How to drill .125" +/- .0002"?

Nerdlinger · Jul 18, 2017

Hey all! I am not used to holes with such a tight tolerance. I need to cross drill .125" +/- .0002 in 3/4" round 1018. Will a high quality 1/8" carbide do it or should I go a size under and then ream? Production would be in a tight Brother S700 (not sure what the runout is but no crashes (yet)) so it should be pretty good.

Bonus question - For starters I tried using some carbide metric equivalent of .1245" in a Haas TM-1. I didn't "measure" the hole but the no-go gage go'd, so it drilled oversize by at least .0008". I put an indicator on the drill and measured .0015" TIR. Will that actually translate to the hole being .0015" larger with carbide?

Thanks!

G00 Proto · Jul 18, 2017

It should be no problem hitting +/-.0002 all day long with a standard jobber drill from Harbor Freight, as long as you are using a home built router with a Chinese spindle

.0002 is hard for me to hit, day in day out with even the best drills. I have a bunch of call outs on a family of parts that have that tolerance on a .1265 hole, and I hit it (most of the time) with a 3 flute carbide 3.2 mm drill. Sometimes, if the wind blows just right, they come in a bit large or a bit small. I know that they are a press fit for a .125 DP so there is a little wiggle room (internal product).

If they were external parts I would certainly ream them, and check them often. At that tolerance, my experience is even reamers are susceptible to getting dull or varying their diameter due to differences in lubrication at the cutting edge.

michiganbuck · Jul 18, 2017

Likely the .1245 would have cut .0002/.0004 over the micrometer size if you had pre-drilled a bit smaller..But with heat and dulling you could not count on a drill to hold .0002 for ever. Even a good reamer can dull and heat up for +.0002.

That is where a TC grinder comes in handy.. you can try a reamer and then grind it back on the back-taper to get the exact size. Yes just shorten it..

QT [the drill and measured .0015" TIR.} likely it was the drill point off center .0004.. not the TIR IMHO.

I would likely pre-drill #31 or #32 on a sample 1018 and re try the ,1245.. if it should start out .12485 and grow you are in.

[will a .125 do...should I go a size under and then ream?] Yes you have to go a bit under then ream.

Laptr · Jul 18, 2017

That's a tough project. Definitely drill and ream. Make sure your reamer has the right cut amount.

litlerob1 · Jul 18, 2017

Follow this link to the Guhring website, I have found myself in lots of difficult to accomplish drilling situations and Guhring has always had the answer for me. The link is to a carbide coolant fed drill for steel @ 8x diameter and a drill diameter of .1248"

I don't use reamers, unless I have literally tried everything else within reason, but if you must I would invest in a carbide reamer.

Guhring, Inc. - Tool List

R

eaglemike · Jul 18, 2017

Spot, drill, ream.
The amount of material removed by the reamer can make the difference between success and failure. Reamer style, spiral flute or straight, etc. Different materials can require different material for the reamer. The (seeming old at the time) guys I learned from insisted on lightly stoning the corner of a new reamer. Rpm, feed rate, oil/lube/coolant used all can make a difference. Their old rule of thumb was 1/2 the rpm of the drill, and 2X the feed.
If the alloy is not too hard, and the geometry allows it, I've swaged holes to size by pushing a hardened bearing through it, after reaming a couple of tenths to a half-thou undersize. If you have a bunch of holes of course, major pain. Could always make a tool and put it in the spindle too.
There's always honing and lapping too, haha.

At least 1018 isn't too expensive, or one of the hard exotics.
If you think of it, share what you decided works?

plastikdreams · Jul 18, 2017

Drill and ream...it's in a see and see, just keep checking parts. Use good quality carbide reamers and flood the piss out of it.

I've held those tolerances on a slightly larger hole in carpenter c465 on a late 90s Haas...you should be fine

CarbideBob · Jul 18, 2017

Not many drills are made to within +/-.0002 so your tolerance is blown even if they drilled a perfect hole.
Standard reamer tolerance is +0/-.0002 so half your range is sucked up by the tooling and you would want a .0001 over to center size on .125 so that is a special.
One can do selective grinding as suggested by Michiganbuck but that's rather time consuming.
Or you could buy a bunch of reamers and sort them.

In reality very few people can measure a .125 hole at this tolerance. This is way beyond the world of gage pins and 99% of the CMMs out there.

You want to know how the customer will check the results. Key above all other things.

