drilling/reaming a hole on a lathe

empower · Oct 29, 2019

Hey fellas, trying to drill .213" holes in 7075 aluminum, 1.34" deep. needs to be as straight/concentric as possible/perpendicular to the face.

machine is a yama seiki GLS-2000-LYS. using boring bar blocks with straight shank ER25 holders and dril/reamer held by collets. i indicated the blocks on the turret and they're straight/square but when i indicate the shank of the tool itself, its out about .001" over 1" stroke. is this normal? can it be dialed in better? is it the er collet thats not holding it straight?

desperately need some help figuring it out.

thanks all!

litlerob1 · Oct 29, 2019

Quality of collets is all over the place. So you need good stuff, not economy.

When dealing with them; cleanliness is next to Godliness, the collet nuts, shanks and collets themselves need to be in very good condition. A tiny ding on the ID of any of those components could very easily put it out .001". Dirt, grease, hair, dust, anything at all.

R

empower · Oct 29, 2019

are maritool collets good? i'm using their er holder and collet, brand spanking new

litlerob1 · Oct 29, 2019

Maritool is very good quality. Assuming everything is clean.

We need to know feeds and speeds, size of Drilled hole, coolant, AND what the result of you trying to Ream those holes with that Reamer are....

R

Delw · Oct 29, 2019

empwoer said:
Hey fellas, trying to drill .213" holes in 7075 aluminum, 1.34" deep. needs to be as straight/concentric as possible/perpendicular to the face.

machine is a yama seiki GLS-2000-LYS. using boring bar blocks with straight shank ER25 holders and dril/reamer held by collets. i indicated the blocks on the turret and they're straight/square but when i indicate the shank of the tool itself, its out about .001" over 1" stroke. is this normal? can it be dialed in better? is it the er collet thats not holding it straight?

desperately need some help figuring it out.

thanks all!

Thats the problem ive had recently and went and used a brook field holders except min was 1.850 long drill
1st make sure like bob said you have no nicks. also try rotating the shank a few times and see if you get the same results.
also if you use try different collet sizes Like one up and one down. Another thing is dont tighten the collet so tight.
the one size fits xxx drill sizes dont usually work on long close tolerance stuff. you could lap a collet or find a metric that's even closer to the size you need..

I am going this route here soon as I am tired of messing with it.
CNC lathe Adjustable small drill/reamer holders

the gaff system, teachmeplease turned me onto it.

empower · Oct 29, 2019

litlerob1 said:
Maritool is very good quality. Assuming everything is clean.

We need to know feeds and speeds, size of Drilled hole, coolant, AND what the result of you trying to Ream those holes with that Reamer are....

R

i havent even cut a hole yet, just indicating in my tools and seeing them not straight to spindle in both xz and yz planes. maybe i'm not indicating them right?
how do you guys check that your drills are straight to the spindle?

btw the holders/collets and nuts are BRAND NEW, sprayed out with brake cleaner and then air. no dirt or chips in there.

empower · Oct 29, 2019

Delw said:
Thats the problem ive had recently and went and used a brook field holders except min was 1.850 long drill
1st make sure like bob said you have no nicks. also try rotating the shank a few times and see if you get the same results.
also if you use try different collet sizes Like one up and one down. Another thing is dont tighten the collet so tight.
the one size fits xxx drill sizes dont usually work on long close tolerance stuff. you could lap a collet or find a metric that's even closer to the size you need..

I am going this route here soon as I am tired of messing with it.
CNC lathe Adjustable small drill/reamer holders

the gaff system, teachmeplease turned me onto it.

how are those holders adjustable? can you tweak it so the drill/reamer is straight?

Jason S · Oct 30, 2019

empwoer said:
Hey fellas, trying to drill .213" holes in 7075 aluminum, 1.34" deep. needs to be as straight/concentric as possible/perpendicular to the face.

machine is a yama seiki GLS-2000-LYS. using boring bar blocks with straight shank ER25 holders and dril/reamer held by collets. i indicated the blocks on the turret and they're straight/square but when i indicate the shank of the tool itself, its out about .001" over 1" stroke. is this normal? can it be dialed in better? is it the er collet thats not holding it straight?

desperately need some help figuring it out.

thanks all!

As far as your machining process: c'drill, drill(peck?), bore to reamer size(adjust so you don't leave marks) approx .20ish deep, and then ream.

Mike1974 · Oct 30, 2019

empwoer said:
Hey fellas, trying to drill .213" holes in 7075 aluminum, 1.34" deep. needs to be as straight/concentric as possible/perpendicular to the face.

machine is a yama seiki GLS-2000-LYS. using boring bar blocks with straight shank ER25 holders and dril/reamer held by collets. i indicated the blocks on the turret and they're straight/square but when i indicate the shank of the tool itself, its out about .001" over 1" stroke. is this normal? can it be dialed in better? is it the er collet thats not holding it straight?

desperately need some help figuring it out.

thanks all!

