Indexable drilling on Turning Centre/VMC

NarulaMech · Aug 9, 2018

Hi,
I am a small business owner in India, new to this forum, with no background education in machining/mechanical engg. Just plain 4 yrs of experience in manufacturing automobile parts (machining + fabrication).

I am using several indexable drills (we call them U-drills) of various sizes (17mm-22mm) on Turning centre/VMC. On Mild Steel and EN8(carbon steel, C-0.4 to 0.5) material. Maximum feed I have been able to achieve is 80-130mm/min, using RPMs of ranging from 1000 to 2100 and feeds of 0.05 to 0.08 max.

I have tried using Sandvik, Tungalow, Taegutec brands of tool holders and inserts, who all claim to be able to maintain feeds upto 0.15mm, but practically are not being achieved in my shop. Why this gap.

The only drawback of my machines is that they do not have provision for through coolant. Can this drawback be the cause of such drastic differences from what companies claim and what I can achieve.

litlerob1 · Aug 9, 2018

I might know what you are asking. But I/we need to know what a "Turning centre/VMC" is. A Turning centre is acceptably a Lathe (most commonly Horizontal) and VMC is an acronym for Vertical Machining Centre, sooo basically different Animals. If we are talking a VTL (Vertical Lathe) that's okay, just need some clarification.

Robert

wmpy · Aug 9, 2018

I would say that your lack of through coolant is the problem. Indexable drills can work with only external flood coolant, but they can't go very deep before you encounter problems. What is the drilling depth, and what problems do you encounter that keep you from achieving the recommended feed rate?

Kaszub · Aug 9, 2018

One times dia no need for thru tool coolant but as you go deeper every psi helps

NarulaMech · Aug 9, 2018

Drilling depth maximum i have is L/D=2.
Well when i increase the feed rate, there is definitely vibration and noise, and i know if i don't reduce the feed immediately, the drill would probably break/wear off within 8-10 seconds.

NarulaMech · Aug 9, 2018

litlerob1 said:
I might know what you are asking. But I/we need to know what a "Turning centre/VMC" is. A Turning centre is acceptably a Lathe (most commonly Horizontal) and VMC is an acronym for Vertical Machining Centre, sooo basically different Animals. If we are talking a VTL (Vertical Lathe) that's okay, just need some clarification.

Robert

I meant both actually. Be it a lathe (horizontal) or a VMC (vertical milling), results i can achieve are similar (probably worse on a lathe, as gravity doesn't help here with coolant).

NAST555 · Aug 10, 2018

From my experience sometimes a U drill does sound a bit "wrong" when it is feeding properly.
What I have found is sometimes running the RPM on the lower side and bumping the feed a bit helps because of chatter reasons. Those drills HATE vibrations, as you pointed out, so on the lower side of the RPM's it helps to reduce chatter a bit.

On EN8 you should be getting nice and consistent results. It is a beautiful material to machine. On your mild steel situation (EN1? EN3?) you could pick up a few problems with inconsistency with chip control, it your problem mainly there?
Are you getting consistent tool life? Also how are you holding these drills? Side lock/Collet? Are your parts clamped nice and rigid? Are they mainly through holes?

0.05 is probably a bit on the low side for the tool reps but what I have found is sometimes they don't really have machining experience and just blabber out the numbers to you that is given to them without taking your actual setup (work holding, machine, coolant etc etc) into consideration. I got burnt this way with Widia drills on a crappy 300WA flange part. Had loads of them to do, 12 off 18mm holes per part, and thought a U drill would be the best way to go. Set it up with the conservative side of the reps numbers and blew a drill up on the third part. Phoned him and told him to come look. He brought the same drill with and said I was feeding too low. My part was raised off the table with 4 parallels and two clamps because of the through holes so I asked him if my setup was correct and he said it was more than rigid enough. I ran it with him next to me and blew another one up on the first part with my hand on feed hold to try catch it because his numbers seemed ridiculous after what I had explained to him happened with the first drill. He nearly crapped his pants and he left with both drills to send to Germany to be "tested". I never got feedback but thankfully I never paid for the drills or inserts. I suspect it was the horrible inconsistent material but he did not want to hear me out. I eventually plugged away with a HSS drill just to get them done.

