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.

Have you checked your spindle & chuck runout?

CR.

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.

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.

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. :D

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.

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.

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.

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.

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

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.

Palerider; Beat yah.:D

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

I was glad to see that someone more eloquent than myself had taken the cause of truth.

rich05 said the holes were comming out oversized. What I suggest is to Spot one hole and drill it with the proper feeds and speeds using a Cobalt drill and see how the size comes out. Not sure if Carbide is your best choice for drilling mild steel.

Absolutely.

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.

For the sake of being complete:

Runout:

Runout is not exactly the play in the spindle , it is how precisely your holder, drill chuck or collet, holds the tool so the centerline of the tool coincides with the spindle centerline.

When the drill is not held on center the tip of the drill is actually going around in a small circle; this is easier to visualise if you imagine the drill being a long way off center.

When the off center drill enters to workpiece it does not enter at a point that is on the centerline of the spindle, it enters where it first hits and drills the hole there. The result is that the hole is tapered, larger at the entry, because the drill is flexing as the spindle rotates it off center.


Carbide drills fed by hand:

Don't do it.

If you can only hand feed use HSS.

Carbide has to be run fast and fed fast, and more importantly fed at a constant rate for best results.

Geof,

Should you Spot or center drill before you use that HSS drill?

i agree that spot drilling before drilling with a carbide will destroy the drill , also a carbide drill that is not dialed in within a couple tenths will also face very rapid premature breakdown , which will obviously vary depending on the material

one question i have is what kind of quality are the 1/4" drills , if they are of mediocre quality then chances are they may not be ground properly on center straight from the manufacturer and no matter what you do , you will never get a proper hole from that drill

Geof,

Should you Spot or center drill before you use that HSS drill?

Yes. (although the answer could be it is not essential if the drill is a stubby and you wanted to save a tool change.)

HSS drills are not as precise as carbide and even if the drill is held in a collet the tip may be wandering because the drill is not straight; spotting makes a starting point that is pretty well exactly on the spindle centerline, the HSS drill aligns into this point.

The drill tip angle is different to the spotting angle and if you feed slowly you will hear the drill scream as the periphery hits the spotted depression, but HSS is much more forgiving than carbide and it does not chip.

I cross drill in 8620 with 1/16 in. carbide drill and no spot all the time. Cross drill 5/64 & 7/64 carbide drills thru the threaded section with no spot. Have had to use 7/64 HSS drills on occasion to drill thru the threads. Naturally these are stubby drills. I have on occasion used a center drill first for the HSS drills, and must admit to preferring to use the center drill.

I agree with the advice of not using a spot or center drill for a carbide drill, and using one for an HSS drill. Points on cheap drills can be really bad, though normally one that large isn't as bad as the smaller size drills. However, if it is cutting on one side only, you are going to have a hard time holding size. :)

Some people have a hard time understanding that cheap drills aren't the cheapest way to go...if you know what I mean. Drilling is one of the best places to cut cycle times. Sorry, but a Chinese drill ain't going to cut it! Even if you can find one that cuts on size.

Rich05,

What did you end up doing with this problem?

I cross drill in 8620 with 1/16 in. carbide drill and no spot all the time.

What brand of drill are you using?

What speeds and feeds do you use?

How deep and how many holes do you get from one drill?

Flat stock or cylindrical?

How many do you break?

You say the size is good but how about the True Position and the Metrics?

What is the hole size tolerance?

Spot drill, drill 15/64th, ream .250. End of story.

Spot drill, drill 15/64th, ream .250. End of story.

I agree. Ream and/or Bore if you require true cylindricty and position as well as ultimate size control. :D

You won't see me ramming unspotted CJT Carbide drills, regardless of size, into precision fixtures or round parts. That might be all the rage in the Production world but not for me.

i didn t realize those were meant to be precision holes , i suppose i'm in the habit that if it's marked fractional then the hole size is generally +-1/64 or some sort of open tolerance :)

speaking of carbides , garr makes a nice 3 flute carbide drill that works great on mild steel ,i used to use them on production parts with a tolerance of +.0005 , we'de run thousands of holes in 1018 with a 1/2" dia drill 1/2" deep with a nice finish , i honestly don t think people take enough advantage of those types of drills

I want a tight fit for a 1/4 shoulder bolt to slide through.

Not a lot of slop there. :)

oh ya there we go , wasn t paying attention to the shoulder bolt thing

Tight fit, little loose, wish I knew what was dimensionally needed.

Size, Roundness, and Cylindricity. :)

I am familiar with those terms. I always have numbers with which to associate them to our reality when called upon it make a hole.

I am familiar with those terms. I always have numbers with which to associate them to our reality when called upon it make a hole.


Indubitably. :D

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.

Check your bolts, too; I wouldn't be surprised if they're a whiff undersize.

[QUOTE=Mike Stevenson;474415]What brand of drill are you using? not sure of brand says Co. USA about $6.

What speeds and feeds do you use? about 2 ipm

How deep and how many holes do you get from one drill? 1" 8 holes
Flat stock or cylindrical? flat

How many do you break? bent one while alligning part..

You say the size is good but how about the True Position and the Metrics? no sure what this is.

What is the hole size tolerance? not sure .001? just so bolt is fairly tight



Mike I have not resolved it yet. just gave the fellow the parts. but need to know for the next time.

.001 tolerance?
You can't get much easier than drilling and reaming.