The shank of drill, or reamer? A typical HSS chucking reamer (they do make 'jig reamers' which are a little different) is meant to follow the holes, so IMO you want to hang that out a little more so the shank can flex a bit. So .001" runout shouldn't be a big deal, depending on how tight the tolerance of hole is. Like the last guy said, drill, bore to size .20-.30 deep, maybe .0005" undersize, then ream and you should be ok.

litlerob1 · Oct 30, 2019

Your set-up might be perfect. Try making a hole, then get back to us. You're fixing something that isn't broken.

R

hanermo · Oct 30, 2019

Indicating a drill shank is probably not a needed step.
The drill will drill more/less straight at best, and more/less on size at best.

But grab a gage pin in the collet.
Does it indicate straightish ?

Trying to get a hole 5.4 mm in size 34 mm deep, 1:7 D/L ratio.

Suggestion.
Drill undersize by 0.4-0.3 mm, about 5.00 mm, stub length drill, to maybe 1:4 deep, 20 mm deep or so.
Now bore to 5.2 - 5.3 mm, 0.1/0.2 mm undersize, 20 mm deep.

The hole should be perfectly round, cylindrical, and on-size to better than 0.01 mm.
The next drill only needs to go 14 mm deeper, and the existing bore should keep the drill from wandering.
At least with a carbide drill, or anything decent.

Then finish ream to size, even if the reamer was off by 0.01 mm in alignment, it will likely follow the hole and finish it to size.

Because:
The shorter boring bar, to 20 mm deep, will make a very true hole, very fast, without too much or any chatter.
Since it´s only removing a little material, a skinny boring bar should work well, in soft easy alu.
And you can probably run it really fast, 3000-5000 rpm in alu, if your lathe permits.

Why:
My suggestion does need need anything exotic re: drills or boring bars, and should be very fast to do in workflow, and very accurate in results, with minimal tooling wear.
1. The boring cycle might take 10-15-20 secs, somewhere around that.
2. But the stub drill will make the starter hole much faster than a full-length 34 mm deep drill will.
Probably save 10-20 secs on the drilling cycle, since You can likely run a stub drill twice as fast or more (8x more rigid) than the full-length drill.
3. The 2-op drill/bore then final-drill to depth, adds one op with probably near-zero additional time, sans a toolchange.
4.
Removing the first drill, should get the chips out if you dont have coolant-thru.
This makes the next drill op much easier.

Might still need to full-retract halfway if the final drilled hole does not clear the chips well.
Depending on drill, and stuff like coolant.
And speed desired.

HTH.

Ox · Oct 30, 2019

#1 best method for dead straight hole is to use a live spindle / live drill.

Then use a floating reamer holder for the reamer.

Personally - I'd put the drill in a floating holder if I was using it dead.
(Not the C-drill tho obviously)

--------------

Think Snow Eh!
Ox

Delw · Oct 30, 2019

empwoer said:
how are those holders adjustable? can you tweak it so the drill/reamer is straight?

shim stock, do the same on brook fields when needed also. Obviously your machine needs to be square as you dont want to be adjusting everytime.

empower · Oct 30, 2019

litlerob1 said:
Your set-up might be perfect. Try making a hole, then get back to us. You're fixing something that isn't broken.

R

ok, i'll do that. how do i check if the hole is straight/perpendicular to face?

empower · Oct 30, 2019

Ox said:
#1 best method for dead straight hole is to use a live spindle / live drill.

Then use a floating reamer holder for the reamer.

Personally - I'd put the drill in a floating holder if I was using it dead.
(Not the C-drill tho obviously)

--------------

Think Snow Eh!
Ox

sorry i'm very new to lathes, could you post a link to an example of a floating reamer holder?

Thanks!

Ox · Oct 30, 2019

If the hole is on center in the front of the part, and it's on center in the back of the part, the odds are pretty good that it's perpendicular by default.
It would be difficult to produce a hole that is not square if all work done in one chucking.

That issue would be more concern if you blanked the part off and then stuffed it in a vice in your mill to drill the hole.

-------------------

Think Snow Eh!
Ox

empower · Oct 30, 2019

hanermo said:
Indicating a drill shank is probably not a needed step.
The drill will drill more/less straight at best, and more/less on size at best.

But grab a gage pin in the collet.
Does it indicate straightish ?

Trying to get a hole 5.4 mm in size 34 mm deep, 1:7 D/L ratio.

