New to insert drills-Chatter

ManualEd · Sep 28, 2015

I've got another stumper.
Lathe is a 96 SQT15MS.
I had to wrap some .002 shim stock around the shank to get a nice tight fit in the boring bar holder.

First time using insert drills, (well, second time) and I'm having some chatter problems.

17mm Corodrill 880 ran incredibly in my live tool block. 2200RPM .002/rev, I couldn't even hear the thing cutting.

Now I'm trying to dial in a 2" 3xD Ingersol Quad twist 1.5" shank in a solid boring bar holder.

Recommended speeds/feeds for low-alloy (2.9375 1045 precision ground) steel is 450-800 SFM and .004-.0095/rev.

At 400 sfm and .004/rev (all the way to 450sfm/.008/rev)this is what it ends up looking like.

Heres Ingersol's site http://www.ingersoll-imc.com/en/products/NEW-132-2_Quad-Twist.pdf

The inner insert has one part of the cutting edge that is supposed to contact first and help centre the drill, but it seems like thats pushing the drill off centre, then on retract it cuts those grooves to the 2".
It currently drills 1.970", offsetting in X helps cut to size, but still leaves those grooves due to spring back on the retract.

Any tips? More speed maybe? Or program the first .200" at .001/rev?

Thanks,

Ed.

Captdave · Sep 28, 2015

I would put a piece off drill rod in the holder and run your DTI down the length to insure it isn't cocked at an angle then sweep the bore of the tool holder to insure its cutting on X0,. My limited experience with VDI tool holders hasn't been the best and sometimes they need a little more tweaking then just bolt on and go.

Good Luck

ManualEd · Sep 28, 2015

Captdave said:
I would put a piece off drill rod in the holder and run your DTI down the length to insure it isn't cocked at an angle then sweep the bore of the tool holder to insure its cutting on X0,. My limited experience with VDI tool holders hasn't been the best and sometimes they need a little more tweaking then just bolt on and go.

Good Luck

Thanks Cap.
Holder is on centre, and it's holding the drill and a test bar to about .002 over 6".
Also tried programming it .200 deep at .001/ rev and I got the same grooves on retract.

Blake1978j · Sep 28, 2015

It's been my experience that recommended sfm and chip loads often exaggerate what the tool can actually perform well at. As a rule I will figure to the low side of their range, then take 80% of that calculation to start. More chip load, if all is ridged, should eliminate the vibration.... I agree with aaront, don't believe I would turn this size of drill, if it can be avoided. Good luck

ManualEd · Sep 28, 2015

AARONT said:
Take it out of the live tool holder. Put it in a solid tool block and use the spindle. I wouldn't be trying to spin a drill that size in your live tool holders.

Oh geez, this thing is in a solid boring bar holder. It was a 17mm drill in the live tool holder.

Blake1978j · Sep 28, 2015

Sorry, didn't read carefully! It really does sound like a rigidity issue, maybe the shim is causing issues. If you could make a block that fits it well... Possibly open one that is close up a little, I think it may be worth the time

Captdave · Sep 28, 2015

AARONT said:
Take it out of the live tool holder. Put it in a solid tool block and use the spindle. I wouldn't be trying to spin a drill that size in your live tool holders.

Dont tell me I have to run out and buy several sets of ER 64 collets.

AARONT · Sep 28, 2015

ManualEd said:
Oh geez, this thing is in a solid boring bar holder. It was a 17mm drill in the live tool holder.

Damn. It's only Monday and I can't even pass reading comprehension. :willy_nilly:

gregormarwick · Sep 28, 2015

It's the holder.

When you're working with bigger insert drills like that in a lathe then secure clamping of the shank is everything. The fact that you're shimming it tells all. Tighten the clamping screws, compress the shims, not enough contact on the shank.

You need a holder that's a tight sliding fit on the shank to start with. I work a lot with insert drills in the lathe 50-100mm range. Often I'll loctite the drill in the holder, even when it's a tight fit to begin with. It makes the difference between squealing and not squealing.

ManualEd · Sep 28, 2015

gregormarwick said:
It's the holder.

When you're working with bigger insert drills like that in a lathe then secure clamping of the shank is everything. The fact that you're shimming it tells all. Tighten the clamping screws, compress the shims, not enough contact on the shank.

You need a holder that's a tight sliding fit on the shank to start with. I work a lot with insert drills in the lathe 50-100mm range. Often I'll loctite the drill in the holder, even when it's a tight fit to begin with. It makes the difference between squealing and not squealing.

I think you're right. I put an indicator on the holder, then hand wheel-fed it in, and I saw a .0015 flex, but no vibration. I'll throw some blue loctite around the shank tomorrow and give it a shot.

