Not very deep pocket problems

[Cory]

I'm trying to cut an appx 2" square pocket 1.7" deep (it ends up being a through hole, but I'm cutting it as a pocket and flipping it) in 6061 aluminum on a new Haas VF-1. I'm using balanced ER-32 collet chucks with appx 3" gage length. Very conservative DOC. Tried between 0.100 and 0.075. 50% stepover.

It has 1/4" corner radii. I've tried a couple things--

1) Drilling out the corners with a 1/4" drill to avoid leaving a lot of material for the 1/4" EM finishing pass. Using a 1/2" 4 flute Cobalt roughing endmill, appx 2.5" long to rough out the pocket. Tried every speed and feed combination I could think of, all the way from 3000 RPM to 8000 RPM or so. Started feeding at 20 IPM. Sounded absolutely horrible. Even dropping it down to 6-8 IPM gave me unbelievable chatter. the walls of the pocket were gouged so badly that the 1/4" finisher couldn't even save them.

2)Same thing as above. Swapped to a 2 flute HSS TiN High Helix endmill of the same length, in the hopes that it would clear chips/chatter less. Ended up running it at around 5000 rpm and 12 ipm. Still sounds horrible. Leaves terrible surface finish, but the finisher almost cleans it up.

3) Drilled the 4 corners. Drilled out as much of the 'meat' of the pocket as possible. Used a short 1/2" coated carbide endmill to get the first 0.850 cleaned out. The surface finish on this portion of the pocket is beautiful. I was running at around 100 ipm and 85000 rpm.

Next switched to the longer 2 flute HSS endmill to clean out the rest of the pocket. Terrible chatter still, untill I finally dropped the RPM's to about 2000 and the feed to 8 IPM. Not too much chatter, but this seems unbelievably slow. I have to imagine I can machine a pocket this shallow much quicker. Surface finish is ok, but still pretty terrible compared to a good carbide endmill.

Would switching to an extended length solid carbide endmill really improve the rigidity that much to eliminate all the chatter? What else can I try?

Thanks for your help.

[dertsap]

sounds to me your feeding far too slow , i would suck the tool up as far into the holder as you can , if your going 1.7 deep then try to have a stick out of 1.75 max if possible, .05 clearance is a mile , sometimes if a tool is new it may be too sharp , what ive done many times is run a stone ever so slightly across the cutting edge (don t go silly on it ) , many close minded people may disagree with this technic but it was taught to me years ago and it has saved my butt many times

also noise while hogging is no big deal as long as it s not damaging

[Cory]

Originally Posted by dertsap sounds to me your feeding far too slow , i would suck the tool up as far into the holder as you can , if your going 1.7 deep then try to have a stick out of 1.75 max if possible, .05 clearance is a mile , sometimes if a tool is new it may be too sharp , what ive done many times is run a stone ever so slightly across the cutting edge (don t go silly on it ) , many close minded people may disagree with this technic but it was taught to me years ago and it has saved my butt many times also noise while hogging is no big deal as long as it s not damaging

I have the endmill as far in as I can get it without clamping on the flutes.

I had it programmed originally for around 7000 RPM and 40 IPM, and the noise was unbearable.

It wasn't the kind of noise that makes you think your tool is moving some serious metal, it was the "something is going to get ruined if I keep running this" noise. As I mentioned before, there was so much chatter, a 15 thou finishing pass couldn't even clean it up. Even the finishing passes have a ton of chatter.

My only guess is that the total gage length of my cutter and holder is pretty long... 5.5-6 inches. Would it make much of a difference to switch to a carbide endmill for rigidity? How about a 3 flute? Supposedly they're supposed to help with chatter.

[dertsap]

a 3 flt carbide would be ideal

[CarbideBob]

A 3 flute carbide as dertsap recommends will be much stiffer and should run much better than HSS. No mater what you use at 1.7 deep with a 1/4 incher its a slow run. One of those (expensive) variable flute carbide endmills might work well. How about finishing everything but the corners with the 1/2 incher and go in and just clean out the corners with the 1/4 incher?
Bob

[79Jimmy]

I agree a 3 flute carbide would work very well, I've had great results with a line called "Gorilla" mills, the "Silverback" to be specific. I also use Garr 4 flute VHM's which is a great rougher and tends to lessen the load on the spindle. As far as RPM-max it out. How are you entering the pocket? Helical, ramping, plunging.....? How rigid is your setup? Needs to be as rock solid as possible. As far as feed goes, again we tend to be quite aggressive in aluminum 4000mm/m and up for roughing. Like dertsap said the endmill should be only as long as absolutely necessary, 1.75 flute length, 2.0 max and LOTS of coolant! Since this is a small pocket I'd probably rough it and finish with the same 1/2'' tool. I've used Garr 2 flute 242M for this then clean up the corners with a similar 1/4" I usually take a .1mm finish pass (.004"-.005")

[Boots]

One thing you did not mention is how you are clamping up the part. You can't have it sticking out of the vise. If it is make a set of tall jaws and put an indicator on the back jaw when you tighten it up using a Torque wrench. Get the highest preasure you can get short of tilting your part to the back. Sometimes you can get 100 ft. lbs. before it starts to push your part out of sq. Always a rule of thumb on chatter is less flute contact at any given time will produce less chatter. Like someone else mentioned here that honing the edges of a new tool will give you less chatter is "right on". I have shattered new tools before but after honing there was no problem.

[big_mak]

Carbide is the way to go. Der, I've run cutter's backwards before and hit them with some emerycloth(fine). I've only tried it on HSS. This seems to do the trick, especially if your cutter rad is the same as the corner rad.

I'd do as much work with the 1/2" as I could. Then with a relieved 1/4" End Mill, I'd plunge the corners a few times, then just finish the corners to get rid of the cusps left from plunging.

[DareBee]

Get your gauge length as short as possible and CARBIDE CARBIDE CARBIDE. Either a special aluminum coating or TiCn or TiAln. TiCn is best for aluminum but I find tooling suppliers don't stock them at all, TiAln is normal stock.
Variflute will definately help because it breaks up the harmonics.

Tin coating is on the outs, it costs the same money as other coatings and is nowhere near as good.

[JROM]

Try a 3 flute 50 deg helix Garr carbide 1/2 dia.
5000 RPM
70 IPM
look at your setup and make it as stout as you can.
Throw alot of coolent at it. and ramp in your cuts in Z
also don't use less then a 55% stepover or you lose the climb cut advantage.

[Geof]

I don't see where anyone has told you to ditch the ER32 holder and go with a setscrew holder using a carbide two or three flute. I would do the initial roughing using a 5/8 cutter, then 3/8" to take the corners out and finish with the 1/4".

In my experience the collet holders are not as rigid as a setscrew holder and we do a lot of holes from 7/8" dia up to 2" dia and 2" to 2-1/2" deep in 6061.

If you are breaking through, which it sound like you are, it is a good idea to stop just shy of break through and do a clean-up pass, in other words make a flat bottom hole. Then move the cutter in maybe 20 thou from the sides to do the break through. We have found that if you just go straight through the cutter deflection is released as it penetrates so the cutter springs back and digs in along its entire length because it is now cutting material that was missed because of the deflection.

[Boots]

I agree with Geof, solid holders yield better results when chatter is a concern.
You may have to go with an extended holder if your head will not clear. But short always works best with tooling.