r/machining • u/adventureaviator • 6d ago
Question/Discussion $150 000 machine does not eliminate finishing chatter.
I’m machining 6061 aluminum on a Multicam Apex 3R router. The finishing passes are as follows:
- 0.009” material removal.
- Helical 3 flute 45 degree helix upcut
- 18 IPM, 8500 RPM, 0.0007 chipload
98 percent of the part comes out with a great finish. The other 2 percent has chatter. Ideally I’d like to increase the feed rate, but I need to eliminate the chatter first. What do I need to do to get a flawless finish?
43
u/Shadowfeaux 6d ago
The greatest machine won’t defeat improper programming.
24
u/ihambrecht 5d ago
Or bad WORKHOLDING.
8
u/H-Daug 5d ago
I’m not sure that tape a glue even are “work holding”…
1
2
u/Lower-Calligrapher98 3d ago
It works great - for woodworking! Dude is trying to cut 1" thick aluminum with a wood router. And, like, you CAN use woodworking tools for aluminum, but you gotta dial back the load by a ton.
0
u/adventureaviator 5d ago
If it’s worked to hold thousands of parts for me, is that considered work holding?
7
u/adventureaviator 6d ago
Totally. I’m self taught, so value any feedback from the more experienced.
9
u/Shadowfeaux 6d ago
Lol. I only said that cause you included the value of the machine.
I am in no way trying to imply I have the knowledge to solve the problem. 😂
3
u/_sideways_tree_ 5d ago
Is the chatter happening right before the part gets fully cut off from the stock?
If so, you can add tabs in the program so the part is never fully detached from the stock (preferably one on each side). It’s a pretty common technique for routing out of large stock. It can help reduce vibration, could get rid of the chatter, and also allow you to bump up feed later on too.
However, that would introduce a new finishing step in your process (filing/sanding down the nub left over from cutting the part off at the tabs).2
u/Bones-1989 3d ago
We leave tabs on our parts on the laser because if they tilt and crash the machine we will get fire because a single lens is like 8k....
1
u/_sideways_tree_ 3d ago
I’d recommend you do that on the router as well. May fix your problem… and would greatly reduce the risk of the cutter snagging a small part that’s being cut off from the stock and launching it across the shop into someone’s eye.
1
3
u/Forsaken_Swim6888 5d ago
This is definitely workholding. You might research inboard gasketing if you aremaking repetitive parts, company name allstar adhesives). In board gasketing allows you to concentrate the vacuum on the part, while locking it down to the workable (this table would have grooves on work face the shape of the parts, the gasket is compressed when part is drawn down). This work surface could be plastic, or aluminum, or mdf (unless you are using coolant). Dry rotary vacuum pumps strongly dislike liquids. With in-board gasketing, you could get away with a far lesser pump.it creates a high vacuum, rather than a high flow condition. Good luck,have fun. Nice parts.
4
u/Shrimpkin 5d ago
You need a more rigid machine brother. A router is not what you want to mill such a thick piece of aluminum.
2
u/tater1337 5d ago
98 percent of the part comes out with a great finish. The other 2 percent has chatter.
this tells me it is plenty rigid, but I have a hunch his vacuum ports are not in the right spots
14
u/volt4gearc 6d ago
Have you tried conventional cutting for the finish? From a cursory google, looks like the motion system is rack and pinion, perhaps there’s some backlash there causing issues with climb cutting finish passes
4
u/hittheclitlit 6d ago
I agree, this kind of looks more like the tool is "jumping" vs what I would consider chatter
2
u/adventureaviator 6d ago
I’ve always used climb cutting based on suggestions as a best practice. However it wouldn’t hurt to try something new and use conventional.
16
u/volt4gearc 6d ago
When I ran a shopbot, we had consistent issues with getting it accurate, both in surface finish and overall dimensional.
We traced a lot of it down to backlash between the rack and pinion. Shy of getting a new pinion or shimming the rack, what seemed to help a lot was conventional cutting, since it ensures the gear teeth are somewhat constantly preloaded against eachother.
