Derive Hole Locations From Mesh Scan (no thickness)

[Anonymous]

I am working with a scan file of the interior of a cargo van, and am trying to reverse engineer the hole positions to a datum (to then design fixtures that mount to the holes). The scan is essentially a surface, and is therefore infinitely thin. Because of this, I cannot create a "mesh section sketch" at a single plane that intersects all of the holes. Each hole is on a slightly different plane due to the resolution of the scanner.

What would be the best way to derive the hole locations from a scan file like the one I have attached?

Thanks for the help!

[TheCADWhisperer]

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@Anonymous wrote:

What would be the best way to derive the hole locations from a scan file like the one I have attached?

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Eyeballing and logic (designer is likely to use standard drill sizes and put holes in a straight line at logical distances, 100mm rather than 100.0123mm).  And if you have access to actual part - caliper measurements.

If you then find that you are off a bit - because you have used a parametric modeler - editing is easy.

[MRWakefield · Accepted solution]

Is this roughly what you're looking for? Here's what I did:

1. Import mesh & move to a convenient place nearer the origin (you might want to position and orientate it in a way that makes most sense)
2. Edit mesh & reduce face count in the unimportant areas (I probably could have just deleted the parts of the mesh that we're not interested in)
3. Insert a 'Base feature' (I could have just turned off design history instead)
4. Perform a Mesh to BRep
5. Finish the Base feature
6. Start a new sketch on the appropriate plane
7. Project the BRep surface body to the sketch
8. Draw 3-point circles using projected points. This will enable you to get approximate sizes and positions of your holes.

Model attached.

Hope this helps

[Anonymous]

Marcus - really appreciate you working this out! That is exactly what I am looking for.

[MRWakefield]

No problem, you're welcome. After I posted I also tried reducing the entire mesh (rather than selecting the parts of it) and selected 'Preserve Boundaries' and this worked just fine too.

[Anonymous]

Good to know, quick point of clarification - is the "base feature" you mentioned in Step 3 just a dummy feature with no geometry? And don't you nee to turn off "capture design feature history" between steps 1 & 2 in order to reduce and edit the mesh?

Also, do you know why Fusion 360 is not recognizing the selected faces? See screenshot.

[MRWakefield]

The base feature enables you to do things that you'd only normally be able to do when history is turned off. Effectively it temporarily turns off history so you can do things like reduce the mesh, when you exit 'Base Feature' you're back to normal (history intact). The alternative is to turn off design history but of course you then lose any history you might want to keep.

No, I don't know why that's showing as 0 faces selected 🤔

[Anonymous]

Got it, thanks! I restart Fusion and faces can are now registering. #solved