[8man]

I converted a 47158 harbor freight micro mill to cnc. The cut that I am attempting to make is: facing a .250 piece of 2025 aluminum. Using a .250 cutter at 2000rpm. The tool chatters a lot. Even with a super low feedrate, ex. .25 IPM, still chatters. (not as bad but still there)

No play in the axes. There is backlash in the gear drive. Is this the trouble? More cutter speed? I can do the same cut with .125 cutter, and have no issues. (at the same feedrate) I need the .250 cutter, it is a ball end and I am using the ball at a different spot. Don't want to switch cutters. Help.

[snowshovelbmx]

If it is a hss endmill I would maybe try slowing down the RPM to 1100 and increase the feed to about .002" Chip/tooth. so if you have a 4 flute E.M. run it at about 8.5 IPM

chris.

[8man]

So if its a 2 flute, try it at 4 IPM @ 1100 rpm?

Sorry this part has me puzzled. (increase the feed to about .002" Chip/tooth)

[xiphmont]

Stupid question--- but is the quill locked? Since it's CNCed I assume so, but maybe it came loose... Whenever I have chattering trouble suddenly show up inexplicably, it's often because the quill got loose, or I forgot to lock it again after some plunge milling.

The gear train shouldn't be the source of any chatter, but it will make any chatter *sound* alot worse. I used mine for a year before going to belt drive and had often wondered the same thing, but the belt drive didn't make it chatter less, it just made it quieter.

Monty

[laszlozoltan]

Its a fairly thin piece; have you faced something this thin before without the chatter ? ( sorry, I am unfamiliar with desktop mills, just the monsters).
How are you holding the workpiece ?

[xiphmont]

Its a fairly thin piece; have you faced something this thin before without the chatter ? ( sorry, I am unfamiliar with desktop mills, just the monsters).
How are you holding the workpiece ?

.250 counts as thin? I guess you _are_ used to the monsters :-)

Or is it .250 wide and thinner than that...? How much is he taking off? I'm used to getting chatter when the planets align wrong and I'm cutting 1/8" deep four inches out from the center of the rotary table and the table has gotten loose, but facing should be damned near effortless with a cutter that small!

I usually just bolt flat pieces right down to the table at the edges. I know, you weren't asking me :-)

Hmm, other thought... hidden play in the ways? Crank the X all the way out to the right, put a finger on the seam between the base and the Y saddle and wail on the X crank... feel any shifting at all? Do the same with Z.... any shifting? If so, that's a likely culprit right there, a jib needs tightening... I know, it's another stupid question, but something isn't the way it should be.

(more grasping at straws... nicked/notched/burred endmill? Oh... it *is* a face-cutting endmill, right? OK, yeah, that's another super-stupid question :-)

Monty

[laszlozoltan]

it could be just a matter of how is he employing his endmill to face the workpiece; could be just the direction he is milling, or distance between his clamps, what is supporting his workpiece ...to diagnose his problem without more information is just random guesswork. Just trying to elict some more information that could be useful.

[xiphmont]

it could be just a matter of how is he employing his endmill to face the workpiece; could be just the direction he is milling, or distance between his clamps, what is supporting his workpiece ...to diagnose his problem without more information is just random guesswork. Just trying to elict some more information that could be useful.

True enough. Part of my response was me getting confused who had posted what... I went back and edited it so it at least made some sense.

Monty

[8man]

The piece is in a jig and held tight.

The axes have no noticable play, but I tried tightening them anyway. Even a slight bit more pressure and my stepper motors stop.

The cutter starts off of the workpiece, and then comes in slowly. .100 from the edge. Yes .100 deep. That's why I am moving so slowly. Even at .25 In/min it still has a slight chatter.

If I try to run the cutter straight into the material, (not facing, but like trying to cut it in half) I cannot run it slowly enough.

The workpice is .250 thick. I am basically notching the ends .100 deep x .336 wide.

The cutter doesn't matter. New, used, 2 flute, 4 flute. Am I asking for too much? I figured that if I slowed the feedrate to a crawl, that I could make this in 1 cut.

.125 cutter can do this job easily, but I need the .250. Otherwise I have to change the tool for the last cut.


Please, there are no stupid questions. The micro mill is not something that I am used to. The big mills and cnc, I know about.

[laszlozoltan]

Ok, well my experience tool chatter was eliminated by reducing the spindle speed. You say you are running 2000 rpm a .25" endmill ? I used to slow my feed rate down when I got chatter; then I was learned that reducing the rpm does it. Try it at a more normal feedrate; say 1000 or even 900 rpm.

