Metalworking (rec.crafts.metalworking) Discuss various aspects of working with metal, such as machining, welding, metal joining, screwing, casting, hardening/tempering, blacksmithing/forging, spinning and hammer work, sheet metal work.

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Report Post  
Bill Chernoff
 
Posts: n/a
Default deep hole question

I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?

Thanks



  #2   Report Post  
PrecisionMachinisT
 
Posts: n/a
Default deep hole question


"Bill Chernoff" wrote in message
news:%q3Ac.732915$Pk3.3341@pd7tw1no...
I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?


Can you bore it with a single point tool ???

--

SVL


  #3   Report Post  
Tony
 
Posts: n/a
Default deep hole question

Are you drilling in a lathe, mill, or drill press? What kind of drill &
fixturing,,Jacobs chuck, morse taper drill, ?? Is the drill new or has it
been resharpened? Are you center-drilling prior to drilling? Is the work
being moved after the center-drilling or is it done sequentially? How are
you feeding the drill, and at what feed rate? Higher feed rates = more
error.

With a proper setup I would expect you should do better that 1/32" that you
are getting now.

Tony
"Bill Chernoff" wrote in message
news:%q3Ac.732915$Pk3.3341@pd7tw1no...
I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?

Thanks





  #4   Report Post  
michael
 
Posts: n/a
Default deep hole question

Tony wrote:

Are you drilling in a lathe, mill, or drill press? What kind of drill &
fixturing,,Jacobs chuck, morse taper drill, ?? Is the drill new or has it
been resharpened? Are you center-drilling prior to drilling? Is the work
being moved after the center-drilling or is it done sequentially? How are
you feeding the drill, and at what feed rate? Higher feed rates = more
error.

With a proper setup I would expect you should do better that 1/32" that you
are getting now.

Tony


No ****! Hell, I work closer than that with a hatchet. A dull one. Uphill, in
the snow, both ways. ;~)

Even Sam could probably do it. heavy sarcasm

michael


"Bill Chernoff" wrote in message
news:%q3Ac.732915$Pk3.3341@pd7tw1no...
I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?

Thanks







  #5   Report Post  
Karl Townsend
 
Posts: n/a
Default deep hole question

I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?


I didn't know it was possible to wander that much, you can do WAY better.

1. Clamp your part down so it won't move.

2. Spot drill or center drill first. This gives you a starting spot that
won't wander.

3. Make sure your drill is properly sharpened. A fellow named Teenut
Robert Bastow wrote the best ever drill sharpening post on this NG if you
don't know how. I've reposted it at least twice under the author "Teenut in
Heaven". Look it up at google.com


Karl






  #7   Report Post  
Machineman
 
Posts: n/a
Default deep hole question

Try some parabolic flute drills, make sure they are long enough to still
have some flute outside of the hole. Start with proper center drill and
that the surface you are drilling into is level. clamp the material down
so it cannot move while you are drilling, same for the table.

Bill Chernoff wrote:

I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?

Thanks




--
James P Crombie
Slemon Park, PEI
Canada
Machinist - 3D Cad Design - Amateur Astronomer

http://www.jamescrombie.com

  #8   Report Post  
Robin S.
 
Posts: n/a
Default deep hole question


"Bill Chernoff" wrote in message
news:%q3Ac.732915$Pk3.3341@pd7tw1no...
I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?


As others have said, center or spot drill first.

No one suggested predrilling with a smaller diameter drill. Something like a
1/16" drill would be good. The web in larger drills (especially those which
are dull or badly sharpened) tends to push the drill around.

Don't cram the drill into the material. Push firmly but let the machine do
the drilling. Peck every couple of seconds as well. Developing a good feel
for how a drill bit should be drilling is important on manual drill presses.
This feel can tell you when the machine is about to toss your piece,
break/melt your drill, or drill a straight and correctly sized hole.

Slow down your RPM if you feel like you have to push hard to eliminate
chatter. The standard (4xCS)/Ø formula will yield an RPM of about 6,000.
This is certainly too fast. I'd go about 1000. It won't hurt the drill and
(if you don't have hundreds of holes to do) time should be ok too.

HTH.

Regards,

Robin


  #9   Report Post  
PrecisionMachinisT
 
Posts: n/a
Default deep hole question


"michael" wrote in message
...
Tony wrote:

Are you drilling in a lathe, mill, or drill press? What kind of drill &
fixturing,,Jacobs chuck, morse taper drill, ?? Is the drill new or has

it
been resharpened? Are you center-drilling prior to drilling? Is the work
being moved after the center-drilling or is it done sequentially? How

are
you feeding the drill, and at what feed rate? Higher feed rates = more
error.

