Insert Drill in Aluminum Speed and Feed ideas

Dupa3872 · Mar 2, 2018

Guys,

I run these parts and parts similar quite often in our HAAS SL-20 lathe. I am using a Sandvik 1.00 coolant thru drill (no High pressure)
I am going 2.10 deep to a flat bottom. The drill is fairly new and inserts are changed as needed.

I want to go as fast as possible but don't want trouble it's 200 piece run. Over the years we get good runs and bad runs using the same program, the drill loads up or will push the part back in the collet (I'm using a W/S S-20 collet Pad nose) and we slow it down it's a pain in the ass at times and I want better consistent cycle time and good parts.

This hole finishes at 1.125 X 2.1 deep. I am drilling with the insert drill then using it to bring my bore within .010-.015 and my last move is in X to center once I reach bottom, Like facing it, leaving .005-.01 on the bottom for the finish tool.

I just want to see speed and feed opinions. And if someone has a better tool in mind say so, remember it's a flat bottom hole.

What about taking out the middle with a drill ? Ive always heard you should not Pre-drill before an insert drill.

Thanks Guys !

Make Chips Boys !

Ron

litlerob1 · Mar 2, 2018

Don't pilot drill.If you ran 5000 RPM you'd be doing fine.

You problem sounds like a material source though.

R

Dupa3872 · Mar 2, 2018

litlerob1 said:
Don't pilot drill.If you ran 5000 RPM you'd be doing fine.

You problem sounds like a material source though.

R

I could not imagine doing 5000 was that a typo ? I hardly have ever pushed this machine past 2500 RPM, Yes I thought about material but we buy only domestic for this customer.

Matt@RFR · Mar 2, 2018

Dupa3872 said:
I could not imagine doing 5000 was that a typo ?

What's wrong with 5000 RPM? That's only 1300 SFM.

I hardly have ever pushed this machine past 2500 RPM

Why? You said you want to speed up your process.

Yes I thought about material but we buy only domestic for this customer.

You will still see inconsistencies from batch to batch, no matter where it came from. Material inconsistencies is a lot more likely than insert inconsistencies in my experience. The only other real player would be coolant.

litlerob1 · Mar 2, 2018

Dupa3872 said:
I could not imagine doing 5000 was that a typo ? I hardly have ever pushed this machine past 2500 RPM, Yes I thought about material but we buy only domestic for this customer.

SL 20 with a collet, yeah. If you want to back it off of Max. do 4750. That's what they're made for not half.
R

Mtndew · Mar 2, 2018

It's aluminum, go as fast as the machine will allow.
Unless it's a crappy 0 temper or 2000 series gummy crap.

Mud · Mar 2, 2018

Yes speed it up. We drill 7/8 in aluminum at 10K in a VMC. Why 10K rpm? Because we don't have more.

Larry Dickman · Mar 2, 2018

We run a 1-1/8 insert drill, 5" deep in 6061 at 9500 rpm and 150 ipm. Never a problem. (Never Chinese material either)

gregormarwick · Mar 2, 2018

In most cases you need to use a significantly lower feedrate to get an insert drill to work in aluminium, this is especially true in a lathe, IME.

All else being equal you will just get strings if you use your "usual" feedrate. Start at half the feed per rev you'd use in steel and it will usually start to break chips somewhere around there.

brian.pallas · Mar 2, 2018

I'd probably just use a regular drill and then go in an endmill to make the flat bottom. Follow up with a bar for the dia and depth. Sometimes we would use just an endmill. No drill and no boring bar. In aluminum.

Ran tons of parts in aluminum on lathes like that. But, also our situation was we wanted lightly tended or unattended machining so hauling ass to save 30 sec or a minute wasn't worth it for us.

One of my main mantras "slow is fast". Doors stay closed, and no problems, everything just runs.

Those Sandvik 880 drills bever did all that well in my opinion. Too many failures, they could be unpredictable. I remember asking the Sandvik repabout boring with one. He just rolled his eyes and said "I wish they hadn't put that in the catalog" lol. Yes, you can bore with them, however....it's still a drill.

And me, personally, a 1.125 hole, what is the stock size? I dont want to be anywhere near a 2" bar spinning at 5k. No thanks for me.

Also, your drills should always have a collar and that should be pushed against the solid face of a boring bar holder. Pushing drills back is no bueno.

gregormarwick · Mar 2, 2018

brian.pallas said:
Those Sandvik 880 drills bever did all that well in my opinion.