[xiphmont]

The cutter starts off of the workpiece, and then comes in slowly. .100 from the edge. Yes .100 deep. That's why I am moving so slowly. Even at .25 In/min it still has a slight chatter.

Oh. ...maybe I was taught wrong (heck, good to find these things out), but I'm used to 'facing' without additional context meaning a final surface dressing (eg, a nice .002 last pass to get things nice and flat). The handbook agrees with you, I've just not heard the guys around me refer to any face cut as facing....

Anyway, now that I know what you're doing, that's a very deep slotting cut for a .250 endmill and the x1. I would expect it to be able to do it (and I've done it regularly--- manually) with constant lubrication, a locked down Z, and a brand spanking new fresh razor sharp endmill straight out of the box. If it's bolted onto a jig, I'd hope that jig is a minimum of 1/2" stock...

However, this is at the limits of the X1's rigidity. The z column is just not stiff enough, especially unlocked, to handle that depth of cut in one pass with any reliability. You should make that cut in several passes.

The cutter doesn't matter. New, used, 2 flute, 4 flute. Am I asking for too much? I figured that if I slowed the feedrate to a crawl, that I could make this in 1 cut.

.125 cutter can do this job easily, but I need the .250. Otherwise I have to change the tool for the last cut.


Please, there are no stupid questions. The micro mill is not something that I am used to. The big mills and cnc, I know about.

Yeah, this is too much -- in one pass-- to expect of the x1 without Z column stiffening mods. Doing the cut is still easy though if you can do it in multiple passes.

[snowshovelbmx]

I would have to agree in doing the cut in multiple passes, even two passes at .05" should make a big difference. The answer is hardly ever slowing the feed right down at .25 ipm and 2000 RPM and a two flute cutter each flute is cutting .00006" of material. In other words you are rubbing the material off and dulling your endmill very quickly possibly introducing the chatter. I would try multiple passes at about 1000 RPM and 4IPM if the X1 can handle it(I have never used one myself).

Chris.

Oh and chip/tooth refers to how much material each tooth of the cutter is removing.

[8man]

Stiffening? Please explain. The Z is not locked, the jig is thick.

What would be a realistic expectation as far as the depth that can be cut reliably? With that same .250 cutter?

With all of the knowledge I am gaining here, I still have a problem.
The one notch that is am making goes al of the way through the material, about .500 wide, right into the side. When I advance my cutter into the side of the material (have to start somehow) I get major chattering. Imagine making a U shape form a square piece of material. How do I remove the middle of the U without, Z down, cut it all out, Z down some more, and repeating this a lot? I am guessing from my results that advancing straight into the side is not going to work.

Thanks a LOT for all of the help, I am learning quite a bit.

[xiphmont]

I would have to agree in doing the cut in multiple passes, even two passes at .05" should make a big difference. The answer is hardly ever slowing the feed right down at .25 ipm and 2000 RPM and a two flute cutter each flute is cutting .00006" of material. In other words you are rubbing the material off and dulling your endmill very quickly possibly introducing the chatter. I would try multiple passes at about 1000 RPM and 4IPM if the X1 can handle it(I have never used one myself).

Right, he hits the other part of why it's not working at such a slow feed rate... You're not anywhere near getting under the chip at 2000RPM and only .25IPM.

When I've done such aggressive cuts in the past, I took the feed rate way down, but I also took the spindle speed way down. The last recent 'pushing the x1 farther than it should go' I did was repeated .130 deep x .150 wide cuts (but not slot; I was only cutting on one side) with a four flute 3/8 mill at a spindle speed down around 800 but still feeding a good 4-6IPM or so; this was by hand, so that's a guesstimate. It didn't dive in, grab or chatter, but it was danged near vibrating off the workbench. This was with Y and Z locked tight and only using X; unlocking Z would cause it to dive in, unlocking Y caused it to wander.

That's about as far as I would take the x1 and expect it to work every time. Oh, with 6061-T6 in case that matters.

Monty

[8man]

So at 2000rpm a 2-flute cutter at 4 IPM would remove
.001 per flute/per rev. Is this correct? I think so.

So at 2000rpm a 2-flute cutter would have to run at 8 IPM, to make a nice cut. It's not that I want to turn the spindle that fast, just an example.

[xiphmont]

Stiffening? Please explain. The Z is not locked, the jig is thick.

The x1 is small and the Z column is thin and not particularly stiff, at least not compared to any larger mills. It's just flexy enough and the dovetails small enough that the head can droop or get flexed around pretty substantially in aggressive cuts-- thus chatter or worse, grab-in/dive-in.

