I’m having an issue related to my CNC that’s very odd.
It’s not likely related to RhinoCAD as that just produces the model but more likely related to RhinoCAM and settings on my CNC. What it is I get very tiny, very shallow ridges when CNCing when doing a parallel pass on the X axis. These build as the machine is moving along deeper along the Y axis. I know it’s hard to explain by description so I’ll upload a sample photo. In the picture the grain in this case is more or less along the X axis. The faint ridges are running front to back on in the image on the Y axis. And, here’s the real strange part: they only appear along on side of these wave forms. To me it looks like they’re kind of burnished in by the climb cut the tool makes in one direction. I’ve discussed this with McNeel and Mecsoft and the CNC builder and they can’t see where theres and issue. If anyone has any suggestions on how to track this down, do let me know.
Tim,
This may not be it but… Sounds suspiciously like your spindle is not perfectly true to the bed.
Mount a trammel in the chuck and check the spindle alignment.
I don’t use RhinoCAM, but rather madCAM. However, I think your issue relates to your mesh setting when you are generating toolpaths. madCAM actually tessellates the model based on the display mesh. So, more dense display mesh yields smaller line segments, yields smoother cuts. I had issues identical to this, and that’s how I fixed them. Are you able to see your gcode visually in Rhino? I always turn on the points for my toolpaths, and then I can see if I will have issues like this. Hope that helps!
Steve, I’m pretty sure my spindle is true to my bed. In fact I just ran some accuracy tests today along with the CNC’s builder including a 3/4/5 test for square to make sure the encoders were doing their job and keeping things square and all seems well.
Sky, What you say does make some sense and I’ll looking into my settings in RhinoCAM to see if anything shows up. Might have something set wrong. Good tip. One question back at you, though. You mentioned that you saw the same kind of issues. Did you see it only on one side like in the photo? I know that this example is wood and I figure whatever is happening is likely on the climb cut in one of the directions, it might be burnishing the wood and that might account for it. Your thoughts?
In this example the cut path is actually going along with the grain (left to right, right to left). It doesn’t matter which way the wood is positioned. Or the kind of wood, though harder woods show the ridges more.
Your description and picture doesn’t make it very clear what you are talking about, but my guess is you are talking about what are called scallops. If you don’t know what the term “scallop” means, maybe this page will help. http://www.cnccookbook.com/CCCNCMillFeedsSpeedsStepover.htm
Sorry, Jim. I don’t have the correct language down and so was using the wrong term. Scallops would then be artifacts from how stepovers are setup then. In this case that doesn’t apply. So, let me start over for maybe a better description. Looking at the photo, the tool is moving horizontally along the Z axis. The deep waveforms are being created as a result of the tool paths. From the front of the photo to the back is the tool works its way away toward the path. In this photo’s example, the step over was just 4%. These very subtle ridges are the faint ones you see on your right that are perpendicular to the direction to the wood grain. It’s those very subtle artifacts that I’m having trouble with. Too much sanding. And, as you get more and more detailed in the output that sanding is no fun at all. The question is how come those artifacts are being formed? And, why only on one side of the wave forms?
Are you using a raster type toolpath and are you cutting in both directions. If there is any defection in your spindle it will show a lot more if you are cutting in both directions. I don’t know about working with wood but with metals you get a better finish with climb milling only.
Sorry about my limited knowledge about this, but I’m not clear about “raster type toolpath”. I’m using RhinoCAM. Is there a setting in there for this? In terms of climb cuts on wood because the tool is moving back and forth in parallel passes, one direction is climb cut the other isn’t. If I was to set the parameters to a climb cut, I’m sure the passes would just be reversed and I would think the results would be the same. Deflection. Might be possible. Hadn’t really thought about that. In this case it’s only a .250 ball mill.
To me anyway, the results almost look like there’s little microsecond pauses as the tool moves along its path. With those extra microseconds the tool is kind of burnishing the wood during the climb cut. As to what’s causing it, I really don’t know.
Tim, Raster means the tool path is in a straight line parallel to the X or Y axis Your photo appears to show “waterline” toolpaths, where they follow the contour of the object.