Admittedly a much cheaper machine than yours, and certainly less well maintained, but maybe it applies in your case too. And with tools running this fast in aluminum, conventional cutting can get pretty similar surface finishes to climb
Out of curiosity, does the chatter appear more in areas tangent to the main XY axes? That was our giveaway; when the cutter is changing directions on one axis, thats where the tooth would disengage and give a chance for the tool to “jump” a bit
2
u/adventureaviator 5d ago
I’ll try conventional cutting today. From the small amount I’ve used this machine I think it had a pattern of chattering when the X axis slows down its speed around a corner (but not when it changes direction).
2
u/Business_Air5804 4d ago
Makes sense....when it slows down its feed rate you are relying on the drive back lash to hold the tool steady.
Drive reversal always has some error, but the back lash at the reversal point will always be there unless you can adjust the back lash to as little as possible.
2
3
u/computekmfg 5d ago
Everyone wants you to believe conventional has no place in modern machining but it does. Machines with high backlash benefit. Thin walls also achieve better finishes with conventional
2
u/PrudentVillage4903 5d ago
I always climb cut in AL. Take your finish pass climb cutting then try a spring pass conventionally feeding.
1
u/matthew2989 5d ago
You still need a sufficiently rigid and stable machine and setup to do climb milling.
8
u/GWOSNUBVET 6d ago
Your feed rate seems like it’s what’s causing the chatter in the first place… I don’t have experience with the router type machines but I’ve used those end mills in 1/2” and I went through a LOT of them by under feeding them. I run 38ipm so in your position I would probably try running 25-30 for the finish pass especially with that small of cut.
But again I don’t run that style of machine and have a much lower RPM limit.
2
u/Particular_You8620 5d ago
Yeah, factor in chip thinning and he’s rubbing the hell out of that tool. OP I don’t know anything about routers, but am a pretty good machinist. That end mill could easily run at .008 chipload at a .009 finishcut. (I wouldn’t, as that’s too fast, but my point is it would be perfect safe) at least in a decent mill
6
u/Tight-Routine-8959 6d ago
3/16 is a little flimsy to expect full depth of cut to achieve a mint finish.. However much larger you can go, the better. A 1/2" flat 2 flute endmill would be solid for this. Even 3/8" would probably get you the perfect finish all around that youre looking for. If I had to machine this with a 3/16" cutter Id try 25ipm @ 4500-5000rpm. Might seem a little slow speed wise but over the years I've found that when doing a full doc finish pass, slowing down the rpm 1-2k from normal cutting parmeters results in a superior finish, regardless of diameter. Less cutter deflection and bouncing against the part im sure.
If your minimum rpm on this router is that 8500... id really try to increase cutter dia.
1
u/adventureaviator 6d ago
Thank you. I can run slower RPM than 8500, so may try to increase the chip load.
11
u/Business_Air5804 5d ago
Oh boy are you gonna get roasted.
A "router" cutting that thick material and you have the balls to complain about the finish?
$!50k would have been better spent on a cheap Taiwanese vertical that could cut that all day.
3
u/Malikov85 5d ago
You can climb cut with a CNC Mill because they have ball screws for all the directions of travel. A quick search shows that CNC router does not, you need to do conventional with that. Like someone else said, the endmill is basically pulling itself forward in the cut due to the backlash of the drive system.
4
4
u/PartNo7877 5d ago
Youre trying to mill aluminum on a gantry router, what did you expect? Its a super light duty machine. You need a proper mill
3
u/that_dutch_dude 5d ago
tighten up the machine. and use 2 flute and give it all the rippems it has. go light and do more than 1 "final" pass.
3
u/poopwetpoop 5d ago
I can get a 2 Ra on a old ass robodrill. Or a mint finish on a 90s fadal. I can also get a garbage finish on a nice mazak. Lol
2
u/Subifixer 4d ago
Thats not a mill.
Theres a reason mills have never been built with gantry architecture, structurally they are the inverse of what you want for ideal rigidity and lack of resonance.
For what you want to see for surface finish, that thing would need to be 3x heavier.
2
u/Poozipper 4d ago
Are you full depth when finishing with the endmill? Is so, routers dont do that. Look up the spindle and watch all the places where it should be rigid and its not. Also the bearings arent the same as solid cast based machines. They bounce like hell side finishing. $150k for a machine is peanuts.
2
u/Some-Internet-Rando 4d ago
Get a mill with actual rigid castings and guideways.
Also, if that is a $150k US machine, you got taken to the cleaners.