With a proper setup I would expect you should do better that 1/32" that

you
are getting now.

Tony


No ****! Hell, I work closer than that with a hatchet. A dull one. Uphill,

in
the snow, both ways. ;~)

Even Sam could probably do it. heavy sarcasm


Hey now!!!

I do at least *occasonally* read this group.............

Suggest first center or spot drill, to a diameter slightly greater than the
finish hole size, then drill through with a slightly undersize drill,
perhaps one of them fancy parabolic flute types.

And, as I hadnt noticed at first the depth / dia. ratio here--next, I would
probly finish the hole with a 3 flute core drill.

For even better results, I would bore with an endmill to a very slight depth
using an endmill that is the desired finish size, just prior to the core
drill operation.

Finally, all of this is out the door if your quill or knee travel is not
*exactly* parallel to your spindle bearings rotational axis.

Cheers,

--

SVL


  #10   Report Post  
Dave Baker
 
Posts: n/a
Default deep hole question

Subject: deep hole question
From: "Robin S."
Date: 18/06/04 00:51 GMT Daylight Time
Message-id:


"Bill Chernoff" wrote in message
news:%q3Ac.732915$Pk3.3341@pd7tw1no...
I am drilling 13/64 holes 2 inches deep in 6061. The bottom of the hole
wanders as as much as 0.020-0.030 off center. What is the best

straightness
I can hope for on a hole that size, that deep?

Any drill sharpening, etc, hints?


As others have said, center or spot drill first.

No one suggested predrilling with a smaller diameter drill.


Probably because it's usually a very bad idea.

Something like a
1/16" drill would be good.


The thinner the drill the more it flexes and wanders around. Once you have a
hole that's on the **** the larger drill tends to follow it and the job is
****ed. If you seriously think you can drill an accurate 2 inch deep hole with
a 1/16" drill then I have to suggest you've never tried it.

There is one good reason for double drilling and that's to get good tolerance
on hole size. You drill once at about 0.2mm to 0.5mm undersize and then do the
final pass at a slow speed and feed with the finishing drill which will then
cut pretty much to size.

Putting a very small starting hole in a job is a no no.

My solution basically mirrors a previous suggestion. Start by aligning the
machine as accurately as possible. Ensure your drill chuck has no runout. Make
a countersink to just over the finished hole size with a centre drill. Go as
deep as you can with a 2 flute slot drill (milling cutter) in a collet that's a
tad under finished size. You'll get almost zero wander with a slot drill. Then
either single or double drill to final size at a slow speed and feed.

Peck lightly and don't press the drill hard enough to bend it. Use a brand new
drill. I find you never achieve such evenness of flute width and accuracy of
cut on a resharpened drill as you do with a new high quality one.

A carbide drill has a higher modulus of elasticity than a steel one i.e. it
bends less.


--
Dave Baker - Puma Race Engines (
www.pumaracing.co.uk)
Next time someone insults you remember it takes 12 muscles to smile politely
and try to pass it off but only 4 to reach out your arm and slap the ****.


  #11   Report Post  
jim rozen
 
Posts: n/a
Default deep hole question

In article , Dave Baker says...

The thinner the drill the more it flexes and wanders around. Once you have a
hole that's on the **** the larger drill tends to follow it and the job is
****ed. If you seriously think you can drill an accurate 2 inch deep hole with
a 1/16" drill then I have to suggest you've never tried it.


It can be done. Key is to use a high quality drill. I wound up drilling
an 0.043 hole in a two inch long piece of permaloy. But then I cheated
and drilled from both ends.

This was done with a Gurhing parabolic flute high-cobalt drill, with
the chuck mounted on the lathe compound. Infeed was done with the
compound aligned with the bed, and chip clearing was done with
the carriage traverse, running up to a stop on the bed.

There is one good reason for double drilling and that's to get good tolerance
on hole size.


Here I have to disagree with you Dave, even though you're clearly
well-skilled in general. Larger drills don't cut on their dead center
and the forces that occur at this point do tend to induce wander.
I prefer to drill a straight hole with the small drill first, as
you say the larger one will follow that, spot on.

I would say it's easier to drill a straight hole with a drill that
has the smallest dead center - sure you can get the 135 degree
split point drills, but my tiny drill was ground that way from
the manufacturer too.

