Drilling recommendations

BALNH · Nov 18, 2016

I have a 6061 part with 200+ .250 holes +.001-.000 through hole .500 dp. I was hoping to punch them through with no reaming. I have 10000 rpm and no through spindle coolant. I was thinking of a OSG Gold but I can't recall holding that tight of diameter tolerance with them in the past. Am I in left field with my expectations?

DMF_TomB · Nov 18, 2016

BALNH said:
I have a 6061 part with 200+ .250 holes +.001-.000 through hole .500 dp. I was hoping to punch them through with no reaming. I have 10000 rpm and no through spindle coolant. I was thinking of a OSG Gold but I can't recall holding that tight of diameter tolerance with them in the past. Am I in left field with my expectations?

.
spindle runout or wobble will effect hole size
.
carbide drills often have back taper of .020" or smaller dia toward shank i have seen resharpened drills easily under size over .001"
.
reminds me of the guy who want a bridgeport mill in his garage and has a budget of $200. nice to want things

michiganbuck · Nov 18, 2016

Drill and ream tool are out there. Holding a close size often needs a circle OD land and more that two flutes. I think that +- .0005 is not easy with drills.

1/4 Inch Reamer Diameter, 2-15/16 Inch Flute 2535169 - MSC

Don't know the material but 500 or 700 holes might be the limit between sharpenigs with good set-up.
I have experience with step drills and +- .0005 is close for them.. Simple reamers can hold .0002 with ease.

BALNH · Nov 18, 2016

Parts are quoted to ream, we are a job shop thinking outside the box is rewarded.

doug925 · Nov 18, 2016

There are 3 ways to skin this cat, using drilling only.
1) a 3 flute, 1/4" carbide drill should blow that hole with no problems. The 3rd flute helps stabilize the drill, & act more like a reamer.

2) test cut using the desired drill, and the exact same parameters you programmed for on the actual job. Tweak it until the diameter comes in, or provides enough data to predict if it will work or not.
I would think that a screw machine length, parabolic (?), bright flute would do it without problems.

3) drill a Ø15/64" hole first, and follow that back up with the 1/4", running 1.5x feed and .5 rpm.

Doug.

BALNH · Nov 18, 2016

Thanks Doug I'm looking at 3 flutes now.

dodgin · Nov 18, 2016

If I was in that position I'd call up Sandvik and see if a Corodrill can hold that tolerance. It's been my experience with them that they'll give you a range that they'll guarantee it to hold, and if it doesn't hold it you don't buy it.

I've had good luck with those drills holding some tight tolerance, but I was running TSC with them also, on some pretty damn well maintained machinery.

Mtndew · Nov 18, 2016

BALNH said:
I have a 6061 part with 200+ .250 holes +.001-.000 through hole .500 dp. I was hoping to punch them through with no reaming. I have 10000 rpm and no through spindle coolant. I was thinking of a OSG Gold but I can't recall holding that tight of diameter tolerance with them in the past. Am I in left field with my expectations?

I think you're just leaving yourself open for headaches by not reaming.
Get a LH Spiral .2500 reamer and be done with it.

michiganbuck · Nov 18, 2016

Mtndew said:
I think you're just leaving yourself open for headaches by not reaming.
Get a LH Spiral .2500 reamer and be done with it.

Agree...And if you go in with two drills that is near the time of drill and ream.

BALNH · Nov 18, 2016

I'll end up drilling and reaming.

Rapid_Tech · Nov 19, 2016

Just spend $75-100 on a good stub carbide drill and test it out. Better yet, try a MA Ford circuit board drill. It's listed in the KBC catalogue for about $30 Canadian.

I've drilled about 250 1/8" holes with one circuit board drill through .375 thick 6061 and it cut maybe .0002-.0004" over. Hole size wasn't even important I just wanted a stub carbide drill so I could drill the holes fast. The drill was held in a Maritool ER16 collet, nothing fancy. This was done on an old Haas at 5000rpm at 6 or 8ipm (I can't remember right now) with regular flood coolant pecking every .100.

Unless you've got some special roundness or surface finish requirement, give the drill a test to see how it performs. What have you got to lose?

If you still end up reaming I'd also recommend a MA Ford carbide reamer. I just finished a job reaming 450 .1875-.1878 holes though 1" brass, with a .625" gap in the middle. I drilled the hole with a 4.3mm carbide drill and reamed the hole at 2000rpm with a feed of 10ipm. Hole size from start to finish was .1876, checked with a Mitutoyo small hole bore gage (no guessing with pins). Again, tool was held in a ER16 collet from our good friend Frank Mari.

