[smittys800]

Hey Gang,
Been tinkering with Carbide endmills VS HSS. Now I am not the best in figuring speeds and feeds, go with what is working at the time. Got schooled today, was told to quit wimping out and let er RUN. So I bumped my feeds to 40 IPM ( From the low 20's )in Aluminum, 2 flute HSS Endmill. Cuts fine. Swap out to a Carbide, 2 flute, and chatters like crazy. Both endmills are in a Endmill holder, no collet, RPM at 6k, feed the same, 40IPM.
What am I missing, or doing wrong most likely.
Thanks for your time,
Smitty

[davereagan]

Carbide is more rigid than HSS. My guess is that the helix angle of the flutes on the carbide endmill is lower (closer to straight). High helix endmills made specifically for aluminum can cut several times deeper and with higher chiploads compared to 30 degree standard helix endmills. Aluminum cutting endmills also have sharper rakes that could not hold up on harder materials but cut with less force. A lot of people on here don't know how much better high helix endmills are for cutting almost any material with less chatter and better finish. I first discovered this with aluminum but then used them on mild steel. The clue is that they sell high helix endmills for hardened steels and aluminum. Well, why would they work better for mild steel in the middle of the hardness/ductility spectrum? The answer is they do. If you need a recommendation, write back to me or try www.garrtool.com They havesome awesome endmills for a wide variety of materials and recently introduced a line specifically for aluminum.

Dave

[toastydeath]

What depth of cut? The endmill holder isn't doing you any favors up at 6k rpm, and is probably one of the factors contributing to the carbide chatter. You really should be using a collet chuck at that speed for a whole variety of reasons.

If I recall properly, while carbide has a higher static stiffness than HSS and deflects less, it does have a lower dynamic stiffness than HSS and is thus prone to chatter as a result when used in something like an endmill holder. Endmill holders, by themselves, increase chatter.

You might try reducing your depth of cut on the carbide, and increasing the feedrate somewhere between 60-80 ipm @ 6k rpm. That will put the per-tooth chipload of a 2 flute EM up to .005"-.007" per tooth, rather than .0033" (where it is right now). Both the increased feed rate and the decreased depth of cut reduce chatter. So you might be able to increase your volumetric per time removal rate by doing both.

[Donkey Hotey]

Smitty,

You're doing this on your Toolroom Mill, right? The rigidity of the machine will start playing into this at some point.

While I agree all that has been posted so far, that machine may also require some unique allowances for how aggressive you feed it.

Thanks for the tips guys. I'm getting a better understanding of the cutter geometries and materials too. Keep it coming.

[dertsap]

What am I missing, or doing wrong most likely.
Thanks for your time,
Smitty

it's impossible to come to any kind of assumption as to what the problem is without any information as to what you are trying to make the tool do .

one thing i will point out is , unless the solid holder is of poor quality i would rule out that being the problem ,#1 reason for that being is they are far more rigid than any collet holder , i work with a lot of nasty stuff at high speeds or at heavy loads when chatter become a problem the tool gets mounted in a solid holder period ,and the shorter the better . but if it's piss poor quality then forget it , same thing goes for cheap collet holders.

you need to tell us the depth of cut ,engagement , tool stickout , what the part is being fixtured in (how solid), what is the wall thickness if pocketing etc in order to get a truely educated guess as to what the problem may be .
there are so many factors that will contribute to tool chatter

a simple trick of mine with chattering endmills is to ever so slightly run a stone along the sharp edge of the endmill ,just enough to lighten the edge some ,works like a charm , sharp isn t necessarily always a good thing

[dertsap]

first test you sould do is dial the tool for run out , if you've got runout then remove the tool and check the holder to see if its the tool or the holder

[smittys800]

Great info!!
Series of Depths of cut .1, total of 4
Doing a contour cut along the outside edge
Aprox 1.25 tool stick out
Part is mounted flat on a fixture plate with 2 bolts mounted in the center of the part.
I am using Mari Tool holders
And yes, This is on the TM-1
I think that covers it,
Thanks again,
Smitty
SMitty
Will give it another whirl today

[Geof]

Just to add to dertsap's coments: Do you have several holders? Try switching to a different one. We have found a difference even between holders from the same maker; one will chatter another will not. Also if the holder is getting a bit old and has had several tools broken in it forget using it; it is probably bell-mouther and will not hold firm.

[PBMW]

Smitty
We talked in my shop westerday. You have enough HP to run your half inch carbide endmill full depth on your alum parts. 6K rpm and at least 70 IPM
Get some coolant on it. Use three flute endmills like we talked about to be able to get the feed rate up. I cut alum at 1500 sfm all the time.
You won't know how fast you can go untill you break an endmill or two.
Turn it up!!!

