1" EM Very Loud in Aluminum

[JMFabrications]

So this is the first time I am using a 1" end mill in aluminum. I typically use 3/4" em's if I have a lot of stock to remove because they are cheaper but I figure this time I would go with a 1" to remove more stock in hopes of speeding up the program. The problem I am having is that when it cuts it makes an ungodly high pitched sound that I have never heard before. Just wondering if maybe im trying to remove to much material at once or if that just normal for 1" em's. Here are the specs:

Haas VF2
6061 Aluminum
Niagara 1" 3-flute HSS Roughing EM for ALUM (uncoated)
DOC .5" Slotting
SFM = 450
CHIP = .008
IPM = 41
RPM = 1719
Spindle Load is about 60% (yea im conservative)

Any input as to why the EM is making such a high pitched noise would be greatly appreciated.

Thanks,
Jim

[Rekd]

Sounds like you're not pushing it hard enough. Try either turning down the RPM or turning up the feed rate.

It's impossible to tell you what speed and feed to use because we don't know your setup rigidity and your machine's rigidity and capability. But like I said, squealing (screaming?) is typical of too small of a chip load, so try adjusting the RPM down slowly while it's cutting to see if it gets better.

[Geof]

Originally Posted by JMFabrications .... The problem I am having is that when it cuts it makes an ungodly high pitched sound that I have never heard before...,,Thanks, Jim

That is called chatter; the high pitch indicates that it most likely originating in the cutter not in the machine ways.

Chatter comes about because you have a resonant relationship between the natural vibration frequency of the tool, the rate at which the cutting tips hit the work and the load on the tool.


Natural vibration frequency is related to how rigidly the tool is held and how long the tool is:

How are you holding the cutter? In my experience collet holders are not as rigid as the setscrew holders so if you are using collet switch to the setscrew type. If you don't have setscrew type and have to use collet read on.

Choke the cutter as far up in the holder as possible, the shorter the length sticking out the more rigid.

The rate at which the tips hit the work is related to the rpm:

Maybe back off the rpm, you cannot readily increase it because you are then starting to push the sfm too high maybe.

The load on the tool depends on the feed, chip load per tooth combined with rpm.

Crank up the feed. you can probably go to 0.01" per tooth, maybe even more. Be careful doing this if you are not using flood coolant because you are going to be creating a lot of heat in bigger chips and you may clog the flutes with aluminum on the verge of melting without flood coolant.

You can do the speed and feed changes using the overrides.

It is possible that you will not get any combination that totally eliminates chatter. If you are unable to get much improvement then you get drastic. As the tool gets dull it becomes less prone to chatter; some people suggest stroking the cutting edge with an oilstone just to take off the extremely keen edge. I wince at the idea of deliberately dulling an expensive tool because if that doesn't work you cannot go back to un-dull.

[JMFabrications]

Thanks for the replies! The tool is brand new and is held in a set screw holder. The length of cut on the tool is 1.5" and OAL is 3.75" so its not too long for a 1" EM. The peice I am cutting is 18x5x1 and I am using 2 parlec vises to hold it in place, I am also using flood coolant. Its only the 1" em thats making all the noises, the rest of the program runs very smoothly with smaller tools. Ill try to turn down the RPM or bump up the feed and see if that helps.

Thanks,
Jim

[gsrmmeza]

Try this:

RPM=1390
Feed Rate=12.5

This feed and speed is for high helix roughing endmills.
you can cut 1 diameter deep x 1 diameter wide.

[crashtest]

Hello!
I would try to make 2 passes or add a spring pass that way your not trying take off too much material at once. I haven`t ran any aluminum. Make sure you have coolant on it, I know it will clog up or ball up a drill bit. My company that I work for requires me to take off about 275 thousandths off of regular steel pipe that is 3 1/8 round by 4 ft long and have a decent or acceptable finish. I`m like Hello, nothing to support it in the middle, to long of part, need to make 2 passes taking off smaller amount it will look better. I know! I have altered the program, even though I`m not supposed to, you didn`t here me say that, but at their feed and speed settings it will not cut an inch from the start with out chattering. I think it`s about to come apart it`s so bad. My safety is what I`m thinking. I changed the feed to F 0140 and my Speed to 650 still a fight though. 2ft & 3 ft long piece F 0230 S0850. Hopefully this will help.