Key in any event is to use the highest quality cutting tool you can
get. I was trying to do the permaloy tube thing using cheapistan
HSS drills and was getting about a quarter of an inch of action out
of them before they dulled and had to be swapped.

I drilled three two inch permaloy tubes with the *same* guhring
drill.

==================================================
please reply to:
JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com
==================================================

  #12   Report Post  
Robin S.
 
Posts: n/a
Default deep hole question


"Dave Baker" wrote in message
...

No one suggested predrilling with a smaller diameter drill.


Probably because it's usually a very bad idea.


That's an aggressive posture.

Rarely (never?) in machining are things black and white.


Something like a
1/16" drill would be good.


The thinner the drill the more it flexes and wanders around. Once you have

a
hole that's on the **** the larger drill tends to follow it and the job is
****ed. If you seriously think you can drill an accurate 2 inch deep hole

with
a 1/16" drill then I have to suggest you've never tried it.


Again, posturing. What's with the attitude?

The 1/16" hole doesn't need to go all the way through, although if it does
it probably won't hurt. Once the drill has entered the material and is going
reasonably straight, it should hold its course. Mind you, all of this is up
in the air anyway. If he wants to put a 13/64" hardened shaft through the
hole, it almost certainly won't work as there will be some wander anyway.
But we've only estabilished that he's looking for *less* wander than he had
before.


There is one good reason for double drilling and that's to get good

tolerance
on hole size.


Perhaps in a pinch. I'd be inclined to order the reamer, if you really want
to get technical. But in this instance, we're not getting that technical.

In fact, lets reafirm our objectives he "Home shop machinist" Bill
Chernoff doesn't appriciate that his 13/64" drill wanders .020" through a
piece of 2" thick 6061 aluminum. He hasn't stated his feeds, speeds, machine
he's using, amount of experience he has, other situations that would lead
him to make assumptions, etc.

The above will help us later.


Putting a very small starting hole in a job is a no no.


I work by 15-30% (for a new drill the web is typically about 15% of the
diameter).


My solution basically mirrors a previous suggestion. Start by aligning the
machine as accurately as possible.


How accurately? Do you see notes on drawings saying "as accurately as
possible"?

Yes, I'm being a jackass. As you can see it's about posturing.

Ensure your drill chuck has no runout.


It certainly sounds like we have a profesisonal journeyman machinist here. I
should like to see this drill chuck, and I should like to pay very little
for it because Bill Chernoff probably doesn't want to spend $400+ on such a
chuck.

Remember our reafirmation of objectives above?

Jackass? Yes. It's all about posturing.

Make
a countersink to just over the finished hole size with a centre drill.


A countersink with a center drill? You have to choose.

Go as
deep as you can with a 2 flute slot drill (milling cutter) in a collet

that's a
tad under finished size. You'll get almost zero wander with a slot drill.

Then
either single or double drill to final size at a slow speed and feed.


100RPM, .0003/rev? That's slow.


Peck lightly and don't press the drill hard enough to bend it.


Do you frequently feel your drills bend?

Use a brand new
drill.


Most HSM's have unlimited budgets and time to buy new tooling whenever
required.

I find you never achieve such evenness of flute width and accuracy of
cut on a resharpened drill as you do with a new high quality one.


Perhaps you need to resharpen more drills.

I can see the necessity for new tooling in a production setting but for the
HSM and frequently in tool shops, one drill could be sharpened ten times
before it shatters and another one is used.


A carbide drill has a higher modulus of elasticity than a steel one i.e.

it
bends less.


Ha! That's certainly something Bill Chernoff should go and buy tomorrow
morning. A carbide drill!

Dave, here's the news. Chances are (not absolutly though) that most HSM's
here bought the drill press on special at Harbour Freight and picked up a
set of drills to go with. Total cost was maybe $200.

HSM chucks bit of desired hole diameter and switches drill "ON" at factory
preset RPM. Could be 2500, could be 60. HSM proceeds to lower drill to
piece. Drill bounces around a bit and finally bites. Drill is perhaps
already bent and the bouncing didn't help. HSM crams drill through material
as the bit spins in the $10 chuck with one stick jaw and a bag of grinding
dust in the bearings. Drill miraculasly gets through the material and of
course the hole is in the wrong place.

I'm not attacking the "HSM" but I remember using a micrometer as a c-clamp
once too.

Carbide drills and new tooling for tomorrow's production run on the
receiving bay's floor tomorrow at 9am is best left to the professionals like
you. As for those who like to fiddle around in the basement (and probably
have more fun than anyone getting paid to do it), they just want to know why
the drill made a hole the shape of a "c".