It is possible to G-drill or D-ream to these numbers. Both not cheap tooling with lots of effort spent on getting the process "just right".
If you need 2 tenths you have to think some kind of "should-be" basic control at 20-40 millionths and then the other factors in the world eat up the rest.
Bob

Job Shopper TN · Jul 18, 2017

It takes serious investment to get precision holes like this.

We are capable of holding to a .0004" overall diameter tolerance using precision carbide drills and hydraulic holders. Runout is absolute key. Absolute key. Can't stress that enough. We started using Schunk hydraulic holders for this type of deal. We order sleeves and buy our carbide drills to fit nominal-size sleeves. I mean, really, a couple of tenths' runout can kill you on this.

I grant you, we are checking these holes with go/no go pin gages. No clue as far as real roundness, cylindricity, etc.. But it's how the customer checks 'em.

I would go there, man; get a super-precise holder (hydraulic) and a good drill (we use Walter). Complicating matters is drilling into round bar, but I can't help you there. No real experience on that matter. It may be prudent to mill deep enough to give the drill a flat surface to start on.

RobMcQuillen · Jul 19, 2017

Harvey Tool - Miniature Reamers

With the right setup, achievable.
No chance of actually holding that over .750 length with .0015" TIR :eek:

, when I run them I've always had them under .0001" TIR at the tip. Look at Parlec EROS.

We have evaluated the size and cylindricity of a .500" long bore created by a .1590" reamer, the average diameter was .1590" and cylindricity was under .0002". Good enough for what we needed.

deadlykitten · Jul 19, 2017

Nerdlinger said:
Hey all! I am not used to holes with such a tight tolerance. I need to cross drill .125" +/- .0002 in 3/4" round 1018.

hy Nerdlinger

what is the length of the hole ? 3/4" ? how many parts ?

Nerdlinger said:
Bonus question - For starters I tried using some carbide metric equivalent of .1245" in a Haas TM-1. I didn't "measure" the hole but the no-go gage go'd, so it drilled oversize by at least .0008"

sometimes you may adjust the size by using a different feed, but this wont last when many parts are there

some tricks for short runs are not reliable on series

Nerdlinger said:
I put an indicator on the drill and measured .0015" TIR. Will that actually translate to the hole being .0015" larger with carbide?

if it transfers, it may not be the main deviation that must be eliminated

also, it may not transfer; for example a long drill will bend anyway

ManualEd · Jul 19, 2017

litlerob1 said:
Follow this link to the Guhring website, I have found myself in lots of difficult to accomplish drilling situations and Guhring has always had the answer for me. The link is to a carbide coolant fed drill for steel @ 8x diameter and a drill diameter of .1248"

I don't use reamers, unless I have literally tried everything else within reason, but if you must I would invest in a carbide reamer.

Guhring, Inc. - Tool List

R

And make sure the reamer is coolant thru.
No need to be pecking in this day and age.

zero_divide · Jul 19, 2017

Drill. Ream.
Use carbide reamer as it is less likely to wear.

MIGHT have to hone.

Mike1974 · Jul 19, 2017

CarbideBob said:
Not many drills are made to within +/-.0002 so your tolerance is blown even if they drilled a perfect hole.
Standard reamer tolerance is +0/-.0002 so half your range is sucked up by the tooling and you would want a .0001 over to center size on .125 so that is a special.
One can do selective grinding as suggested by Michiganbuck but that's rather time consuming.
Or you could buy a bunch of reamers and sort them.

In reality very few people can measure a .125 hole at this tolerance. This is way beyond the world of gage pins and 99% of the CMMs out there.

You want to know how the customer will check the results. Key above all other things.

It is possible to G-drill or D-ream to these numbers. Both not cheap tooling with lots of effort spent on getting the process "just right".
If you need 2 tenths you have to think some kind of "should-be" basic control at 20-40 millionths and then the other factors in the world eat up the rest.
Bob

I believe you know more than me about this, but what about tenth pins? They are supposed to be +0.0/-.00004 (or opposite if plus). I would think having those in the appropriate sizes would work. .1248 goes in, .1252 doesn't = good part. SEE BELOW (disregarding temp and any other factors, if your shop runs 80deg..

)

Job Shopper TN said:
It takes serious investment to get precision holes like this.

We are capable of holding to a .0004" overall diameter tolerance using precision carbide drills and hydraulic holders. Runout is absolute key. Absolute key. Can't stress that enough. We started using Schunk hydraulic holders for this type of deal. We order sleeves and buy our carbide drills to fit nominal-size sleeves. I mean, really, a couple of tenths' runout can kill you on this.