I think quite a few guys swear by Sandvik indexable drills but I have found that on the depth you are speaking about that all bigger brands should work fine. I don't like indexable drills because of the costs involved when it blows up but use them every now and again.

on edit: Fantasic first post. Well written and explained.

doug8cat · Aug 10, 2018

On my VMC through coolant with a 1.125" indexable drill is awesome I a can rip through 1" plate all day with great insert life.

NarulaMech · Aug 10, 2018

doug8cat said:
On my VMC through coolant with a 1.125" indexable drill is awesome I a can rip through 1" plate all day with great insert life.

I'm not saying I don't have great insert life. I just feel like I'm missing out somewhere, which can increase my feedrate.
Btw, what feed & RPM do you use for your 1.125" drill.

NarulaMech · Aug 10, 2018

NAST555 said:
From my experience sometimes a U drill does sound a bit "wrong" when it is feeding properly.
What I have found is sometimes running the RPM on the lower side and bumping the feed a bit helps because of chatter reasons. Those drills HATE vibrations, as you pointed out, so on the lower side of the RPM's it helps to reduce chatter a bit.

On EN8 you should be getting nice and consistent results. It is a beautiful material to machine. On your mild steel situation (EN1? EN3?) you could pick up a few problems with inconsistency with chip control, it your problem mainly there?
Are you getting consistent tool life? Also how are you holding these drills? Side lock/Collet? Are your parts clamped nice and rigid? Are they mainly through holes?

0.05 is probably a bit on the low side for the tool reps but what I have found is sometimes they don't really have machining experience and just blabber out the numbers to you that is given to them without taking your actual setup (work holding, machine, coolant etc etc) into consideration. I got burnt this way with Widia drills on a crappy 300WA flange part. Had loads of them to do, 12 off 18mm holes per part, and thought a U drill would be the best way to go. Set it up with the conservative side of the reps numbers and blew a drill up on the third part. Phoned him and told him to come look. He brought the same drill with and said I was feeding too low. My part was raised off the table with 4 parallels and two clamps because of the through holes so I asked him if my setup was correct and he said it was more than rigid enough. I ran it with him next to me and blew another one up on the first part with my hand on feed hold to try catch it because his numbers seemed ridiculous after what I had explained to him happened with the first drill. He nearly crapped his pants and he left with both drills to send to Germany to be "tested". I never got feedback but thankfully I never paid for the drills or inserts. I suspect it was the horrible inconsistent material but he did not want to hear me out. I eventually plugged away with a HSS drill just to get them done.

I think quite a few guys swear by Sandvik indexable drills but I have found that on the depth you are speaking about that all bigger brands should work fine. I don't like indexable drills because of the costs involved when it blows up but use them every now and again.

on edit: Fantasic first post. Well written and explained.

I have all proper fixtures to hold my components tightly (all my parts have through holes), no issue on that part. I use collets for most of my drills.
Another issue for me is chip control. I get long unwanted chips which once a while get stuck to the drill, then the operator has to pause before the next drill begins, and remove the scrap. Every single person whom I've asked for guidance, says "increase feed-rate to reduce the time of contact between insert and base material, which will make smaller chips and increase edge life". But I'm left confused by these words. Every time I try increase feed, the VMC vibrates, load increases to 15-20% (above 25% something usually breaks I think). Heck I've even tried to bear the vibration once, and the tool wore out after 5-6 drills.

Although I've accepted in my mind that I cannot reach higher production speeds, I still feel I'm missing out on something.

litlerob1 · Aug 10, 2018

Can't you plumb coolant to the Drill on the Lathe?

NarulaMech · Aug 10, 2018

litlerob1 said:
Can't you plumb coolant to the Drill on the Lathe?