BTW, it's all about posturing. Your posture got me in a bad mood and sent me
off on this rant. If we could all be a bit nicer, this wouldn't happen so
often. I'm a bit squirly today because I had a practical midterm today. The
German Chamber of Commerce has calculated that 7.5hrs is required to make
the assembly you have to make, given a qualified apprentice. They give us
8hrs (precisely no more). Under the gun for 8hrs straight (minus two breaks)
causes people to get a bit frazzled.

Regards,

Robin




  #13   Report Post  
Dave Baker
 
Posts: n/a
Default deep hole question

Subject: deep hole question
From: "Robin S."
Date: 18/06/04 02:49 GMT Daylight Time
Message-id:


"Dave Baker" wrote in message
...

No one suggested predrilling with a smaller diameter drill.


Probably because it's usually a very bad idea.


That's an aggressive posture.


Not really. It just is a very bad idea. A 1/16" drill bends like buggery, they
snap like carrots and they only have the flute length for an inch or so of
drilling. It isn't the tool for starting a 5mm hole 2 inches deep. When I need
a second opinion on a machining matter I ask my mate who's a 30 year CNC
machinist making high volume complex items. We've looked at accurate hole
drilling many times. The answers are mainly common sense. Use the shortest
drill you can. Stub drills are stiffer than jobber length ones. Carbide stub
drills are stiffer than HSS ones. Slot drills are better than either. Centre
the hole first. Use the highest quality drills you can afford. Use the biggest
drill you can get away with if you're double drilling.


Rarely (never?) in machining are things black and white.


Something like a
1/16" drill would be good.


The thinner the drill the more it flexes and wanders around. Once you have

a
hole that's on the **** the larger drill tends to follow it and the job is
****ed. If you seriously think you can drill an accurate 2 inch deep hole

with
a 1/16" drill then I have to suggest you've never tried it.


Again, posturing. What's with the attitude?


Moi? Attitude ?


The 1/16" hole doesn't need to go all the way through, although if it does
it probably won't hurt. Once the drill has entered the material and is going
reasonably straight, it should hold its course. Mind you, all of this is up
in the air anyway. If he wants to put a 13/64" hardened shaft through the
hole, it almost certainly won't work as there will be some wander anyway.
But we've only estabilished that he's looking for *less* wander than he had
before.


What he is looking for is as good a job as he can get. Same as anyone else. The
advice should be to get him spot on if possible.




There is one good reason for double drilling and that's to get good

tolerance
on hole size.


Perhaps in a pinch. I'd be inclined to order the reamer, if you really want
to get technical. But in this instance, we're not getting that technical.


If you're after tenths then sure a reamer is essential. Double drilling can get
you within half a thou thou or a thou with a good quality drill and the right
technique.



In fact, lets reafirm our objectives he "Home shop machinist" Bill
Chernoff doesn't appriciate that his 13/64" drill wanders .020" through a
piece of 2" thick 6061 aluminum. He hasn't stated his feeds, speeds, machine
he's using, amount of experience he has, other situations that would lead
him to make assumptions, etc.

The above will help us later.


Putting a very small starting hole in a job is a no no.


I work by 15-30% (for a new drill the web is typically about 15% of the
diameter).


Don't understand that comment.




My solution basically mirrors a previous suggestion. Start by aligning the
machine as accurately as possible.


How accurately? Do you see notes on drawings saying "as accurately as
possible"?


Yep - In the UK it was deemed to mean within 1 thou in the celebrated law case
Arkell V Pressdram (1971).



Yes, I'm being a jackass. As you can see it's about posturing.

Ensure your drill chuck has no runout.


It certainly sounds like we have a profesisonal journeyman machinist here. I
should like to see this drill chuck, and I should like to pay very little
for it because Bill Chernoff probably doesn't want to spend $400+ on such a
chuck.

Remember our reafirmation of objectives above?

Jackass? Yes. It's all about posturing.

Make
a countersink to just over the finished hole size with a centre drill.


A countersink with a center drill? You have to choose.


Can't see your problem here. A countersink is what a centre drill is designed
to make.



Go as
deep as you can with a 2 flute slot drill (milling cutter) in a collet

that's a
tad under finished size. You'll get almost zero wander with a slot drill.

Then
either single or double drill to final size at a slow speed and feed.


100RPM, .0003/rev? That's slow.


On a 5mm drill I'd say 250 rpm for a slow second pass.



Peck lightly and don't press the drill hard enough to bend it.


Do you frequently feel your drills bend?