Cutting in both directions is referred to as bidirectional, and usually the machining app will give you the choice of bidirectional or single direction.
It sounds like you are using mixed for cut direction. You might want to experiment with Climb or Conventional, when you use one of these it will mill across the part in only one direction then rapid to the clearance height and rapid back to the side the first cut started from so only cutting one way. I guess you’re using Parallel finishing by the way.
And, the advice to run in a single direction and then rapid back to the beginning would likely end up in a smooth result. I’ll have to give it a try, both climbing and regular to see if the problem goes away. The only issue for me is the added time to cut. Some pieces I’m done have taken 27 hours to mill. Going in one direction only certainly would add to the time.
i do some 3 dimensional carving of figured hardwoods, and often choose climb only for a better finish. takes longer unless you part lends itself to a spiral path.
another long shot is if your toolpath is defined as many very small line segments, your control may have trouble keeping up. i know i had this problem years ago but assume controls are much faster now. we cut wood at such faster rates than metal that my metal cutting machine was not expected to need to go 200ipm. slowing the feedrate down would tell you if this is the case.
Tim,
I have these often. As far as I know it has to do with the meshing in Rhino. Since RhinoCam uses the mesh to create the toolpath, it must break the path into straight segments that move across the surface of each polygon. In your example, the “ridges” occur when the curvature changes and the settings on your controller tell it to stop the machine’s motion then restart in the next slightly different direction. So this momentary stopand start creates vibration that causes a bit of a ridge. (I believe that these settings can be changed per machine). With a finer mesh this can be alleviated to some extent since the direction change isn’t as great.
You can test this by making a surface that gradually changes from gentle corrugations to larger ones. At a certain point the controller will decide that the change in direction is too great to do without slowing to a stop and re-accelerating.
Nick
This sounds right to me. How do I control the mesh created in Rhino is so that RhinoCAM will be working at a finer detail and hopefully eliminating those ridges?
There is a limit to how much you can prevent this. If you can find out at what point your controller decides that the angle is too acute to move smoothly from one line segment to the next, then you can try to make a mesh that keeps the adjacent poly’s within those parameters.
Setting mesh parameters in rhino is an art and science unto itself, generally the finer the mesh the smoother the transitions. But edge legth and other parameters come into play. Maybe some Rhino gurus who do machining can help? @Helvetosaur?
I think you should expect that that you will always need to do some clean-up with RhinoCam on a topography like you show. Some of the very expensive toolpath software breaks NURBS surfaces down to very minute facets which give an essentially smooth product. Also since you have allowed for large scallops it seems like you expect to do some clean-up.
Nick
Great advice, Nick. Much appreciated. I figured that there would be no perfect way to do this, but I’ll work on improving the mesh issue to see if I can at least improve it quite a bit. There’s plenty of incentive as I expect to do some fairly ambitious topography for my carvings. The folks at Rhino and Mecsoft are looking at this now, as well. Maybe they’ll have some suggestions, too.
Here’s a post I did on my blog about the same issue I had with madCAM:
As I said before, I think that even though you are using different software, I think that the problem is the same. When you take a NURBS surface and generate a g-code over it, since in theory that surface could have an infinite number of points, it has to be meshed somehow. madCAM, and I believe RhinoCAM too, utilize the fact that a mesh of the object already exists, in the form of the display mesh. I’ve created some presets that I use when I generate toolpaths, they just have much more dense mesh settings. Modify the display mesh settings (in Properties), and you modify the way the toolpath is generated. FWIW I tend not to do any hand finishing on the molds I make, and they are almost always freeform NURBS surfaces. madCAM is a ~$750 piece of software, so you don’t need some crazy high end software to make it work, just some trial an error.
One thing to note is that you can overdo it - if you set it too dense, then you will overwhelm your CNC controller with input. It’s a balancing act that is unique to every machine and the type of work you want to do.
I would say for starters, see if you can turn on the points of your toolpaths in Rhino the way I have done on my blog post. See if you are getting areas where the breaks in the toolpath all lines up.