The back of the drill is threaded for a coolant plug, so I even made an insert that sucked the face of the flange against the toolholder, but no dice.

Krovvax · Sep 28, 2015

Just my 0.02$ use the green one loctite 609 is the small gap for slide fit. Its going to be better than the blue one for thread!

Jashley73 · Sep 29, 2015

ManualEd, experience has taught me that these drills just like to sing. Sometimes you can quiet them down, but seldom will they ever run "noise-free". Personally, I wouldn't get too caught up about the shims under the holder.*

Your picture shows some terrible marks on the ID from retract. Have you measured the hole to see what size the drill is actually cutting? And where's the outboard inserts? Is it facing +X or -X? I always set my drills up with the outboard insert facing X+, make sure the holder is centered, (indicate the holder bore,) and then give it a test run. I drill in maybe 3/4" deep, then measure the bore. Is the hole on size? Then, adjust the X-offset, and try it again.

If you're still getting terrible marks on the ID, try drilling slightly oversize, and then moving back to center before retracting from the hole. Something like...

G0 X.015
G1 Z-2.
U-.015 W.0075
G0 Z1.

* So here recently I've been setting up a job on a brand-new Mazak lathe, and have had an awful time with boring bars squealing like a pig. I tried everything. Loosening a set-screw. Hacking-up the sleeves, making split sleeves, milling flats so that there's 2 "lines" of contact, instead of 1... Nothing worked. Until I pulled the holders off the turret, put electrical tape between the holder and the turret, then reassembled. Just like that, instant fix. Deeper cuts, faster speeds, harder feeds, no chatter... Part of me thinks that between the milled faces on the turret, and the milled faces on the holder, the holder wouldn't sit flat against the turret, and by tightening all 4- bolts to hold the holder on, it was trying to pull the holder out of square/plane. Whatever "it" was, the electrical tape worked...

cnctoolcat · Sep 29, 2015

You have to get the outside insert on the centerline in X+. A properly-set 2" insert drill should drill a hole around .005" of size. You gotta get it drilling the properly-sized hole before anything else.

You do not want to under-size drill down to 1.970", the cutting balance of the drill will be thrown off. I always manually drill (500 rpm, 2" feed maybe) the hole about .100" deep to verify hole size before turning the drill loose in Automatic.

It sounds like to me you've got a centering problem in X, or your drill is too high/low.

Also for larger drills like that just keep slowing down your SFM. I've had to run big drills as low as 100 SFM to make them cut good and fairly quiet. Don't cut the feed back, you need the right IPR to break the chips.

And if all else fails, use a smaller drill and bore the hole out to size.
ToolCat

Jashley73 · Sep 29, 2015

cnctoolcat said:
Also for larger drills like that just keep slowing down your SFM. I've had to run big drills as low as 100 SFM to make them cut good and fairly quiet.

Maybe, but one also has to be cautious of spindle torque. Especially on a 8"-10" chuck sized machine, you've got to stay in the torque curve. Slowing down too much below say, 1100rpm in steel might get you below the peak toruqe curve on a smaller machine. At a previous job, I had a Cincinatti Talon lathe, with an 8" chuck and 15hp? I believe. Using a 2" insert drill in steel, there was a big difference between the spindle loads at 1050 vs. 1300 rpm...

Mtndew · Sep 29, 2015

Carbide indexable drills on a lathe love to make noise, they feed off of it.
But, excessive vibration and chatter are different than just squealing.
As said above, make sure it's on center before anything else.
Then run it at recommended speeds and feeds, you can really push those drills.

ManualEd · Sep 29, 2015

Toolcat, the drill is on center within .001.
I'm not sure whats flexing enough to cause the tips to flex and cut undersize, then spring back to 2.000 on the retract.

I'll spend some more time with a dial on various parts to see where this play is today.

Jashley, the hole is 1.970. Ofsetting in X will get me to 2", but I still have those gouges on retract the same amount.
The outside insert is set up facing X+ so that you could use it for boring.

I took the drill out, put a 2' chunk of IHCP in the holder, set a dial to it, and reefed on it. 230lbs only got .002 of movement, so I don't think (hope) all that movement isn't coming from the turret or rails.

Thanks everyone for the replies. I'll be trying things throughout the day and updating as I go.

HuFlungDung · Sep 29, 2015

The drill design is quite flat on the end. I've always used insert drills that take a W insert, and these cut a decidedly deeper v shaped channel. With the flatter insert profile, I suspect the drill is wobbling around like a square-ended slot drill plunging into a hole on the mill.

Jashley73 · Sep 29, 2015

ManualEd said:
Toolcat, the drill is on center within .001.
I'm not sure whats flexing enough to cause the tips to flex and cut undersize, then spring back to 2.000 on the retract.