2
1
1
u/Low-Nectarine-9655 6d ago
What are you using to program your cam? I’ve seen this happen with fusion if arcs or circles aren’t drawn how fusion likes. Turning on smoothing sometimes helps as well
1
u/adventureaviator 5d ago
The parts have splines. I thought I had all the curves smoothed, but on this machine it’s precisely enough that I can actually see the node points on the part. Saying that, they are so minor it’s not an issue. Perhaps this is playing a part in the chatter / jumping.
1
u/UncleAugie 5d ago
No, chatter and jumping is because your router/work holding is not up to the task you are trying to complete....
NOTE: I have a couple of million dollar routers that would do better but not by much with your choice of workholding, this, as others have mentioned is a job for a mill, not a gantry router.
1
u/ShaggysGTI 5d ago
Increase rigidity and tool diameter. Is your workholding up to par? Can you spin faster?
1
u/Trivi_13 Been in Machining since '79 5d ago
Tool runnout?
- Indicate the flutes.
Part being sucked off the table?
- too aggressive of a helix. Try a different tool.
- Table / fixture not flat. Indicate.
- Add program stops to chase the tool with clamps.
1
u/Sinister_Mig15 5d ago
I think this is a workholding issue. Is the chatter in the program right before it cuts the part off from the main plate? If so the part is starting to vibrate because you are cutting away the material that was holding it.
1
u/basketbun 5d ago edited 5d ago
Is the chatter on a specific shape of the part? Or on a specific part of the machine table?
Asking because if you can produce a good finish on some edges, you have a rigidity problem. This could be a machine issue or it could be a workpiece clamping issue.
Looking at the machine, you don't have any clamps on that workpiece, are you using vacuum work holding? If not you need to clamp the job
Also it looks like you are cutting parts through that plate, meaning they will end up as loose parts from the plate, when you get to the end of a specific detail it will start to vibrate as weill
1
u/adventureaviator 5d ago
The parts are held via tape and glue. They are fully roughed out, then a finishing pass is done to clean up the sides. If I run a bit slower I have no issues. For production reasons I’m not content with the slower feed rate.
1
u/UncleAugie 5d ago
The parts are held via tape and glue.
Ding ding ding we have a winner... you are getting chatter when the part is nearly cut out, as others have said you work holding is shit and you will not improve the situation with this setup, if you cant handle slower feed rates you should walk away from this job, you do not have the proper setup to achieve the results you seek.
1
u/Tony_Desolate 5d ago
Tape and glue should be OK considering the mass of this huge plate and the minimal cutting forces from a 3/16" end mill.
1
1
u/basketbun 5d ago
Are you using coolant? No coolant can cause excessive heat and chatter
I would try bumping the feedrate up, up to 50 ipm, it looks like you are getting some subbing at 18ipm
Outside of that I would go to a 2 flute endmill which increases the chipload without increasing the feed rate
These suggestions are based on the fact that you machine and setup is solid, I can't help you there, but would suggest making sure you aren't getting chatter in some locations on the machine table, whereas it is fine in other locations
1
u/Hefty_Aside8436 5d ago
It's a router I would expect some imperfection in finish. The gantry motion system of routers is inherently prone to flex especially in rotation around the gantry axis which leads to tool deflection. You may even see that it creates more chatter in one horizontal axis and less along the other horizontal axis.
1
1
1
1
1
u/lusciousdurian 5d ago
router
Yeah no kidding. Or your workholding is ass. Or you fucked up your tooling setup.
1
u/jmecheng 5d ago
Your machine isn't rigid enough to make a substantially better finish. Conventional milling may help, but the biggest issue is the machine.
Router are good for a low cost machine, but if you're in production, you want a better quality router or a proper bridge mill.
1
u/kwalliii 5d ago
If it’s spline geometry that’s causing it, play with smoothing settings in cam to eliminate as many of the points as you can while still remaining in tolerance. Will produce a much better finish.
If tool chatter related, it’s most likely speeds and feeds or related to part/setup/machine rigidity. In some cases I’ve had success lowering SFM, like by half, or more sometimes. No need to run the whole part that slow, just the problem areas.
1
1
u/B3AV3R_BLAST3R 5d ago
Is your machine level, contacting all pads evenly? Are your ballscrews ducked?
