create 3D model from point cloud on Inventor

[christeen.salloum.1994]

Hello all,

 I am new to the 3D scanners, and we are getting one at work in order to scan the whole site and then the plan is to have the point clouds as one solid on Inventor and model the parts individually from there.

Now what is the best way to create a 3D model for each individual part from the point cloud that I have on Inventor?

in other words, is there a better way than creating points and planes on the point clouds? as I do not believe it will be accurate as I am loosing the quality of the point clouds the more that I zoom into the part in order to create points and planes to put my sketch on!

If there is anyone who can help me with this, will be much appreciated!

Thank You,

Christeen

[blandb]

This is the same struggles we are facing. We are not converting parts from point clouds, but we are laying in equipment based on point clouds. My boss was wanting to get solids of clouds as well and I have tried some different software's to get meshes, but all of them kind of looks like melted ice cream or dont give great results. So instead, I just place the point cloud into a part as a building reference file and viewing in Navisworks appears to give a better viewing result that viewing directly in INV. 

I to am very curious about better point cloud results. We cannot put these clouds into INV drawings, but they can be brought into ACAD drawings.

[romu51]

Hi,

@blandb @christeen.salloum.1994 

From personal experience I don't think Inventor is capable of without third party Add-In. 

Your best bet is to use the dedicated scanning software to initially create an STL or OBJ file format. These can be imported into Inventor for comparison.

You could then ideally convert then to solids but these create huge file size. 

I've been successful with Geomagic and Polyworks but unfortunately pricey! 

[Gabriel_Watson]

I went through this struggle about 5 years ago and took some notes, after consulting with a reseller and some other people at Autodesk. Here are my notes, if you wish to test this out too:


- Converting Point Cloud data into Inventor solids/surfaces: Open the RCS/RCP point data in Autodesk ReCap, and save it as PTS extension. Rename the file extension to ASC, and open it with MeshLab (free software). Pick "Filters > Remeshing... > Surface Reconstruction: Ball Pivoting" in MeshLab, and Apply a 0.1 world unit or smaller if possible. Export Mesh as OBJ extension. Open the OBJ file in Inventor and Convert to Base Feature the mesh features. Tips for big data sets:
Filters > Sampling > Poisson-disk Sampling
Filters > Point Set – Select Visible Points
Filters > Cleaning & Repairing > Remove Duplicate Vertices
Filters > Cleaning & Repairing > Remove Vertices wrt Quality
Filters > Remeshing Simplification and Reconstruction > Surface Reconstruction: Ball Pivoting (see settings above, experiment till you get the right settings for your worklflow)
"It is advisable to simplify large models by reducing the number of points (Filters > Sampling > Poisson-disk Sampling). First generate normals on the loaded model:
Render > Show vertex normals
Save the file (Export Mesh, .ply) with the option Normals and re-open it
Filters > Point Set > Compute normals for point sets
Consequently, it is possible to generate a 3D grid (mesh) model:
Filters > Point Set > Surface Reconstruction: Poisson
Remember to use the top command bar to switch to the 3D mesh model.
The resulting 3D model can be then saved to a DXF format that can be loaded into any standard 3D CAD application."

[christeen.salloum.1994]

Thank you for your reply@romu51

what are the Adds-In that we need if you know?

just so i can have an idea, and is it just for getting an STL file that i can open in Inventor as one solid or what is the process?

Thanks Again,

[romu51]

@christeen.salloum.1994 

Hi, 

i found this discussion which discusses the subject. 

https://www.laserscanningforum.com/forum/viewtopic.php?t=19559

[christeen.salloum.1994]

Thank You@rumo51,

I have checked the link and seems like they did not reach a proper solution!

So the posted  problem was exactly the same of my case, and some suggeste different 3D softwares (and that won't work in my case as we can't change Inventor at work), where others suggested few scan softwares which is similar to Recap I believe ( where you can crop and clean individual parts before exporting them to Inventor), but again that won't help in terms of  improving the 3D modeling environment in Inventor( I mean rather than creating inaccurate points and planes on the point clouds in order to create your sketch so you can remodel it)!

Am I missing anything there?

Thanks again,

Christeen 

[christeen.salloum.1994]

Thinking of what you just mentioned above, how about using the scanner software to crop the individual part that I want to model for example and export it to STL file where I can open it in Inventor as one solid but at least I have my planes and surfaces where I can remodel it-Not sure about the quality then?
do you think this might work for my case?
With thanks,
Christeen

[LT.Rusty]

This is something that I've been doing rather a lot over the past couple years, as we get more and more projects with the budget for 3D scanning.

First thing I do is cut the point cloud down to a manageable size with Recap. If I need to copy an asset out of the cloud, that means that I might use the limit box to block out everything except the exact bit that I need.

Then, with Inventor:

1- create new assembly to be your point cloud host.

2- insert the point cloud into the assembly at the origin location. Don't screw around with the origins in the file where you have the cloud. If you're just doing an individual part this may not be important, but if you're going to be putting a full scene together later with Navisworks and you've got stuff crossing 3-5 different software packages, you do NOT want to be trying to get origins sorted out. If the origin locations in every one of your files don't match up, you're not going to have a lot of fun in Navisworks.

3- when you insert the point cloud, turn the point density up as high as it will go. (Or as high as your video card will let you go. I've got a couple of point clouds that really put some stress even on my 4090.)

This is where the workflows diverge, depending on what you're doing. If you're modeling something that will be fitting into the scene, then create a subassembly (or part) and, again, keep it grounded to origin, and model your stuff in whatever orientation that happens to land in. This is the important file, the one that you'll insert into Navisworks later, because it contains your models but does not contain the point cloud. (Navis seems to throw an error for Inventor 2023 and earlier if I append a part or ass'y that contains a point cloud. Doesn't seem to happen with '24, but I haven't played with that enough yet to be sure if I can get away with it or not.)

You can create new ersatz-origin planes if necessary to represent floor or platform levels or north-south / east-west for aligning parts added to your assembly, and below this level it's okay to model as normal around the origin planes. It's just the top-level file that goes into Navisworks that must have the same origin and orientation as the ReCap file.

If you're just trying to model assets out of the real world that you will then re-use in any assembly, then you don't have to be as sticky about origins. I'll still generally put the scan in the host .IAM file at origin, but I'll usually locate the part file directly on top of (or right next to) the point cloud, and aligned with it, just to make sketches easier.

If you're having trouble picking out shells of the point cloud to use for lining up sketch geometry, use the BOX CROP tool (Manage tab, Point Cloud panel) to cut down to just a slice. That will usually do the trick- hiding irrelevant points cuts down on the clutter substantially.

There's more to it, but those are the important bits that I can think of right off. If you have some specific questions, though...?