize the dwg or dxf file for that kind of stuff So Inventor doesn't want to die every time I import one?? (I have not really noticed any differences timewise between using splines or polylines)