No - I use mine with careful feel and technique.


Use a brand new
drill.


Most HSM's have unlimited budgets and time to buy new tooling whenever
required.


Struth. A 5mm HSS drill costs what? a dollar or two?




I find you never achieve such evenness of flute width and accuracy of
cut on a resharpened drill as you do with a new high quality one.


Perhaps you need to resharpen more drills.


I've resharpened **** loads of em and never managed to get them as nice as a
brand new high quality one. That's even using a drill sharpening fixture. If
that's my own fault so be it but if I can't do it then so can't most other
people.


I can see the necessity for new tooling in a production setting but for the
HSM and frequently in tool shops, one drill could be sharpened ten times
before it shatters and another one is used.


A carbide drill has a higher modulus of elasticity than a steel one i.e.

it
bends less.


Ha! That's certainly something Bill Chernoff should go and buy tomorrow
morning. A carbide drill!


I'm not advocating that everyone needs to use carbide drills. Just pointing out
the physics of the thing. I only have a few myself and they were given to me by
a friend who'd got them free from someone else. When I'm drilling really tough
materials and need good concentricity (aluminium bronze valve guides) I start
with a 5mm carbide drill and then finish with the 8mm HSS one. Advantage is the
carbide drill never wears and stays sharp and takes the bulk of the material
out. The 8mm one follows what's there.

Still, a 5mm carbide drill isn't mega bucks either if the job merits it.


--
Dave Baker - Puma Race Engines (
www.pumaracing.co.uk)
Next time someone insults you remember it takes 12 muscles to smile politely
and try to pass it off but only 4 to reach out your arm and slap the ****.
  #14   Report Post  
jim rozen
 
Posts: n/a
Default deep hole question

In article , Robin S. says...

Peck lightly and don't press the drill hard enough to bend it.


Do you frequently feel your drills bend?


No, you *see* them bend. When I was drilling that
deep hole in the nickel-iron tubing, I didn't want
the material to work harden - so I was pushing the
drill pretty hard. When I went too far it went
beyond the column limit and bowed out a tad...
so I backed off a bit.

Use a brand new
drill.


Most HSM's have unlimited budgets and time to buy new tooling whenever
required.

I find you never achieve such evenness of flute width and accuracy of
cut on a resharpened drill as you do with a new high quality one.


Perhaps you need to resharpen more drills.


Honestly for this one I have to agree with Dave here. There
is simply no way I would be able do do as good a job as Gurhing
with pointing one of their drills. That the holes came out
as good as they did (about two thou out over an inch) I attribute
mostly to their drill sharpening prowess.


I can see the necessity for new tooling in a production setting but for the
HSM and frequently in tool shops, one drill could be sharpened ten times
before it shatters and another one is used.


For larger drills, yes. But for the smaller ones (and remember, I'm
advocating pilot-drilling deep holes) there is no way the HSM can do
as good a job as the manufacturer.

Jim

==================================================
please reply to:
JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com
==================================================

  #15   Report Post  
Dan Caster
 
Posts: n/a
Default deep hole question

I was taught by a skilled machinest long ago to first drill with a
drill bit that is the same size or slightly bigger than the web of the
drill needed for the final hole. I think this is what Robin means by
the 15-30%. If you are going to drill a 5 mm hole then use a 1 mm (
20% of 5mm ) pilot drill.

But for holes up to about 5 mm I usually don't use a pilot drill. But
for a 25 mm hole, a 5 mm pilot hole helps me. Try it and make up
your own mind.

Dan




oEmails (Dave Baker) wrote in message

No one suggested predrilling with a smaller diameter drill.


I work by 15-30% (for a new drill the web is typically about 15% of the
diameter).


Don't understand that comment.


Reply
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules

Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Deep hole drilling WAS leadscrew repair Roger Hull Metalworking 5 February 28th 04 08:23 PM
Cosmetic Aluminum 'Hole Plugging' Help Needed Jim Flanagan Metalworking 5 January 23rd 04 12:25 PM
OT-Michael Moore digs himself a deeper hole Gunner Metalworking 1 October 6th 03 05:36 PM
Cutting a hole in an external wall Matt G UK diy 3 September 15th 03 09:05 AM
Roughing out 4" hole in .750 thick aluminum. Ryan Metalworking 15 August 8th 03 03:47 AM


All times are GMT +1. The time now is 12:51 PM.

Powered by vBulletin® Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.
Copyright ©2004-2024 DIYbanter.
The comments are property of their posters.
 

About Us

"It's about DIY & home improvement"