[smittys800]

Yea,
Figured it was time you got in on this!! :stickpoke
I will get some of them there 3 fluters and shift into high gear I guess, at least I went from 24IPM to 50 IPM!! Huge leap for mankind and ME!!!
Thanks again,
Smitty

[VWSatOz]

I always found it works best if only ONE flute is in side contact with the work, 2flutes touching gives twice the deflection & chatter, shallow cut & slow spiral so only one flute is scraping up is the trick & don't bump into corners of a pocket... radius path around them with CNC

[Donkey Hotey]

This'll be interesting to see what your results are. We have a TM-2 at work and I've heard complaints about stalling the spindle and rigidity problems compared to a machining center.

[VWSatOz]

never heard of TM-2.... I guess its a baby compared to a machining centre
With ally I used to run a 16mm cutter at 6000rpm &just feed it until depth by width by feedrate of cut gave same max. mm3 of chip volume per minute, heaps of coolant & woof! amazing metal removal rate, provided the carbide flutes were open & polished to let the coolant in and the gooey ally not weld up on the ramp-in plunge prior to start of cut. Great fun.... but that was years ago, my mc only has max feed of 4meters/min

[Geof]

....We have a TM-2 at work and I've heard complaints about stalling the spindle....

Just as a side comment: Use AUTOFEED for Setting #84 TOOL OVERLOAD ACTION and set the max spindle load at something like 120%. This way it is not likely you will stall the spindle because the feed backs down to keep the spindle load around 120%.

[Donkey Hotey]

Yup, that's why I keep bringing up the fact that he has a Toolroom mill: it's a great machine and very versatile but rigid and powerful are not part of its mission.
http://www.haascnc.com/details_VMC_NEW.asp?ID=179

So recommendations that would apply to a really rigid spindle and heavy bed casting won't necessarily work on the TM-series. They might, they might not.

The guys I know who use the TM-2 look at me like I'm crazy when I tell them the speeds and feeds I run in my VF-2.

For aluminum, I run carbide, 0.5" or smaller at 10K RPM and 0.002" chip load. That's 80 IPM at 10K RPM (4 flute--yeah, yeah, I know--'chip clearance'). I don't use more than 1/3D for depth and try to keep the face engagement under 1/3 as well.

The guys running the TM-2 rarely run the spindle above 3K, cut the same 0.002" chip load and use two-flute end mills. That's 12 IPM in the same material. Above that and they say that the head and table start chattering.

I don't think they've done much experimenting (they don't have the time) so there may be a lot of room for improvement. I'm just saying that the final performance numbers may still be less than other experience would suggest.

[Geof]

....For aluminum, I run carbide, 0.5" or smaller at 10K RPM and 0.002" chip load. That's 80 IPM at 10K RPM (4 flute--yeah, yeah, I know--'chip clearance'). I don't use more than 1/3D for depth and try to keep the face engagement under 1/3 as well....

For roughing when you are not worried about a good finish go to a high helix two flute and you can push it to 120ipm at 10k with a 0.40"doc and full diameter engagement. Just make sure the flood coolant is really flood.

[smittys800]

WELL!!!!
So, swapped out some endmills into a collet and an Endmill holder, started my warm up with carbide in the collet holder. I had to look twice, the endmill looks to be bent?!!! So I put the only other Carbide I had in, and same thing. Man, I have a bent Holder. So I put in a new HSS in the Collet, and spins true. Now mind you, this is all by my Precision Eyeball!!!
So I rolled both endmills on my Vice top, since this is a top-o-the line Chop,
and both are bent at the shank!
Gee, do ya think that might cause some issues?
Hey, but this is all a learnin curve, and I thank all of you for taking the time to shed some light on the subject.
One another note, Donkey Hotey, when I ran my parts last night with my 2 Flute HSS endmill at 50IPM, I was concerned about BASE vibration and Ridigity, but it cut it just fine, with a nice finsh as well. Sure was a spittin those chips out. Might pass that on to your Friends, the TM-1 will handle it.
Merry X-maxs everybody!!!
Smitty

[PBMW]

You have a bent carbide endmill??????????
Never seen anything like that is 40 years. Carbide will break long before it will bend.


Oh...I run half inch endmills on my 6k mini at 6k rpm and about 100 ipm with a three flute for roughing in alum. Bout .375 deep. Works just fine. You can tell when it's cutting...

[dertsap]

are you sure the holders are not the problem ,or a chip in the taper ?
a poor quality endmill will most likely run out on the flutes , but you say this is at the shank ?

[smittys800]

Well,
I think it's bent. When I roll it on the Vise top, you can see how it rolls with a wobble. Then did the same with a HSS and no wobble with the roll. If it can go wrong, you will find me close by!!
Smitty