[HuFlungDung]

I would check the relief clearance ground on the cutter flutes. You can do this with a sharp point on a dial indicator. With the tool in the spindle (and spindle OFF), set the indicator so that it rests against the OD of the tool. You'll need to set the point against the back of the primary relief on the tool flute, this zone is typically about 1/8" wide on a tool that size. Then, note the dial reading and watch the value increase as you rotate the tool allowing the indicator to ride up the relief angle. Note the maximum just before the indicator drops off the sharp edge.

Now estimate how wide the relief zone is, versus the rise, and calculate the arctangent to get the relief angle. .006" drop in about .1" of circumferential rotation would be almost ideal. If its .010" that's getting to be excessive, and will want to chatter until the tool gets worn in a bit. Dulling the edge is a poor substitute for grinding the correct clearance to begin with, but what are you gonna do? Maybe try a different brand endmill.

[Delw]

Geof has some very god info.

If nothing else works. Take a few big wide rubber bands and wrap them around the tool next to the holder then take a few and wrap them around the holder itself.

The rubber bands will dampen the noise however sometimes you will still get some chatter marks.

one other thing it could also be the part itself chattering from teh pressure on the endmill. like a box that has thin walls we usually rgh them all out then fll them up with machining wax and make a final pass on the edges.
the rubber bands work very well on the outside of the parts also.
the other thing to do is step the endmill up in the z a few thousanths each pass as you will get more chatter when your are touching the bottom

[lkenney]

I would try it at about 1100 RPM at 20 IPM for a .5" doc Should keep you at 60% spindle load. I run on a VF-0 with a two flute at about 15IPM

[toastydeath]

This all assumes you have followed everyone else's advice about setup and how things are held.

You can either run the spindle faster or slower to overcome chatter. There's usually a couple small bands of frequencies (RPM settings) in the high end of the machine's spindle speeds where you can cut .5" deep (or deeper) and not get chatter. Likewise, there are a couple frequencies where, even though everything is buttoned down tightly and all your feed parameters are right, you are sitting on top of one of the natural harmonics of the machine and it's going to chatter no matter what you do.

The other thing that you can manipulate is the depth of cut. The length of tooth engagement (depth of cut) determines the gain of the vibration - by cutting a shallow slot, there is less gain to amplify chatter. The chatter needs a particular amount of gain to develop, so by cutting a shallower channel, you can go under this.

A third, not quite as important item is the chip load. You should be at about .010", as Geof suggested. A smaller aspect ratio between length of engagement and chip width behaves as a damper to vibration (thicker chip, less depth of cut).

[dapoling]

Originally Posted by JMFabrications So this is the first time I am using a 1" end mill in aluminum. I typically use 3/4" em's if I have a lot of stock to remove because they are cheaper but I figure this time I would go with a 1" to remove more stock in hopes of speeding up the program. The problem I am having is that when it cuts it makes an ungodly high pitched sound that I have never heard before. Just wondering if maybe im trying to remove to much material at once or if that just normal for 1" em's. Here are the specs: Haas VF2 6061 Aluminum Niagara 1" 3-flute HSS Roughing EM for ALUM (uncoated) DOC .5" Slotting SFM = 450 CHIP = .008 IPM = 41 RPM = 1719 Spindle Load is about 60% (yea im conservative) Any input as to why the EM is making such a high pitched noise would be greatly appreciated. Thanks, Jim

Since your load meter is already at 60% decreasing your rpm will only increase pressure.

I would reduce the depth of cuts to .1 or .2 and then increase your rpm and feed rates.
I would go with carbide if you can.
Shorten you tool holder and length to minimum as mentioned above.

I would suggest following with good coolant flooding.
RPM: S5000 to start
FEED:
2 Flute 30 ipm to start
3 flute 45 ipm to start
Depth of Cut .1 to start

A general rule of thumb, if possible cut no more the 2/3 width of cutter and or to a depth of 1/3 dia of cutter, otherwise adjustments will be required in feed and speed.

If you want to keep your depth of cut, shorten tool holder and length and then reduce rpm and feed to get rid of the harmonics.