What could be causing me to get chatter while adaptive clearing on my Shapeoko 3 happening always on the same spot in aluminum (Dots on the picture show where it happens. Same spot every time and more significant on the red side than on the orange)? It gets worse with higher DOC but doesn’t really seem to go away. Wondering if there’s an easy fix because I feel like it’s the main thing preventing me from speeding up roughing more. Everywhere else along the cutting path it is completely smooth. I haven’t had chatter problems with other toolpaths and the problem persists across a range of tool sizes and flute counts, with a variety of feeds, speeds, and depths. One problem I know that I haven’t been able to test yet is my surface speed is a little low (550-650 sfm) but I’m not confident going up to 800+ sfm could fix this rather weird issue. Any advice?
This pattern is where the Y axis is moving more. Since an SO3 check your v-wheels on x and y. Power off Shapeoko and wiggle side plates on sides of gantry. Slowly push gantry forward and back slowly and side to check for mechanical issues. Move project to another location to see if problem persists. Likely a mechanical problem. If it is a roughing pass does this happen on finishing pass?
I get the exact same thing on my SO3 (original). I get the same when profiling the outside of a part as well. I’ve tightened belts and v-wheels as much as I can, but yeah my wheels still are not as tight as I would like, I think adequate though. But I wasnt ready to take it down and file the holes yet. I do agree that there must be some “loosness” in the system some where. But it is a plastic v-wheel machine so that is a given.
And you are right that more SFM wont help…I’m up around 1500 and still get it.
(1/4" single flute, 24000 RPM, .003"IPT, .020" WOC, .200" DOC).
I would challenge that this is where the Y is moving more. Y would be moving more from 3:00 (or 9:00) to this position, and X would be moving more from this position to 12:00 (or 6:00). This position is where they are moving exactly the same velocity for a split second (and the farther out you go the longer this overlap is, hence more chatter). That sounds like a perfect opportunity to set up a resonance and amplify the “loosness” mentioned above for that split second. But why then not at 10:30 and 4:30 positions which have the same situation? I can only imagine cutting forces and tool rotation are the other variables that are at play here.
Sorry for the long post and not giving any solutions. I kind of gave up and accepted this as a limitation of the flexible SO3 design when forcing it to cut aluminum. My “bigger hammer” solution is prepping for a rail and ball screw upgrade.
Check for debris on the V wheels especially the Z. On my 4XL I get something similar if there is dust that has compacted on the rail or in the V wheels. It’s minor, but when the V wheels roll over the dust that has compacted, it ever so slightly lifts up in the Z axis and causes a small bump or ledge. On a circle I could see this happens once on each side as it rolls back over that same spot with a different Y location.
I know clean my rails with a stiff brush after each cut or project.
I’ve already tightened my v wheels but I could probably spend some time to get it more perfect. Yes this is a roughing pass, it doesn’t happen on my finishing pass which is just a contour that takes of the .005” radial stock to leave—not enough stress on the machine to cause any of this chatter. I should definitely try to go as far away from where I typically cut as possible to see if that helps. Is there any chance switching from climb to conventional milling could help? A random thought I had
My rails could definitely use a cleaning. Seems weird that it would be causing this exact issue, but I hope it is
Unfortunate to hear that it might not be an entirely fixable issue. Have you learned anything about how to maximize MRR while minimizing chatter? Your speeds and feeds are definitely much higher than mine—to a point where it feels like my shapeoko would explode if I tried those. Currently I’m using a 4mm single flute endmill.
My main thoughts on ways to cut fast with less chatter are:
-
Prioritize federate before increasing DOC or WOC. This seems to have much, much less of an effect on chatter.
-
Decrease DOC and increase WOC—this seems to generally work to minimize chatter, hopefully the same applies here
-
Switch to conventional milling? This one is pure speculation but i’d imagine it’ll change something, and maybe it’ll be for the better.
