So for the first time I’ve got myself some STL files from a 3D Scan, that I now need to turn in to a usable model that I can then make some modifications to.
I can import all my STLs in to SW fine and get some imported mesh bodies (with no errors).
First problem, all the parts are in wonky orientations relative to base planes which I’m finding makes thing difficult to mate them up in an assembly. Using the Move/Copy Body command isn’t working for me as I can’t use any of the mesh body geometry (element face or edge) to then mate to one of the base planes. Reading around, the Scan to 3D addin allows for body manipulation so, I fire that up and reimport my mesh. I now have an error in the tree with the error “The mesh has topological errors!”
Given that the software isn’t giving much useful guidance at this point, what are my options for resolving said topological errors?
I suspect this will be the first of several questions on this subject…
Thanks for the offer Mike! I’ll double check if I’m allowed to be sharing these models.
As for my original query, I’ve had some luck with the ScanTo3D Mesh Prep Wizard now which has done some sort of magic to remove the error from the tree so I might be able to cobble along for now.
I have an STL file sent to me. I want to perform a shell operation to hollow it out, or to even make extrude cuts, but am getting nowhere. I was hoping the ScanTo3D add-in would help, but I’m still not getting anywhere. Can any of you help? I’m using SWX2021.
Not allowed to share the files, but I was allowed to get the 30 day free trial of SE - so far it’s looking a better prospect for hacking about with these mesh files and I’ve already got them oriented how I want. Thanks for the pointer!
Thanks, JSculley, but I am really hoping to learn a technique within SWX (desktop Professional). Your model had many fewer surface segments, but they still keep me from achieving the desired result. If this was a native SWX part, or even a dumb solid with only a single face on the flat end and the other surfaces minimum in number I would be able to select the end face and shell the interior.
I thought that SWX, in the last couple of years, introduced some abilities to deal with STL files such as this. I tucked that nugget of info far into the back of my brain, where it gets mushed around with a lot of other things I might never use, because I had no use for it at the time. Now I’m not sure that’s something they did. I haven’t been finding anything in their help and I really don’t like wading around in their 3DSwamp to look for it either. That’s why I came here for help.
[mention]dave.laban[/mention] All mesh you get straight from a scan will have topology errors, it is better to clean and reposition it in other software before importing in SW.
For example, this is a bike stem I scanned this week, in Materialise Magics shows all errors of the mesh: [attachment=7]image.png[/attachment] [attachment=6]image.png[/attachment]
After cleaning up in PolyWorks Modeler Light and Magics: [attachment=5]image.png[/attachment] [attachment=4]image.png[/attachment]
In Rhino there is the QuadRemesh that can convert the STL mesh to SubD and later to NURBS [attachment=3]image.png[/attachment]
After that it is easier to work with a step file (NURBS) in SW, the Intersection Curve and Silhouette Entities will provide better results. Also SW wont be so slow, since it cannot handle STL files very well [attachment=2]image.png[/attachment]
[mention]DennisD[/mention] file after converting in Rhino
[attachment=8]image.png[/attachment]
[attachment=1]image.png[/attachment]
[attachment=0]image.png[/attachment]
I just used the QuadRemesh feature, there is a longer workflow in Rhino: creating guide curves and rebuild the NURBS to get fewer faces.
Most popular software to deal with Reverse Engineering are Geomagic Design X and PolyWorks Modeler, but they cost around 20,000 USD. Faro RevEng is about half the price, I might get a trial next year…
I made a topic about RE in the SubD and Mesh subforum, if you are interested:
Convert to Mesh Body (sometimes the tools won’t work without this)
Slicing (great to get many profiles fast)
Sketch tools:
Intersect Curve (for profile)
Silhouette Entities (for profile)
Spline on Surface (comes in hand when you need BRep for surfacing)
Fit Spline (For fast resketch or complex geometry)
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I took this door handle as an exercise today, here are the results I got for now:
Used Slicing and Intersect Curve to get the profiles
Renamed the Sketches I wanted with numbers; used Fit Spline and deleted the original lines from Slicing.