I'll spend some more time with a dial on various parts to see where this play is today.

Jashley, the hole is 1.970. Ofsetting in X will get me to 2", but I still have those gouges on retract the same amount.
The outside insert is set up facing X+ so that you could use it for boring.

I took the drill out, put a 2' chunk of IHCP in the holder, set a dial to it, and reefed on it. 230lbs only got .002 of movement, so I don't think (hope) all that movement isn't coming from the turret or rails.

Thanks everyone for the replies. I'll be trying things throughout the day and updating as I go.

(1) I'd offset that drill so that it's drilling 2" diameter. Centering the holder is a good idea for initial setup, but not critical for the actual cutting performance. Centering the holder with an indicator is really only useful for 2 things - Making sure you're turret is radially aligned correctly, (you're not above or below center in the imaginary Y-axis,) and ball-parking that the X-offset is right. Once you start cutting though, you need to move the X-offset around so that the drill is drilling as it should. (On-size.)

(2) 230lbs is nothing compared to the thrust required to push what is essentially a 2" piece of metal through another 2" piece of metal. Lookup how much axis-thrust your machine will generate in the Z-axis. Then watch your Z-axis servo load as you're drilling the hole, and do the math. If you're in a 10-15: chuck size machine, I'd expect it to generate around 1000-2000 lbs of Z-thrust. As the machine is drilling, it's trying to rotate the turret assembly on the X-axis cross-slide base, so it wound't surprise me if you're seeing a little deflection while it's running.

gregormarwick · Sep 29, 2015

HuFlungDung said:
The drill design is quite flat on the end. I've always used insert drills that take a W insert, and these cut a decidedly deeper v shaped channel. With the flatter insert profile, I suspect the drill is wobbling around like a square-ended slot drill plunging into a hole on the mill.

There is always the possibility that it's just a rubbish drill but Ingersoll seem rarely mentioned around here and I know I've never used them so...

There are other drills (Seco for instance) that are very flat on the end that drill fine so I wouldn't jump to that conclusion necessarily.

I'm still betting on how it's held. I kind of doubt loctite is going to make much difference when it's so loose in the holder to start with. Assuming the shank is not undersize on the drill (indexable drills tend to be an h6 on nominal shank size) do you have a better holder to put it in?

Also, pulling the drill into the holder seems like it should help, but did you sweep the face of the holder first to make sure it's square to the spindle? If it's not you could just be forcing the drill off-centre. Worth noting that dedicated drill holders (talking rotating tool now) are ground on the face as well as the bore so that they don't influence the drill centreline under load, unlike most sidelock holders.

DMF_TomB · Sep 29, 2015

ManualEd said:
I've got another stumper.
Lathe is a 96 SQT15MS.
I had to wrap some .002 shim stock around the shank to get a nice tight fit in the boring bar holder.

First time using insert drills, (well, second time) and I'm having some chatter problems.

17mm Corodrill 880 ran incredibly in my live tool block. 2200RPM .002/rev, I couldn't even hear the thing cutting.

Now I'm trying to dial in a 2" 3xD Ingersol Quad twist 1.5" shank in a solid boring bar holder.

Recommended speeds/feeds for low-alloy (2.9375 1045 precision ground) steel is 450-800 SFM and .004-.0095/rev.

At 400 sfm and .004/rev (all the way to 450sfm/.008/rev)this is what it ends up looking like.

View attachment 150398
Heres Ingersol's site http://www.ingersoll-imc.com/en/products/NEW-132-2_Quad-Twist.pdf

The inner insert has one part of the cutting edge that is supposed to contact first and help centre the drill, but it seems like thats pushing the drill off centre, then on retract it cuts those grooves to the 2".
It currently drills 1.970", offsetting in X helps cut to size, but still leaves those grooves due to spring back on the retract.

Any tips? More speed maybe? Or program the first .200" at .001/rev?

Thanks,

Ed.

.
2" dia drill
400 sfpm
.004/rev
1045 steel
maybe 0.6 cubic inches per hp per minute
so
16 hp and about 1300 lbs of force required
,
at 100 sfpm
4 hp and still 1300 lbs of force as feed rate per rev the same but often the noise is less when less hp is needed
.
many machines make noise when high hp is used. usual question is the noise vibration destroying the inserts or causing sudden tool failures

New to insert drills-Chatter

Stainless

Titanium

Stainless

Plastic

Stainless

Plastic

Titanium

Stainless

Diamond

Stainless

Hot Rolled

Titanium

Diamond

Titanium

Diamond

Stainless

Diamond

Titanium

Diamond

Diamond

Similar threads