There are folks out there who have made thicker columns, filled the colums with concrete, added head counterweighting, etc, to try to make the mill stiffer. IMHBCO, not worth it. There are lots of mods worth making to the x1, but that's not one of them. If you need something stiffer, get a bigger mill. If you don't want to get a bigger mill, just bite off smaller cuts at a time. Give up on the idea of just assuming you can make any cut you want in one pass.

What would be a realistic expectation as far as the depth that can be cut reliably? With that same .250 cutter?

A direct slot, cutting on both sides? Depends on material and how 'tight' the mill currently is. But like the other gentleman said, two .050 deep passes will be way easier than 'twice as easy as one .100 pass'. Especially since aluminum is soft and gummy, deep slotting cuts hit the wall real fast.

At a guess? I'd not try any deeper than .050. And if you're computer controlled, I'll bet two .025 passes will end up being reliably faster than one .050 pass. That is a guess; don't be surprised to find I'm off by a factor of two in either direction. I still work substantially by hand (most of my parts are simple and one-offs), and I know the 'feel' of the mill and materials well. I just dial in and go, and when it doesn't feel right, I adjust.

With all of the knowledge I am gaining here, I still have a problem.
The one notch that is am making goes al of the way through the material, about .500 wide, right into the side. When I advance my cutter into the side of the material (have to start somehow) I get major chattering. Imagine making a U shape form a square piece of material. How do I remove the middle of the U without, Z down, cut it all out, Z down some more, and repeating this a lot? I am guessing from my results that advancing straight into the side is not going to work.

Thanks a LOT for all of the help, I am learning quite a bit.

Don't go deep. Keep the mill tight. do you mean chattering or squealing? Real chattering means you're going too fast. Squealing means you're going too slow. Both can mean you're just cutting too deep.

Monty

[project5k]

if i may, can i interject a question to xiphmont?

ok chattering is taking too bigga bite per flute on the endmill?
and squeeling is the tool rubbing and not cutting effectivly?

i'm just trying to understand as i'm still fairly new to this myself...

[xiphmont]

if i may, can i interject a question to xiphmont?

ok chattering is taking too bigga bite per flute on the endmill?
and squeeling is the tool rubbing and not cutting effectivly?

i'm just trying to understand as i'm still fairly new to this myself...

I keep hoping other people will pipe up too... I'm not exactly formally trained, I just absorbed this stuff from doing it and being around other guys who did good work but weren't formally trained either. We're all engineers, and we're just sort of expected to know/be able to do this stuff, no one ever taught us... "You need a part? The machine's over there. Quit whining and go do it."

When I feed too slow while trying to cut too much, the cutting edge doesn't have enough material to bite, so it's not actually cutting. It more abrades/pushes the material rather than slicing in and chipping/cutting it off. It will probably also be squeaking and squealing the whole time, exactly like an unlubed bearing that wants to seize.

If the mill biting too hard and deep, either because the feed rate is too high or because something is loose, it can resonate and self reinforce causing chatter, or if it really gets out of hand, dive-in/grab-in. The x1 isn't all that stiff, so that's a problem to contend with regularly. It's flexible enough that if a flute grabs too much metal, all that stored up energy in the drive train can reel the whole head in and cause a huge mess (then it will probably spring free and snap back like a huge steel spring, and something ends up broken).

The squealing from going too slow will have no vibration associated with it... well, no cutting vibration, the squeal will vibrate... cutting just sort of stops even though everything is spinning.

Chatter vibrate like the mill is trying to tear itself (or the workpiece) apart.

In either case, stop and contemplate the situation before you burn up the end mill or break something :-)

The mill also has natural resonances that you can exploit/avoid. One of the first things I learned is that sometimes you'll get some mild chatter on a moderate cut because it just happens to tickle the mill right and the correct (if paradoxical) solution is increase the feed rate. That one's hard to explain... you just end up knowing it when you hit it. Some RPM/feed rates just don't mix on small mills and that one is hard to predict.

Monty

[Dar]

sounds to me like you shouldremove the ball end mill and use a sq end . ball end mills have a lot of surface area.how can you face with a ball end mill anyway???? Dar

[project5k]

ok, well on my x3 i have run into a little squeeling now and then, so i was just wondering... i dont really have a chattering issue, course i'm not cutting that hard or fast either..

ok, i think i get it, i'll try it next time i try and cut something... squeeling = speed up the feed a little..

thanks