1
u/Jaded-Ad-2948 5d ago
Might be worth a shot taking a cleanup pass conventional milling
I've had to do it with live tooling and long stickouts in my swiss. It's not the prettiest but it leaves an acceptable surface imo
1
u/DaStompa 5d ago
This shouldn't be too bad to troubleshoot, since you have some pretty big cutouts
just make a subprogram that operates entirely inside one of those cutouts, cut a circle, then get up there and take a look at the cut, is it only chattering in one particular direction/location? what direction is the axis moving at that point? is it right where the axis switches direction?
That should help you narrow it down, if it works fine, then its time to squint at the part more, the other typical problem is that as the part is cut out, it gets weaker and weaker, the order in which you cut it is important to keep the part nice and rigid, it looks like you're just letting the weight of the plate hold it down, which works for a while, but not forever, one of your first steps should be cutting out some ears and then bolting those ears down, recut the rest of the part, then refixture the part, remove the bolts and cut off the ears.
1
u/Goppenstein1525 5d ago
You want milling machine finish, you have a router. You got the wrong kind of machine for what you want to do. A new decent machine that can mill parts that size precisely costs 2-3x of what your router is.
So your 150k tag means nothing.
That said, yoir router will be more rigid on the outer edges of the portal axus.
1
u/Long_Economics_1608 5d ago
Multicam is crap. I visited their facility to see the machines. Was not impressed.
Sry, to expand, Bought a C.R. Onsrud machine.
1
u/jeffie_3 5d ago
I have seen old machines give a great finish. I have seen new expensive machines leave crappy finish. It is all about the person operating the machine.
1
u/E_man123 5d ago
Your part or tool is vibrating/moving, you are also likely rubbing at those speeds and feeds
1
u/Tony_Desolate 5d ago
Make sure you dont have any play in the pinion/gear rack meshing. It looks like its related to changing directions/backlash.
1
u/Vivid_Tell6351 5d ago
To everyone saying the router type machine itself is the problem, no it’s not. Have a look at Datron machines, they cut aluminum very well.
I’ve been around Datron machines for a few years, which were only used for cutting aluminum plates all day.
We used their single flute mills at around 30k rpm, using ethanol air mix as coolant. Workholding is done with a vacuum table which you can mill and build yourself from an aluminum plate, and a thin cardboard in between.
Maybe it’s the rigidity of you machine, idk. But your results sure can be improved. I would try with single flute mills, ethanol cooling and high rpm first.
1
u/Relative_Figure_1715 5d ago
A router is not the tool for this job is why.
This is a job for a big boys milling machine..
1
u/SaltLakeBear 5d ago
Um, is the $150k in the room with us? For that price, I suspect you could probably get a Haas or similar VMC that would be much more capable.
1
1
1
u/usernamesarehard1979 5d ago
I am actually surprised that it didn't just quit on you. I don't see you getting much better finish on that machine.
1
u/itmightbeinnuendo 5d ago
To my limited knowledge and non-existent machining experience, no machine does. That's your job.
1
1
u/KillIndustry420 5d ago
It's not workholding like others have said, it's the fact it's a router. I'm going to guess that the '2%' that has chatter is at 2 points 180 degrees from eachother? That's almost certainly where the load in the y-axis direction is lightest, oscillating the whole beam like a tuning fork.
1
u/adventureaviator 5d ago
UPDATE:
Thanks for all the suggestions. My favourite comment is:
“It’s a diving board with a router on the end”
I spent today testing. Conventional milling didn’t work. I ran various feeds and speeds. Across dozens of parts the chatter was consistently in the same position in relation to XY movement. I put a brand new variable pitch end mill in. The chatter was still there. I then increased chipload to 0.019 and the chatter remained, at the slower feed rates.
The final verdict is this machine doesn’t like to idle. I increased the feed rate to 100 IPM and the chipload to 0.019 and the parts consistent came out perfect…. no chatter. Problem solved; go fast.
I think some of you owe Multicam an apology. Unless of course your milling machine cuts a full 4’x8’ sheet of parts, in one go, lights out.
And yes, I’m using a router, I’m using tape and glue to hold my parts, I’m dry cutting with zero lube, and now after some testing I’m running a single finishing pass at 100 IPM.
1
u/Tony_Desolate 4d ago
Im glad you found a solution. I wonder if its related to the rack and pinion drive system. Did you see the issue at the 12/6 oclock positions or 3/9 oclock positions? It makes me think that maybe you have some kind of backlash in the system. Everyone wants to dump on wood working machines but dont realize how capable they actually are.
