CNC Circle-Cutting Accuracy in Solid Wood
CNC pros help troubleshoot when a CNC router cuts circles that look more like ellipses. August 21, 2006
I cut a 1.5" D circle .74" deep in solid oak with a .375" DC in one pass at 60 IPM. The result was sad - looked more like an oval. I assume the result was an oval because the greater resistance to cut cross grain, causing greater tool deflection. Since I know the material didn't move and the machine I was cutting with weighs 12,000 pounds, I can only conclude that tool deflection was the cause. With .06" deflection I'm surprised the tool didn't break.
I've never experienced noticeable tool deflection before. I've also never cut solid wood this way before. I assume a larger tool diameter and/or multi passes must be used to result an accurate cut. Can someone recommend a tool diameter and rule of thumb to follow?
From contributor A:
All materials are different. The best rule of thumb I can tell you for wood products is to do a test run first and if there are problems, troubleshoot them. With your particular problem, try to do the hole in more than one pass. It also depends on the type of bit you use. I do not know the program you are using or the router. With the one that we use I would have cut my hole in two passes leaving a very small amount of material and then would have done a final cleaning pass, and I would have used a down spiral 0.25 bit at 40ipm to do the first rough operation and a 0.375 straight bit at 60ipm for the final operation. Just keep in mind all machines and programs are different.
From contributor B:
My observations from cutting holes and round pocketing - the size of the hole and the speed feed have a direct correlation. The smaller the radius the slower the speed feed. Try slowing your speed down - for 1.5 diameter try 50ipm. Keep in mind when you decrease your speed, you need to decrease your RPMs.
From contributor C:
I would increase the cutter diameter to .75, 3/4" or more. In doing this, the spindle RPM will drop somewhat to account for the different surface footage. If you were running 18,000rpm with the 1/2" bit, a comparable 3/4" bit will run 14-16,000 (consult your tooling manufacturer). Your feed will drop proportionately also. Insure your tool is loaded in the holder to maximize rigidity. You can also change your machining strategy. If you are plunging in vertically off the finished tool path, then feeding to it, try instead to helically feed in on the path with a final cleanup at the bottom.
From contributor D:
Is there any way to stick a pen/pencil in the spindle and draw the toolpath on something to eliminate a software problem? Then check it with a circle template. How often have you cut circles?
From the original questioner:
The machine is a Stratos SUP with about 50 hours on it, the software is MV. I don't cut circles very often, but when I do they’re larger than 18" diameter and in plywood or MDF, they turn out fine. I was experimenting with an idea for custom stile and rail joints for solid doors, involving round pockets in the stile and a round cutout at the end of the rails. In a test I did with MDF the test went well, the joint fit correctly. When I have time I'll do more testing on solid with the advice mentioned. Thanks for the input. I like that pen idea. I was thinking about having the router detail parts using a sharpie. At the beginning of every program I'd set it up so the first operation was to take the cap off, sliding it sideways into an apparatus that put pressure on the cap, then come straight up out of the cap. The opposite would happen at the end of every program. This sure would save time detailing parts as they come off the machine. A series of dots left by the sharpie would tell the banding detail. Since all our cabinets use a locking blind dado, placing the dots there would be hidden after assembly. I wonder if this would be better than forking out 7K for a touch screen and industrial printer setup to run part labeling. Has anyone ever heard of doing this?
From contributor F:
Always use the biggest cutter available. I cut a lot of solid wood and when cutting 1.80" or 2.30" thick I will usually make the first cut .030" big in .500" passes, then make one cleanup pass to remove the last .030". This has worked very well for me on a Biesse Rover 24.
From contributor G:
If this was a solid carbide tool, it should have broken with this much deflection. When you are doing an interpolating machining action, your software is trying to read ahead of the cut, knowing when to slow down. As has been suggested, slow down your feed speeds and RPMs and use a larger diameter tool.
From contributor H:
This sounds more like a calibration issue between the X and Y axes than tool deflection. If you program a line on a 45° angle, is it perfectly straight or does it appear to be an arc? If it's an arc, this supports the calibration issue. Someone more familiar with your machine should chime in.
From contributor I:
60ipm is really slow. With my MV you can use a helical ramp-in. We used to have an Andi and it was very solid. Use the shortest tool you can with the shank set into the collet the full depth of the collet. It is hard for me to believe you could have enough tool deflection to be noticeable without breaking it.
From contributor J:
I suspect that your oval circles have less to do with the difference in crossgrain or grain resistance and more to do with how your control is set up. I do not know what kind of control you have, but servo gain and acceleration/deceleration time constants need to match for X and Y. Even with that, there is always a following error in a driven axis which means that the faster you go, the smaller the circle will be.
Try cutting the same circle at the same feed rate very shallow in MDF or particle board. If you get similar distortion, you can rule out tool deflection. If you have a high speed/high precision option (G8P1 maybe), turn it on and see if that helps.
From contributor K:
I have to agree. Eliminate the possibility of machine or code error before getting too wrapped up around tool deflection. If the test produces a round hole, then confirm that your part is not moving, and lastly, check that the spindle is not deflecting.