I'm interested to hear why you think that?

My opinion is that the 880 is practically unrivalled even after almost two decades at the top of the pile.

Curious why our experiences have been so different...

Captdave · Mar 2, 2018

We use Kennemetal inserted drills on Mazak SQT15 from 1.0" to 1.75" and run 2,500 rpm (6.0 D 6061 parts) and what ever feed breaks a good chip without pegging the Z thrust.

david n · Mar 2, 2018

gregormarwick said:
In most cases you need to use a significantly lower feedrate to get an insert drill to work in aluminium, this is especially true in a lathe, IME.

And I do the exact opposite...............I bump the feed. Sometimes way up to get the chip to break.........................

As mentioned, crap material can really be a pain................even domestic stuff.
Right now I'm running some Kaiser 2 1/4"Ø 6061. Drillin with a 1 3/8" Ø drill. 3500 rippems and .009 feed. Could up the R's, but I get some vibes as I'm runnin' 4 footers and bar pullin'

Oh...and no push back in the collets here..................FlexC collets are the cat's meow :smoking:

gregormarwick · Mar 2, 2018

david n said:
And I do the exact opposite...............I bump the feed. Sometimes way up to get the chip to break.........................

That's always the first thing that comes to mind for sure with aluminium - for whatever reason with insert drills I've just never had much luck with that. Maybe I haven't ever been aggressive enough...

david n · Mar 2, 2018

gregormarwick said:
That's always the first thing that comes to mind for sure with aluminium - for whatever reason with insert drills I've just never had much luck with that. Maybe I haven't ever been aggressive enough...

There is a threshold that needs to get crossed...................keep pushing it until the chip breaks and the Z thrust/spindle loads are at acceptable levels.................

litlerob1 · Mar 2, 2018

OP I wouldn't worry too much about feed for now. Run .006" per rev. (that's 30 IPM). But that hole with the second boring pass is literally a 5 second hole. Not counting tool change and rapid, but from start cut to rapid away is 5 full seconds, maybe 7 depending on how you control the spindle speed, and assuming rapids are 100%.

Is that fast enough?

Also you say "Aluminum", but do you get the exact same temper and grade each time? In your first post you say that you run well sometimes, then it sort of chinks up. There is no reason for that, if you are getting the same thing from the same *reputed supplier.

* there are several reputed suppliers and some of them sell trash-----if you buy it. You can't get away with that in a more strict environment.

R

Bill3D · Mar 2, 2018

Sandvik has all the possible feed and speed data you could want as well as various insert materials. You pair those up and the 880 should be scary fast and the tool and spindle won't break a sweat. Their values always seem good to me so you shouldn't need to guess what the max is. I usually machine steel, not aluminum though. Running the max in steel sounds like a gun range and I dial it back because it's rough on the door glass and I don't want to damage the optical sensor (VMC).

Speedie · Mar 2, 2018

.006 will not break a chip. Run .012+

litlerob1 said:
OP I wouldn't worry too much about feed for now. Run .006" per rev. (that's 30 IPM). But that hole with the second boring pass is literally a 5 second hole. Not counting tool change and rapid, but from start cut to rapid away is 5 full seconds, maybe 7 depending on how you control the spindle speed, and assuming rapids are 100%.

Is that fast enough?

Also you say "Aluminum", but do you get the exact same temper and grade each time? In your first post you say that you run well sometimes, then it sort of chinks up. There is no reason for that, if you are getting the same thing from the same *reputed supplier.

* there are several reputed suppliers and some of them sell trash-----if you buy it. You can't get away with that in a more strict environment.

R

litlerob1 · Mar 2, 2018

Speedie said:
.006 will not break a chip. Run .012+

Probably true, but 2x diameter doesn't really need the chip to break.

R

Guest · Mar 3, 2018

Dupa3872 said:
I could not imagine doing 5000 was that a typo ? I hardly have ever pushed this machine past 2500 RPM, Yes I thought about material but we buy only domestic for this customer.

What type of domestic? Service Center is considered domestic but they are importing ingots from China and mixing it with whatever they recycle, the stuff is garbage.

Insert Drill in Aluminum Speed and Feed ideas

Stainless

Diamond

Stainless

Titanium

Diamond

Diamond

Diamond

Titanium

Diamond

Hot Rolled

Diamond

Titanium

Diamond

Diamond

Diamond

Diamond

Plastic

Stainless

Diamond

Guest

Guest

Similar threads