Yes. I've precisely done that.

If you were given a task to drill dia 17 (depth 16, material EN8) with a u-drill on a lathe or a VMC, what parameters would to your mind.

What I am achieving practically is 2000RPM, feed=0.065, making it a max 130mm/min. Above that insert life starts deteriorating, tool vibrates sometimes. So I'm steady at this speed.

I just want to know, if this is the max I can go.

Kaszub · Aug 10, 2018

NarulaMech said:
Yes. I've precisely done that.

If you were given a task to drill dia 17 (depth 16, material EN8) with a u-drill on a lathe or a VMC, what parameters would to your mind.

What I am achieving practically is 2000RPM, feed=0.065, making it a max 130mm/min. Above that insert life starts deteriorating, tool vibrates sometimes. So I'm steady at this speed.

I just want to know, if this is the max I can go.

Right there you pretty much answering your own question. I like to set it and forget it. You start pushing to save few cents at the end will cost you more in broken tools.

Philabuster · Aug 10, 2018

NarulaMech said:
(all my parts have through holes), no issue on that part.

Just for clarification, do your parts have holes already in them before you start drilling or are you drilling into solid material?

wmpy · Aug 10, 2018

Your parameters seem fine, though conservative. If I was setting this for the first time, I would start with 2800 rpm and a feed of .076 mm/rev.

On the lathe a misalignment of the tool could cause problems. An easy way to check this is to make sure that the drill is cutting to size. A little big is usually ok, but you don't want it cutting undersize.

If you're not using through coolant, I would watch the tool very carefully to make sure that the chips are coming out nicely. If the chips aren't evacuating, that can cause the higher spindle loads you are seeing.

Your use of collets to hold these drills would make me a little nervous. I always use a bushing with screws locking on the flats. Maybe it's ok to hold with a collet, but I wouldn't do it.

For your vibration problem, that could be a machine issue. Can you provide the machine make and model?

Jashley73 · Aug 10, 2018

At 17mm, I'd be using a replaceable-tip drill, not an indexable/U-drill. Although most indexable drills will go down to 15mm, I don't think it's wise to do that unless it's a seriously strange application.

At 25mm and larger, the indexable drills make a lot of sense.

I think you're not using enough feed. A 25mm drill in low-carbon steel should be feeding around .075-.125mm/rev. Too light of feed, and you won't break the chips.

If you have a 40-taper milling-machine, you may not be able to use indexable drills much larger than 25mm. Simply put, the machine may not be rigid enough. One reason for this, is that indexable drills have a radial-imbalance since they have two dis-similar inserts. As such, a 32mm indexable drill may be too much for a 40-taper machine. To make this worse, often these drills are held in a Weldon/set-screw toolholders, which usually add somewhere between 75-100mm in extra gage-length. This makes the tool WAY less rigid, and makes rigidity issues much worse.

If you have a 40-taper machine, and are struggling with rigidity on larger diameter indexable drills, then consider an alternative method for making holes. Perhaps a replaceable-tip would be a better choice, since they are radially balanced, and will be more stable on weaker machines.

If you are having trouble with these drills on your CNC lathe, then you need to make sure that your machine is properly aligned. If the drill is not parallel to the machines ways & spindle, or if it is off-center in the Y-axis (above/below center) then you will have problems with these drills regardless of speed & feed.

Search

Largest Manufacturing Technology Community on the Web

Search

Indexable drilling on Turning Centre/VMC

NarulaMech

Plastic

litlerob1

Diamond

wmpy

Hot Rolled

Kaszub

Hot Rolled

NarulaMech

Plastic

NarulaMech

Plastic

NAST555

Stainless

doug8cat

Titanium

NarulaMech

Plastic

NarulaMech

Plastic

litlerob1

Diamond

NarulaMech

Plastic

Kaszub

Hot Rolled

Philabuster

Diamond

wmpy

Hot Rolled

Jashley73

Titanium

Similar threads