I grant you, we are checking these holes with go/no go pin gages. No clue as far as real roundness, cylindricity, etc.. But it's how the customer checks 'em.

I would go there, man; get a super-precise holder (hydraulic) and a good drill (we use Walter). Complicating matters is drilling into round bar, but I can't help you there. No real experience on that matter. It may be prudent to mill deep enough to give the drill a flat surface to start on.

How the customer checks them is probably the most important factor. Ask them, and hope its not just on a cmm!

michiganbuck · Jul 19, 2017

Think after try the drill with a pre-hole a decent .1248 reamer might fill the bill..If you are lucky..(perhaps a .1247 ?)

A carbide drill will make a good number of same size holes but one drill to another may be a big change.

Sharpening back for size or just sharpening for dull such a small reamer is difficult because you want zero/dead true run out at the end and it's hard to get with any holding device..

Most reamers taper back perhaps .0002/.0003 per inch. Some are not easy to measure because the measure device is straight across and flutes are not always straight across. Foe larger reamers the OD land fill that area so measure is more accurate.

The way I run small reamers is to drill and then ream with the same reamer to make a slug to become a reamer bushing then with holding in that bushing and a double tip finger grind the end with perhaps 9* primary with a 320 wheel. The double tip finger has a tall portion to ride the Od and so hold the lip stop at the same diameter. Yes a .125/.127 or so bushing would be fine for .124 reamer.

The same using a bushing can be done for drill sharpening to get the primary then perhaps hand back off the secondary for high precision drills.

Yes larger reamer perhaps 1/2" and up are often done between centers. Yes a .125 (or so) can also be done between centers.

Problem with bargain basement reamers is the end often is not true to the OD.

deadlykitten · Jul 19, 2017

helix + grinding stone + coolant driven holder ?

ps : excalibur / esl / etc / kindly / double kindly

litlerob1 · Jul 19, 2017

Nothing personal Buck, but screw reamers. Just drill it with a good drill and be done with it. If you need to buy 5 drills, shit they're 1/8" drills, it's not like you are never going to use them again. Buck you got some Voodoo going on with your reaming,

do I have to sell my soul for that kind of knowhow? :bowdown:

Oh wait I already did sell it, trying to figure out how to change Fanuc ladder logic. Fresh out of soul, maybe I could use one of the guys'

@ Nerdlinger, I do agree when you drill good holes then switch from drill to drill and expect the exact same hole that can get a little touchy, at that size and tolerance.

R

Dinosaur Engineer · Jul 19, 2017

Carbide 3 flute drills are much more accurate than 2 flute types but +/- .0002 is a tight tol to achieve. 3 flute drills can achieve reamer tols and control roundness much better.

michiganbuck · Jul 19, 2017

litlerob1 said:
Nothing personal Buck, but screw reamers. Just drill it with a good drill and be done with it. If you need to buy 5 drills, shit they're 1/8" drills, it's not like you are never going to use them again. Buck you got some Voodoo going on with your reaming, do I have to sell my soul for that kind of knowhow? Oh wait I already did sell it, trying to figure out how to change Fanuc ladder logic. Fresh out of soul, maybe I could use one of the guys'

@ Nerdlinger, I do agree when you drill good holes then switch from drill to drill and expect the exact same hole that can get a little touchy, at that size and tolerance.

R

Agree a drill would do if it drilled .125+- .0002.. The drill the Op has may do the job well..Buying a $15 or $30 reamer would be Ok also. But two may be needed as may a drill to find the size... With making perhaps 600 holes and a sharpening might be due. Still $30. divided by 600 is a nickle a hole. One may not chose sharpening as one reamer would take perhaps an hour to make a bushing and run the job ..At $70 an hour not worth the due, but instead of watching a boring TV show may be the way.

And one might go fishing for sport and another grind reamers. :cryin:

Qt: [to sell my soul..] I may need one , How much? Want to trade it for a grinder?

deadlykitten · Jul 19, 2017

just drill it and adjust the tolerance with a bearing sphere and a hammer

How to drill .125" +/- .0002"?

Stainless

Hot Rolled

Diamond

Plastic

Diamond

Stainless

Diamond

Diamond

Cast Iron

Aluminum

Banned

Stainless

Stainless

Diamond

Diamond

Banned

Diamond

Aluminum

Diamond

Banned

Similar threads