Noise and chatter when milling, HF 42976 machine

[PStechPaul]

I have not done a lot of milling on my Harbor Freight 42976 milling/drilling machine, and when I have, it is quite noisy. I am running at 400 RPM, which might be somewhat low for a 1/2" four flute end mill. It's about 52 SFM, while it should be more like 220. But I think it has mostly to do with the lack of rigidity of the machine, and also because of the rather long distance from the spindle to the end of the mill (almost 5"). I was using it this time to mill a tool holder for my lathe, basically a 5/16" x 5/16" notch in 1/2" square mild steel, for tooling of the same size, rather than using shims:





Here is a video of my experience:

I think the end mill is OK. It feels pretty sharp, and there is only one small chip on a cutting edge:

[Ironwoodsmith]

Did you try it at a higher RPM?

[Arthur.Marks]

Up the feed rate, man!! Haha! & if that is just plain steel (~1018CRS or similar), why running so knowingly slow? With HSS and plain steel, I usually just plug 100 sfm into the formula because it makes it easy. More often a racket noise is just a loose screw somewhere and has nothing to do with poor bearings, machine rigidity and the like. For example, on my mill/drill, the middle pulley between the motor and spindle swings on an arm. The arm has two bolts that hold it in place but can't be fully tightened. If they are, no more swivel adjustment. Those two bolts work their way loose regularly and start to sound like a metallic snake rattle while the spindle and pulleys are turning. I'd be looking for loose connections like that first. In the meantime, try pushing that endmill! They actually like it better

[PStechPaul]

I suppose I have always approached machining with a lot of caution, since I have not had the benefit of a mentor showing me what to do. Also, my previous milling experience using the Jacobs chuck rather than a proper mill holder has made me a bit "chicken". I calculated the SFM after the fact, and I've usually just used this low RPM for almost everything.

[edit] I used the 220 SFM from a chart for turning. For milling plain carbon steel it's 65-110 for 1006-1026, and 25-100 for higher grades: http://www.littlemachineshop.com/Ref...tingSpeeds.php

Also, I had started with a vertical depth of about 0.01 to 0.02, and then worked my way up to 0.020 to 0.050, and the full width of the notch (0.312"). I don't have a fine vertical feed (Z-axis), so I just loosen the spindle lock slightly, tap it down a bit, and then give it a try.

I was also wondering if it was better to set the depth to the full 0.312" and take multiple passes using the Y axis, or shave the full width of 0.312" as I did, and then take cuts at increasing depth, which is whatI did. Next time I need to do something like this, I'll get a little more bold and up the RPM and feed rate.

Also, perhaps a collet would get the cutting edge closer to the spindle. They are available from Little Machine Shop for $11 each.
Thanks.

[Arthur.Marks]

Your caution is completely understood and not at all a bad thing. For that particular piece, I wouldn't take the whole .312" depth of cut for the simple reason that there isn't much of the workpiece to hold onto in the vise. There is also a relationship between depth of cut (DOC), feed and speed to be aware of. A deep cut at a slower feed is similar to a lower DOC at a faster feed. Varying the spindle rpm with the same feed rate also changes the amount of material each flute digs into to make the actual cut. This is called chip load--a similar but different way to measure the "depth" of the cutting action.

So now that it sounds terribly complicated and esoteric, I'll say that SFM and RPM is all that really needs to be referenced and calculated out. The rest can be picked up by feel on the manual handwheels and learned by experience. I'd recommend getting a good size block of steel that is taller than your vise jaws and try burning up an end mill It'll teach you a lot. Try deep cuts, shallow cuts and fast cuts. See when and how the resulting surface finish and end mill performance relates.

Before all that, though, it sounds like you are building confidence in both toolholding and workholding. In that respect, those end mill holders such as you are using are extremely safe. The end mill is physically retained by the set screw, and the holder is physically retained by the drawbar. The failure modes are going to basically be *overheating the end mill--it'll turn colors and start to look like a misshapen lump instead of having cutting flutes *break off a sharp corner on one of the flutes, thereby creating a horrible surface finish only good for roughing *overheat the workpiece--then there aren't "chips" because the molten mass welds to the edges of your cutting tool, happens a lot with aluminum

I expect, though, you will be shocked at how much of a cut, feed, force it takes to achieve these failure modes with a 1/2" HSS end mill. Anyway... I don't know if my verbose reply has anything to do with the original intent of this thread. I apologize for that...

To address your specific questions:
*yeah, 20 - 50 thou' DOC is pretty normal for a machine of that size.
*I like to use the longer length of engagement on the edge--not the end--of the end mill if possible. I think that is what you were getting at with the third paragraph above?
*collets are good, but I would like to know what your spindle is: R8, MT2, MT3? When you start getting into larger end mills, like 5/8" or 3/4", collets of these types start to become questionable in resisting large cutting forces (depending on who you're listening to ). Just something to heed and be aware of.