Made some Guide Splines as Guide Curves
Divided the solid in many parts, because it was slow and failing to build
Could not finish the tip, SW was building it in a bad way, probably due to the Fit Spline change
The Body Comparison from it:
image.png
Results: The amount of points used in Fit Spline was giving bad results; increasing deviation, computational time, and reduction of the user’s patience
Conclusion: It is better to use Slicing to get the measurements and draw everything else. Also, the file will became slow if many profiles are created due to the amount of points from the mesh.
OBS: Lots of bugs and geometry loosing relations, used the Freeze Bar to stop that. *****************************************************************************************************************
Using Rhino QuadRemesh:
I tried many configurations and also Guide Curves. In the end, just the regular settings were enough to get a solid build from 10 surfaces. (rebuilding the cap will be just 6)
The Body Comparison in SolidWorks:
image.png
Results: Got a NURBS solid from mesh with high precision
Conclusion: With few surfaces the quality of the Intersection Curve is much better. It is easier to rebuild the solid in SW, or use the Step file fast.
Get Rhino, it’s cheaper than any SW add-in **********************************************************************************************
Critics and suggestions are welcome, I am trying to get better at RE From SW.SLDPRT (6.89 MB) From Rhino.SLDPRT (2.36 MB)
Reposition the part (automatic, using reference and numerically)
Delete mesh faces
Mesh enhancement (Triangle reduction and Smoothness)
Starts Surface Wizard
Mesh Edit
It is Move/Copy Bodies feature, plus scale and offset
Surface Wizard
Automatic and Guided NURBS creation
Automatic: Allow to select Surface Detail and Edit the feature lines (has some glitches but can fix bad geometry)
Guided: Allow to select a symmetry plane and extract surfaces semi-automatically, but it is difficult to set the boundaries. I just got bad results.
Curve Wizard
Failed to select the mesh, so whatever
Deviation Analysis
Need to reopen the STL file and import the solid generated to work. lol
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Tried to Shell the door handle using the Automatic (generated with Min, Max and Intermediate details): Failed
image.png
Importing a Scanned Mesh I got the same topology error, but was able to create surfaces from it automatically. (some intersecting/overlapping triangles are not a big deal to print)
The quality from the NURBS solid was bad tho.
Minimum Detail: 2245 surfaces
Maximum Detail: 37189 surfaces (so slooow)
Rhino: 469 surfaces (and repaired the crappy boundaries)
ScanTo3D for Reverse Engineering:
For Meshes created by CAD (door handle) it works OK or Bad, depending on what you want to do.
For Scanned Meshes the amount of surfaces generated is too high, it is easier to work with mesh data.
This handle is being done by high school students. It is an interior door handle for a B-17 restoration project. There are no markings on the part to indicate make/model and there are no detailed drawings on it so they are using calipers and their modeling skills. They chose to do this originally in Rhino because they could not figure out how to do it in SWX. I don’t have Rhino, nor do I want to use it so I asked for something in SWX.
They initially sent me an STL and I just couldn’t do anything with it. I asked for a dumb solid from Rhino and got a Parasolid. They had added a few features and now I really needed to work on it because, well, the changes weren’t good.
image.png
At least I could cut away the non-blended and non-round barrel they had added and make it match the original different non-round barrel. Really?!
I was also trying to hollow this out somewhat, to a wall thickness of approximately .150". This was going to be printed in a resin printer so it needed to be hollowed out a bit, but the slicer program was leaving artifact tessellated holes using the STL version. Shelling the Parasolid in SWX was failing when I used anything close to .15" so I had to resort to creating a lofted cut. But I got it!
The printed part matches very nicely with the original so now we have a model we can use to make replications.
I would like to see better native abilities in SWX to deal with STL files and was really hoping you all had the answers. Thanks for all your efforts!!
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