brep vs imported mesh for milling smoothness

[calexpavel]

I was doing some tests to see if the geometry created in Fusion is smoother when milling, than the one imported. So i created a sphere in fusion and i imported one from another software which has 65024 triangles. 

In the cam workspace they look identical. You can see the polygons on both of them:

but in the render workspace the sphere created in fusion is much smoother: 

So my question is: Would the sphere created in fusion be smoother if i mill it on my cnc? Why does it look smoother  in the render workspace? Is it just a smoothness effect in this workspace, but when i actually want to mill it it would be faceted like the imported mesh?

I want to know if i should model my geometry in fusion, or another software. Is there any advantage to create the geometry in fusion in regards to milling it on your cnc?

Thanks!

[HughesTooling]

CAD systems use a render mesh for display so your import might look the same but that is only the display mesh. If you right click a Brep body in the browser (the body not the bodies folder) there's an option Display Detail Control that lets you adjust how fine that body's meshed. Added to this some smoothing is also done by the graphics card so a mesh can appear a lot smoother than it is or how it will machine. In the past I used Rhino3d and MadCAM, MadCAM used the render mesh to generate the toolpath from and the standard smoothed display would catch people out. Rhino has an option for Flat Shade that turned all display smoothing off so you could actually see what you get from the CAM.

In Fusion the mesh is calculated for each op based off the tolerance, you also have a smoothing tolerance used to fit arcs to the toolpath. You might find your imported mesh will be less facet if you enable smoothing in the op. Normally a smoothing tolerance 2X the tolerance works well but as the mesh is imported the meshing tolerance is not know so you'll need to experiment.

As for machining native Breps, try a tolerance of 0.01m and smoothing of 0.02m on larger part and 0.005m and 0.01mm on smaller parts, the 2 tolerances need to be added to give the total tolerance. Smoothing only works well for 3d contour and parallel. So yes a native part will give a better finish as you have the option to set how fine it is meshed.

Mark

[HughesTooling · Accepted solution]

---

@calexpavel wrote:

I want to know if i should model my geometry in fusion, or another software. Is there any advantage to create the geometry in fusion in regards to milling it on your cnc?

Thanks!

---

If you model in other software you'll get the same quality as long as you use a file type that support surfaces, STP, IGES etc. Meshes might be OK if they're meshed fine enough, just might be trouble to work with in general making assemblies and positioning in Fusion, picking datums etc.

Mark

[calexpavel]

Thanks! Lots of things i didn't know. I didn't know about iges and stp that it can export the surface and fusion imports it as brep. I'll do some tests in cam now to see how smooth it is after milling and i'll also try your smoothness advice in cam. Cheers!

[bshinos]

Please let us know what you find out.  I have been machining meshes for a while now, and I would like to find a way to keep my machine from shaking (violently) when cutting mesh surfaces.  

It would be nice if there was a way to interpolate mesh surfaces to reduce points and create smoother cutting profiles.

[HughesTooling]

@bshinos  What toolpaths are you using? Smoothing only reliably works on 3d contour and parallel, have you tried these with smoothing enabled? Have you got any designs you can share, if you can export as an f3d and attach. Also what control are you using, does it have any settings for constant velocity machining?

Mark

[calexpavel]

Well i exported my geometry as step format and it is very smooth in cam in fusion. I don't get that surface where you could see the triangles as when i was importing it as stl or obj. Fusion sees the geometry as brep when i import it as step format and i could even bevel the surface perfectly.

[bshinos]

I am using contour and parallel.  My workflow includes 3d scanning (einscan pro), meshmixer to clean and reduce mesh (20k faces) and export as STL.  Import into fusion, mesh to brep convert.  Modify and trim mesh body.

Manufacture:  Adaptive 3d for roughing with 1/2" flat. 

  Contour: Tolerance 0.05mm, Smoothing 0.01mm.  Minimum diameter 1mm, minimum cutting radius 1mm.  Climb, .5mm stepdown.

   Parallel, same settings as contour.

Machine: Home-brew CNC machine with Grbl running on a Raspberry pi Protoneer.

It seems when the contour runs into the mesh it jumps from point to point, pretty agressively.  I don't need the final surface to match the rough mesh.

[HughesTooling]

@bshinos  Have you got a model you can share? The tolerances you're using are not the best, I'd try tolerance of 0.02 and smoothing 0.03 maybe even 0.01mm and 0.04. Never tried on a mesh to brep model though so not sure how\if the smoothing will work.

Smoothing works best if it's 2 or 3 times the tolerance so 0.04 and 0.08 might work better if you don't mind losing some accuracy. 

Mark

[bshinos]

@HughesTooling Thanks for the quick reply and great information.  I have one roughing on the mill right now, I'll try to adjust the tolerance/smoothing.  The reason I have the tolerance at 0.05 is because my processor chokes if I set it any lower (raspberry pi can only process so much I guess).  I'll try my smoothing at .09 and see what that does.  I'm also PMing you a file.  Thanks again.

[HughesTooling]

I've looked at your file from the link you PMed me. The setup looked odd as the stock was in at the wrong height and it only had an adaptive toolpath so a bit difficult to advise. I've setup a couple of toolpaths and arc fitting seems to be working in both. For your part you'd want to use parallel for finishing. Does your post and control handle arcs in the XZ and YZ plane.

I'll PM a link to the file. I set the tolerance to 0.05 and .1 as the part is quite big. For roughing with adaptive I use 0.1 and 0.2 as the total tolerance of 0.3 would still be less than your stock to leave.

Mark

[bshinos]

@HughesTooling Thanks again for the feedback.  I set my tolerance and smoothing as you suggested and the cut was buttery smooth.

  I did the smoothing on the adaptive rough as well, and it seems to have caused some other weird issues; pausing (hold) and stuttering that I did not see when I didn't apply smoothing.  I'll try to go back to my previous settings on this for my second piece and update the forum with my findings.