Drilling question .25 hole is not .25? why

[Rich05]

Drilling mild steel making 1/4 holes and 3/8 holes it seems the holes are allways a bit oversized.

The bolts have a bit of slop in them. If I want a tight fit for a 1/4 shoulder bolt to slide through should I be using a smaller drill? Does the hole come out a bit wider due to vibration/chip removal?

Going through about 1" of steel the shoulder bolts have threads on the exposed end. Using a CNC machine to drill the holes, new carbide drills, very slow feed rates, and slow spindle speeds (300-500 rpm).

Thanks R.

[Crevice Reamer]

Have you checked your spindle & chuck runout?

CR.

[Geof]

How big is 'a bit'?

You can expect drilled holes to be oversize by up to 2% of the drill diameter, for a 1/4" drill this is 0.005".

If you are getting more than this, sayb 0.01" then the drill may not be sharpened well or the drill chuck/collet may be running out.

Also going slow can oversize the hole; you should be running at 3000 rpm, maybe even faster, and at least 10 ipm.

If you want to be daring and have a few parts and drills that can be sacrificed in a learning experience for 1/4" try something like 5000rpm and 20 or 30 ipm, but make sure everything is really flooded with coolant. Set your initial peck, I at about 0.4, J at 0.1 and K at 0.1.

EDIT:

If your really want a tight hole one way to do it is drill undersize by about .005 to .01, then take the 1/4" drill and dull the corners of the cutting edge very slightly, spin the drill and just touch the corners with some fine emery.

Now your 1/4" drill behaves like a rather dull reamer and does not cut oversize, it may even cut undersize slightly.

This is a bit of a hokey way to do it but it works; don't let the machine run unattended and make sure there is plenty of coolant. If the drill is 'dulled' too much there is a chance it will weld itself into the hole; you will have about a second of warning as the spindle load climbs and the drill makes a horrible squealing sound.....that is the time to hit Feed Hold then RESET.

[Rich05]

thanks for the advise, I will check the runout. basically that is the play in the spindle correct? Not sure If i know which meaurement that is.

I might have gone too slow 300 rpm at about 1-2 inch per minute feed rate with peck. I was using the quil manual mode just feeding it by hand.

[g-codeguy]

Originally Posted by Rich05 thanks for the advise, I will check the runout. basically that is the play in the spindle correct? Not sure If i know which meaurement that is. I might have gone too slow 300 rpm at about 1-2 inch per minute feed rate with peck. I was using the quil manual mode just feeding it by hand.

Even without flood coolant, you should be able to double that RPM. Should be able to run about 1070 RPM with flood coolant. That is 70 SFM.

EDIT: You are center drilling them, aren't you? Yeah, I know, stupid question.

[DareBee]

As Geof was more or less getting at, drill them 1/64 under and ream them. Center drilling is also required for accurate hole making.

[Palerider]

I have had excellent results drilling in steels with solid carbide drills, and obtaining near reamed hole results. In fairly high production use results can be obtained which are no less than amazing. I use top quality coated solid carbide drills from companies such as CJT, Gurhing, Iscar. Additionally there are resources avalabe online for proper speed and feed calculation which are very good.

With that being said: Rigid setups and tight equipment are necessary for these drills to work properly.

If you need tight location on those shoulder bolts and are not doing hundreds or thousands of holes the drilling/reaming option is most cost effective as these carbide drills are not cheap.

[Palerider]

Whoops, I forgot one thing.

Do Not spot drill your holes before drilling with a solid carbide drill made for drilling steel. Premature wear and early failure will result.

[Mike Stevenson]

Originally Posted by Palerider Whoops, I forgot one thing. Do Not spot drill your holes before drilling with a solid carbide drill made for drilling steel. Premature wear and early failure will result.

Has no one here ever taken an apprentiship from a master machinist? The old timers know to always spot drill before you drill a hole. Fancy tools and exotic tool materials will never replace the wisdom of these masters.

[Geof]

I think there is some validity in the advice against spotting before using a carbide drill.

It is not really necessary because carbide drills are much stiffer than HSS, they should be mounted in collets running as near perfect as possible and they are normally shorter than HSS drills, so they do not tend to wander as b adly on entry; which is really the only reason for spotting.

If spotting drills were available with exactly the same tip angle as the carbide drills, and I have not encountered them yet, it would not be as harmful to spot. However when something like a standard 90 degree spot drill is used when the carbide drill hits the spotted depression its first contact is at the periphery because the carbide tip is not 90 degrees. This can cause a brief instant of chatter and chipping right at the periphery of the carbide drill. When the spotting drill is not used the carbide hits at the center, on its web, is stabilized and then the cut progresses along the cutting edge in a sgradual manner

[Palerider]

The rigidity of a carbide drill in a rigid holder, combined with the split point design eliminate (in most situations) the need to spot drill for location with a solid carbide drill made for drilling steel. Moreover the point angle of these drills (Typically 140Deg To 150Deg) will cause the drill undue stress at two points on the cutting edge when entering spot drilled surface with a lesser angle which results in a chattering action which will chip the drill.

My recommendation comes from results I have obtained using the instructions laid out by the manufacturers of these tools.

[Geof]

Palerider; Beat yah.

And I even used more words; I must have started earlier given my two fingered typing speed.