Suggestion.
Drill undersize by 0.4-0.3 mm, about 5.00 mm, stub length drill, to maybe 1:4 deep, 20 mm deep or so.
Now bore to 5.2 - 5.3 mm, 0.1/0.2 mm undersize, 20 mm deep.

The hole should be perfectly round, cylindrical, and on-size to better than 0.01 mm.
The next drill only needs to go 14 mm deeper, and the existing bore should keep the drill from wandering.
At least with a carbide drill, or anything decent.

Then finish ream to size, even if the reamer was off by 0.01 mm in alignment, it will likely follow the hole and finish it to size.

Because:
The shorter boring bar, to 20 mm deep, will make a very true hole, very fast, without too much or any chatter.
Since it´s only removing a little material, a skinny boring bar should work well, in soft easy alu.
And you can probably run it really fast, 3000-5000 rpm in alu, if your lathe permits.

Why:
My suggestion does need need anything exotic re: drills or boring bars, and should be very fast to do in workflow, and very accurate in results, with minimal tooling wear.
1. The boring cycle might take 10-15-20 secs, somewhere around that.
2. But the stub drill will make the starter hole much faster than a full-length 34 mm deep drill will.
Probably save 10-20 secs on the drilling cycle, since You can likely run a stub drill twice as fast or more (8x more rigid) than the full-length drill.
3. The 2-op drill/bore then final-drill to depth, adds one op with probably near-zero additional time, sans a toolchange.
4.
Removing the first drill, should get the chips out if you dont have coolant-thru.
This makes the next drill op much easier.

Might still need to full-retract halfway if the final drilled hole does not clear the chips well.
Depending on drill, and stuff like coolant.
And speed desired.

HTH.

thats actually what i did, put a gauge pin in the collet and indicated that, it was out .001" over 1" z length. not even sure how to indicate a drill in a non live holder...

empower · Oct 30, 2019

Ox said:
If the hole is on center in the front of the part, and it's on center in the back of the part, the odds are pretty good that it's perpendicular by default.
It would be difficult to produce a hole that is not square if all work done in one chucking.

That issue would be more concern if you blanked the part off and then stuffed it in a vice in your mill to drill the hole.

-------------------

Think Snow Eh!
Ox

trying to avoid an extra step as we're tooling up to make big runs of these parts so ideally would like to figure out how to do it in one step.

how would you check if its on center, do we absolutely need a CMM for that?

Ox · Oct 30, 2019

empwoer said:
sorry i'm very new to lathes, could you post a link to an example of a floating reamer holder?

Thanks!

https://www.ebay.com/sch/i.html?_fr...tleDesc=0&_osacat=11804&_odkw=Floating+Holder

1/3 of them in that link are NOT "floaters", but rather "Adjustables" mostly for Brown and Sharp type screw machines.
A floater is not just a dead body on Law and Order, but it holds your tool from spinning, but allows it some amount of lattitude in X and Y (some more than others) and a wee bit in Z.

You need your C-drill to be solid - even if it's not on C/L 100%, but drills and reamers (and even taps in a RIGID app) after that will benefit from floating.

Very few seem to doo it, so - maybe just toss my post asside.
I am lazy. I don't like to dick around chasing tool alignment all day on a lathe.
I found a better way 25 years ago.

I use Kenna units with 180DA collets mostly, but there doesn't seem to be any on ebay today.

Floaters are way more beneficial on a lathe than they are on a mill.

------------------

Think Snow Eh!
Ox

empower · Oct 30, 2019

Ox said:
https://www.ebay.com/sch/i.html?_fr...tleDesc=0&_osacat=11804&_odkw=Floating+Holder

1/3 of them in that link are NOT "floaters", but rather "Adjustables" mostly for Brown and Sharp type screw machines.
A floater is not just a dead body on Law and Order, but it holds your tool from spinning, but allows it some amount of lattitude in X and Y (some more than others) and a wee bit in Z.

You need your C-drill to be solid - even if it's not on C/L 100%, but drills and reamers (and even taps in a RIGID app) after that will benefit from floating.

Very few seem to doo it, so - maybe just toss my post asside.
I am lazy. I don't like to dick around chasing tool alignment all day on a lathe.
I found a better way 25 years ago.

I use Kenna units with 180DA collets mostly, but there doesn't seem to be any on ebay today.

Floaters are way more beneficial on a lathe than they are on a mill.

------------------

Think Snow Eh!
Ox

Good stuff man, thanks!

drilling/reaming a hole on a lathe

Titanium

Diamond

Titanium

Diamond

Stainless

Titanium

Titanium

Aluminum

Diamond

Diamond

Titanium

Diamond

Stainless

Titanium

Titanium

Diamond

Titanium

Titanium

Diamond

Titanium

Similar threads