Oldwrench · Nov 19, 2016

Rapid_Tech said:
checked with a Mitutoyo small hole bore gage (no guessing with pins)

If the Go pin is .1875 and goes, and the No Go pin is .1878 and doesn't go, the hole is good. That's not guessing.

Or were you talking about .001 increment pins, as in, "does this one wiggle too much or not enough...or does the next one up maybe start a little bit? Here, try it Jethro, you're stronger'n me..."

BALNH · Nov 19, 2016

After looking at he step file I may end up having to mill the holes to finish diameter. The hole pattern leaves a .013 web between holes. I think reaming will bulge the adjacent hole.

Rapid_Tech · Nov 19, 2016

Oldwrench said:
If the Go pin is .1875 and goes, and the No Go pin is .1878 and doesn't go, the hole is good. That's not guessing.

Or were you talking about .001 increment pins, as in, "does this one wiggle too much or not enough...or does the next one up maybe start a little bit? Here, try it Jethro, you're stronger'n me..."

Yeah, because I'm going to buy a set of pins in .0001 increments! One bore gage will measure from .160-.2. I'd need to buy 400 pins to check all those sizes. If that's your idea of fun, knock yourself out.

HuFlungDung · Nov 19, 2016

Oldwrench said:
If the Go pin is .1875 and goes, and the No Go pin is .1878 and doesn't go, the hole is good. That's not guessing.

Or were you talking about .001 increment pins, as in, "does this one wiggle too much or not enough...or does the next one up maybe start a little bit? Here, try it Jethro, you're stronger'n me..."

Gaging with pins might give you a consistent result, but what size is the hole, really? I maintain your average Joe cannot put a pin in a hole without .0002 to .0003" clearance. I'm talking simple hole drilling and reaming, not some super finished honed crapola that takes a ton of work to achieve perfect roundness and straightness so you can fit something in that has .0001" clearance providing the sun doesn't shine on it.

Mechanola · Nov 19, 2016

BALNH said:
Parts are quoted to ream, we are a job shop, thinking outside the box is rewarded.

In most cases you’re better off thinking inside the box, believe me.

Drill all holes, then ream ‘em.
Of course, you’ll chamfer both sides of the bores.

Philabuster · Nov 19, 2016

Rapid_Tech said:
Yeah, because I'm going to buy a set of pins in .0001 increments!

AKA, Deltronic X Gage Pin sets. :cloud9:

http://www.deltronic.com/literature/Deltronic-Gage-Guide-2014.pdf

Rapid_Tech · Nov 19, 2016

Philabuster said:
AKA, Deltronic X Gage Pin sets.

http://www.deltronic.com/literature/Deltronic-Gage-Guide-2014.pdf

I know they exist, but why spend so much money and take up so much space when one tool will replace 400 individual pins. No offense, but do some people seriously enjoy wasting their time and money?

dstryr · Nov 19, 2016

Rapid_Tech said:
I know they exist, but why spend so much money and take up so much space when one tool will replace 400 individual pins. No offense, but do some people seriously enjoy wasting their time and money?

LOLZ
Deltronic pin sets aren't very expensive.
Just bought a .191 set. $150

This is why Deltronic pins are used... How are you going to check +/-.0002 when the tool is only accurate to .0002? I much prefer deltronic pins even to my Zeiss scanning CMM when the hole size permits it.

Bore Gages Series 526-for Extra Small Holes
Series 526
Features
These Bore Gages measure diameters of small holes. The radial displacement of split-ball contact is converted to axial displacement of measuring rod, which is shown on the dial indicator.

Technical Data
Accuracy:4µm/.00016”
Indication stability:2µm/.00008”
Graduation:0.01mm,0.001mm, .0005 or.00001"

3 flute drill from Guhring or Mitsubishi should do it . +.001 -.000 isnt that bad. Might need them to custom build a .2503-.2505 drill though?
MA Ford Carbide TRU Size reamers are great. They are usually +.0001 -.0000 on hole size.

Philabuster · Nov 19, 2016

Rapid_Tech said:
I know they exist, but why spend so much money and take up so much space when one tool will replace 400 individual pins. No offense, but do some people seriously enjoy wasting their time and money?

For small holes like 1/2" and down, they are the shiznit. Larger holes I use the Etalon bore mics.

Anytime I do small hole precision boring, the Deltronics come out.

Drilling recommendations

Cast Iron

Diamond

Diamond

Cast Iron

Titanium

Cast Iron

Hot Rolled

Diamond

Diamond

Cast Iron

Aluminum

Titanium

Cast Iron

Aluminum

Diamond

Stainless

Diamond

Aluminum

Diamond

Diamond

Similar threads