Cant say it may not be fixable. I just decided I didnt wanna go any farther and wanted to go rails/ballscrews anyway so this was my excuse 
No, I havent done any exhaustive MMR maximization. I just started winging it based on information from others here. Basic rule of thumb I heard was dont go less than .001" IPT, so I started there and kept moving up. I did not go till failure though and once I reached those numbers, I too thought like you that the machine was going to take off…so I just stopped there. I am not a production shop so not totally important for me. And since I’m way less than 50% of tool diameter on my WOC, that .003"IPT is artificially high due to chip thinning.
The way I approached it was to select a chip load I was comfortable with (or actually a little less) and let the CAM tell me the feedrate. then manually override the feedrate during the cut (same as your #1)
I’ve always been conservative with the WOC, and increased DOC till it started sounding ugly (basically opposite of your #2). Basically because I would rather use as much cutter length as I could. I kept trying to cut back due to the issue we are discussing but it never went away, so I decided to live with it for now.
I tried a full depth (0.5") slow conventional pass as a finish (.005") but didnt like the results. I always thought conventional was the way to go for finish, but I havent been able to nail down parameters to make it so.
with conventional the chips get thrown in front of the cutter and recutting becomes a problem. So I just stick with climb and slow down to 20-25 feedrate.
By the way my machine is just a slightly modified SO3:
HDZ
Saunders bed
10mm steel core belts
removed the C3D board and drive the stock steppers with Gecko 203V drives @60 volts
1.5kw air cooled spindle
running on Mach4
I use Autodesk Inventor for CAD/CAM (basically same as Fusion 360)
George,
When climb cutting, your cutter is trying to pull your machine along the direction of cut. When conventional milling, your machine is trying to push the cutter through the metal. Climb milling is the correct choice but you simply need to reduce your radial depth of cut. Take it down to 15-20% of the diameter of the the end mill. Axial depth of cut at about 50% of the cutter diameter. Now crank up the SFM and chip load per tooth. Because your radial depth is so shallow, you are in effect thinning the chip. The smaller your radial depth of cut, the faster your feed rate.
If you climb cut in aluminum, it will most likely gaul up. (build up on your cutter teeth) Carbide and aluminum do not like each other at all. It fact, most carbide end mills for aluminum are very high polished and very very sharp with special flute geometry. That said, use the newest, best end mill you have. Use cutting fluid to add lubricity and keep things cool. Tap Magic works great. Just squirt some in the path of your cutter during operation. Know the grade of aluminum you are cutting. 6061-T6 cuts great. 3003 is super gummy and cuts like crap.
I’m already using a radial DOC of around 15% and axial of around 50% (though I’ve tried 25% and the issue persists, just a little less substantial). I will see how a larger chip treats me though. I’ve been cutting 6061-T6 exclusively and tap magic has not helped this problem.
Keep going down on radial depth of cut and mild increase on feed rate. The machine is just a bit light duty. Try 10%
Pull the collet out and clean it as well as the inside of the spindle tapper. Could be some junk in there keeping you from getting a good seat.
Update: After doing some cleaning of my v wheels, rails, and the inside of the collet holder, the problem is (mostly) gone. Messing around with settings did not seem to remove the problem, but I am now running about 2.5x higher MRR with little chatter, which is good enough for me for now.
Yea. It always turns out to be something simple. Make the chips fly. Since the announcement of the SO5 and the SO4, pro and HDM have been out a while I wonder what the percent of SO3 machines are in the install base?
Like my truck I will drive it until the wheels fall off, get out and put them back on. I think the new machines are great but my SO3 is still working fine and does what I am interested in. I like the specs of the SO5 but as soon as I bought an SO5 the SO6 would come out. It is a zero sum game trying to be on the leading edge. For an existing machine the expense vs the output is not at a point I can justify that ROI. Plus I am cheap at heart. Should my SO3 disappear I would definitely want an SO5, but since I dont practice magic I dont think that machine is going to disappear anytime soon.
The good thing about the forum it is full of knowledgeable people that have helped many of its users from noobies to the most advanced users. Yea for US!!!
George,
As a side note, take a look at this post.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.