Re: noise, rattles, etc.
I should have also mentioned that locking unused axis is a good practice. So if you're only feeding in X axis, lock Y axis and Z axis (quill). That might help too.

[PStechPaul]

Excellent advice. Certainly a few things I can try. I have quite a few large endmills, some of which are not as nice as this, so I wouldn't mind trashing one. I have a set of new Harbor Freight 2-flute mills, but I'd rather not mess them up. And I like 4-flute types better - they just seem to cut smoother. Also, I think using the full outside edge of the mill gives a better cut because of the overlap of the spirals. I'll have to do some experimenting and report back with results.

Thanks.

PS: I found a video that shows a very heavy and fast cut.
https://www.youtube.com/watch?v=1AMZlDHwebw

[Old Hat]

Holder issues.
The holder's diameter at the point Mr Morse leaves the quill
is the limiting factor. Good as it's gonna get pretty much.
the heavy-er feed ratio might buy you a little sollace but only just.

[PStechPaul]

It's hard to find good videos of manual milling of the sort I was doing. The link I provided was CNC. Here is milling of slots in steel using a Bridgeport, and the material removal was not all that much more than I was able to do, once I settled into the process. I think a higher RPM and somewhat heavier feed may reduce the chatter, and tightening the gibs also helps.

The Bridgeport (most of the action is toward the end):

[becksmachine]

Noise?? On a HF mill drill machine??

Ok, I didn't read all of Arthur's replies so if I duplicate here, sorry.

First, you are absolutely correct, 5" is way to much overhang. Are you stuck with using Weldon style holders or is there a collet setup alternative that you could use? I am assuming here that a collet would reduce overhang considerably.

Second, you have taken very good photographs and because of this it is plain to see that that end mill is essentially junk. Chips in the margins of the flute indicate a number of problems with the operation, none of which are good. The bright line on the edge of the flute that extends each way from the chips also indicates the "dullness" of the cutting edge. This is visible where the helix of the flute allows the light to shine on it at the correct angle.

Third, the advice to run greater FPM at higher feed rates could possibly make the operation quieter, but it would more likely cause some greater catastrophe. I think that the premise here is that feeding harder will keep the slop and deflection going one way continuously, but that would do nothing for precision. I think that your selection of rpm is actually right on, 50 FPM with HSS tooling and no coolant is about right, and the depth of cut may be light, but that should help eliminate chatter, not cause it.

Fourth, this is probably not the best application for a 4 flute end mill, especially on steel and in a very light (as in FLEXIBLE) machine. If you were using the sides of the end mill to take a few thousandths off of an edge, you would achieve smoother finishes for any given combination of feed rate and spindle rpm. However, if you were wanting to remove an 1/8", a four flute version would just chatter.

On even the heaviest machines, a 4 flute would chatter and leave a horrible finish and probably an oversize slot whereas a 2 flute end mill will cut a keyway to full depth in one pass (1/2" wide X 1/4" deep, 3/8" wide X 3/16" deep, etc.) without chattering. Now this slot will not be absolutely plumb, as the end mill will have a significant amount of deflection while making this cut, but it is usually of no consequence as the slot will be very close to the proper size to provide a tight fit for the key.


Dave

[schor]

Lots of good replies already.

I'll just speak from experience as a newbie myself. I used to run really low speeds on my benchtop, usually forgot to lock the quill and/or the unused axis and not enough cutting fluid/coolant.

For cold rolled I go with 100sfpm then use the basic formula spfm*4/dia, in your case 100*4/.5=800rpm. Running at a faster speed effectively gives you more control on the feed rate, with the flutes flying past faster they are each taking less cut if you keep the feed rate the same as your slower rpm. Just start out with light cuts and increase until you feel your in a sweet spot.

The first time I started speeding things up I had some anxiety, but your in control with the feed and depth of cut, so start small until you get your confidence up.

[fixerdave]

...
On even the heaviest machines, a 4 flute would chatter and leave a horrible finish and probably an oversize slot whereas a 2 flute end mill will cut a keyway to full depth in one pass...

All this time...

It never occurred to me to try a 2-flute to reduce chatter. I always thought a 4-flute would be "better" and only used 2-flutes when I needed to plunge into the work. Wouldn't be the first time reality disagreed with my understanding Any idea of the underlying theory as to why 2 flutes chatter less?

I have found, with my flexy little Chinese 3:1, that smaller endmills chatter less (1/2" instead of 3/4"), that tightening down all possible axis is important - even snugging up the one being moved, and to avoid climb milling if at all possible, no matter how light the cut. I just use feel to set the feed rate, sometimes pushing a bit more if that helps reduce chatter, sometimes backing off to get out of the chatter-zone. Oh yeah, sharp is good too. Next time at the mill, I'm going to try a 2-flute.