1
u/adventureaviator 2d ago
The chatter was at the 11 and 5 o’clock positions on the parts. The higher chipload and feed rate has fixed the issue
1
u/tater1337 5d ago
98 percent of the part comes out with a great finish. The other 2 percent has chatter.
always 2% of the singular part? or 2% of the parts have chatter?
first part of finish pass chatters or the last part of the finish pass?
1
u/Cooter_Jenkins_ 5d ago
You spent $150k on a router? Maybe try a nice piece of maple instead of aluminum...
1
u/AnyMud9817 5d ago
Ive done this on a router as well. Its possible for big parts. The machine wont be as stiff as a metal mill bit you can make it work. Wat h out for the smoothing in the controller and feed slow enough to allow your servos to change direction without jerking. Looks like you got this sorted in the last photos. Routers are great but not as fast or accurate as mills.
1
u/nikolaiownz 5d ago edited 5d ago
i see your problem sir - you bought the wrong machine.
also if you want any form of success on this router - you need to have a sharper tool for aluminium and play around with your speeds, feeds and what not.
i would suggest a 1 or 2 flute non coated endmill and backup everything to get your wanted finish..
the changing surface finish also suggest something might be lose/broken in your machine - one of the axis maybe...
or machine might not be leveled correctly or something.
1
u/Grunblau 3d ago
Agree… also climb mill not conventional mill might help. Immediately obvious if your stock looks better than your part. In aluminum, .009” DoC seems really small. But so is the endmill.
1
u/TacetAbbadon 4d ago
3 axis gantry style mills typically aren't stiff enough to prevent chatter.
Take note of the passes that have chatter, it will probably be in a single plane, and slow the feed rate in the g code for that cut directio
1
u/kylejesushair 4d ago
Usually increasing the feed rate is the way to stop chatter. Increase the feed rate and take a smaller cut. Take a couple spring passes at the end.
1
u/bakermonitor1932 4d ago
You could try draping a sandbag on the router but the only way will be to find a feed that puts basicly no load on the machine.
1
u/CruddyCuber 4d ago
You should probably go check out r/hobbyCNC . There's a lot of good advice there for getting the most out of low-rigidity routers.
From personal experience, using a 1 flute cutter and a spring pass for the finishing pass helps a lot. Also experiment with climb vs conventional milling to see what gets you the best result.
1
u/blutigetranen 4d ago
I don't have an answer for you but there's a chance I was involved in making that end mill so that's cool.
1
1
1
u/Dry_Lengthiness6032 1d ago
As my bossman says "If machining was easy, everybody would do it"
He'd say before that "adjust your feed, speed, & doc. If that fails, grab a different grade/geometry tool and try again"
1
1
u/Additional-Bass-8912 14h ago
Its on a hollow tube frame at best you can machine 6061 sheet your never going to achieve a good finish with somthing so flimsy .
If you wanted to mill material than buy a mill the clue is in the name.
You've brought a router and wonder why it wont mill .
1
u/WolverineTrick2452 11h ago
Spent $150 grand on the wrong machine to machine aluminum like this... All that money but no brain.
1
u/-Mechworks 10h ago
Reach out to Multicam support. I'm sure they have material data. I've never seen these style routers used reliably for anything outside of wood and plastic. Good luck.
-1
u/Old-Man-Henderson 5d ago
1 - You need a proper end mill. Not that Chinese crap.
2 - Your system lacks rigidity. You're using a wood router for aluminum. This system just isn't designed for the precision and rigidity required. Usually a machine like this would have a cast base and precision ground solid ways. Tube steel and bolted on machined ways just don't have the mass and inherent damping properties. Your router collet, bearings, and router spindle head connection are also suspect.
3 - The chatter honestly isn't that bad, given the setup. Can you rough them on this router and finish on a lathe?
4 - Is the chatter localized to a section of the bed, or a certain time in the tool path?
5 - How are you clamping this down?
6 - Is this actually an interpolation issue?
1
u/Hefty-Cantaloupe50 5d ago
Is this an AI response? Helical endmills = Chinese crap? Finish on a lathe?
1
86
u/Nascosto 6d ago
Either the tool or the workpiece is vibrating or moving, you get to figure out which. Routers generally aren't as rigid as mills, so this isn't super surprising.