David...

[mattthemuppet]

I have about 10h experience using a mill and most of those are on a converted drill press, so I'm hardly one to offer advice. However, the few things that I've learned machining brass and alu is that cutting oil helps (alu at least), don't climb mill, milling with the end instead of the side seems to require less power, roughing end mills are totally awesome.

I also go by ear alot - the squealing sound of rubbing (too shallow a cut) is quite a lot higher pitched than the noise produced by chatter and goes away with more feed (whereas the noise from chatter will get worse), the vibration from the cutter entering the work is different from the vibration when it's chattering, and so on. For me, higher speeds = less chatter and vibration, plus nicer looking chips. A lot of it is just "suck it and see"

[PStechPaul]

One more thing. When I looked more closely at the mill and holder, I saw that it is a double end mill and thus it sticks out further than it should, and the set screw does not seat in the notch. So I'll see if I have a single ended mill, and also maybe try a two-flute type. Other advice I have gotten:

1. Avoid purchasing HF tools and tooling (mills and lathe bits) - instead try Craig's list, eBay, and tool shows
2. Disassemble the machine and carefully inspect for poor fit, cheap fasteners, and other problems that can be corrected (or at least recognized as the culprit)
3. Always make sure the unused axis is tightened securely
4. Collets will help reduce overhang and flexing (and they are not expensive)
5. Try different SFM, RPM, and feed rates, and sometimes "pushing" the tool works better
6. Use safety measures, such as:
(a) Use chip brushes and not rags
(b) Use pliers and not fingers to remove swarf,
(c) Don't use gloves or wear loose clothing or have camera straps, etc, dangling
(d) Always wear safety glasses, and ear protection in some cases
(e) (reminder to self) Use a tripod when taking video

Perhaps there should be a "sticky" thread with this and other advice on safety, techniques, and problems with cheap machines and tooling.

[becksmachine]

Any idea of the underlying theory as to why 2 flutes chatter less?

Approximately 1/2 as much "area" engaged with the workpiece.

One more thing. When I looked more closely at the mill and holder, I saw that it is a double end mill and thus it sticks out further than it should, and the set screw does not seat in the notch. So I'll see if I have a single ended mill, and also maybe try a two-flute type. Other advice I have gotten:

4. Collets will help reduce overhang and flexing (and they are not expensive)
5. Try different SFM, RPM, and feed rates, and sometimes "pushing" the tool works better

Yes, yes and yes!

Dave

[J Tiers]

I don't know that collets will be a huge help.... They may be, or not.

A weldon holder is SOLID... deep hold on the shank (several diameters), secured by a screw but already a close fit, not loose. A collet generally has a far less deep hold, often barely a diameter, and is held only by the radial force from pulling in the collet and hoping it slides down the taper with a good inward force vector due to the slope.

Yes, the weldon sticks out. if quill is loose, that's an issue.

1) agree, the cutter is dull as ditchwater. The chip isn't helping either. Maybe that dullness is from "idling in the cut", as I saw apparently happen in the video. The cutter should be fed, or backed out, but never idled in the cut so that it just rubs.

2) I'd be willing to bet that quill is a bit loose. That won't be helped by added length of a holder, but that is the fault of the machine and NOT the holder. Loose quill WILL give you chatter.

3) How do you know you have chatter? I really didn't hear chatter, although the audio system isn't great at chatter frequencies. The scalloped cut is typical of milling, although not always that visible, and not at the snail-like feeds I saw. So maybe ther is some chatter.

4) Going slow doesn't have to be bad, although I DO think that 100SFM for general "machine steel" (1020) is a good aim.

5) Feed, feed, feed. I wasn't seeing much of what I expected, which is CHIPS. Therefore the feed was probably way too slow.

You should feed fast enough to get 0.001 to 0.003" of cut per tooth. Every tooth, all the time.

So at 400 rpm, with a 4 flute end mill, there are 1600 "edges per minute". Using 0.001" cut per tooth, that is 1.6" per minute feed, and I don't think you were getting that. A more reasonable feed is 0.002" per tooth, which is 3.2 inches per minute, and I really doubt that was approached. You would need to feed a half inch per 10 seconds to be there.

if you do NOT feed at a reasonable rate, all you do is RUB, and that will just rub the edge off the cutter. That looks to have been already done, that cutter won't "dust off" any half thou, it probably needs some force to get any sort of chip,

6) Discover the "roughing cutter". These have serrated cutting edges, and cut like crazy. In mild steel, using a 3/8" cutter, 5/16" deep in the material, I can cut about as fast as I want to crank the handle, using a mill with a 1/4 HP motor.

But you are going to have to decide to crank on the handles..... roughing cutters want feed.

7) did I mention increasing the FEED?