Thread: Feeds on a standard drill bit

Originally Posted by gcodeguy

Apparently you didn't read my post very carefully. I said "the feeds and speeds the tech gave me for drilling on a lathe were greatly reduced". The catalog called for 375 SFM while the tech told me to run at 200 SFM on the lathe (spindle turning, not live tooling). I think his suggestion for the feedrate was to lower it from F.006 to F.002, but not positive as that was over a year ago.

That wasn't the part I was commenting on. It was this:

[QUOTE One of the high performance drill catalogs specifically mentioned that the SFM and feedrates were for mills and live tooling on lathes only. ][/QUOTE]

If the sfm and feedrates were for mills and live tooling on lathes only, then it's sort of implying that it would be different on a lathe without live tooling, no?
In other words, I'm wondering why they would specify that feed and speed only on certain applications, as if it wouldn't work in all applications.

Originally Posted by ewlsey

You are confusing the machinability rating with the power constant. Machinablility is a percentage that is compared to a reference material (mild steed). It really has no meaning other than telling you that some materials are harder to machine than others.

The power constant is the amount of power required to remove a given volume of material.

MAPAL Drilling Calculator

ok interesting web site
at 4.8 cubic inches per min removed at 70% drive efficiency and at PF of .81 thats 5.49 hp (i said 6hp)

........ yes drive efficiency % i had at 70% as most times hp is absorbed by gearbox and belts. i have rarely seen a 3 hp motor end up with much more than 2 hp at cutting tool. At high rpm >1000 i usually see better drive efficiency compared to say 400 rpm with a 1750 rpm motor
........ my point is i was taught a 1" drill needs roughly 3hp but if feeding a drill it at 2x higher feed then that is 6 hp needed. on a Series 1 Bridgeport mill even if with a 3 hp motor at anything much more than 1 hp i usually get vibration, chatter, motor drive noise etc......... you could put a 10hp motor on a Bridgeport but structurally it basically don't like much over 1 hp. The extra 2 hp are for if geared down to say 100 rpm you got extra hp for a very inefficient drive. but the structural iron of the mill (and the vise) can only take so much force
..... for me i usually do it the other way i put in a MR for common steel of 0.8 cubic inches per min per hp and adjust the MR number say 0.7 or 0.9 til calculator gives me speed, feed, with mill depth of cut etc. For example with 304 Stainless I get a MR of 0.2 to 0.4. My Excel calculator and cutting tests on a mill easily picks up that some cold rolled work hardened thin stainless is closer to MR 0.2 and some thicker annealed Stainless is closer to the MR of 0.35 to 0.4 commonly given for 304 stainless. I do cutting tests and adjust the estimated MR number according to mill testing results
...... Basically I perform milling tests that gives me a comparative MR number for depth of cut , feed, etc and I adjust MR number as charts of MR numbers normally say +/- 50% probably because motor drive can be tough to figure efficiency 60-90%

Originally Posted by Dave K

That wasn't the part I was commenting on. It was this:

[QUOTE One of the high performance drill catalogs specifically mentioned that the SFM and feedrates were for mills and live tooling on lathes only. ]

Originally Posted by Dave K

If the sfm and feedrates were for mills and live tooling on lathes only, then it's sort of implying that it would be different on a lathe without live tooling, no?
In other words, I'm wondering why they would specify that feed and speed only on certain applications, as if it wouldn't work in all applications.

Ok, I see your meaning. The reason it is different was stated by "winterfalke". Lathe drills are seldom on center. Carbide doesn't like being off center. Drill slower, and you can still make a hole as long as it isn't too far off center and the drill is big enough. Although feedrate remains same regardless of SFM (at IPR), tool pressure doesn't. Thus the tech's suggestion for lower feedrate AND sfm.

Ok, now that makes sense.

In a previous life, I hired a new guy...well not a new machinist, but new for us. He told me for 1018, 100sfm and 6"/min feed - I thought that seemed nuts that you could use the same feed rate for all sizes, but alas, it does work pretty well for Q&D drilling . Most times I'll drop to 80 sfm and 5"/min if it's just a few holes, but anytime there is a bunch of holes, insert drills are as noted before, the cat's PJ's.

In really soft steel (similar to A36) and deep holes (5xD) with an insert drill we will actually increase sfm to 1,200 and drop to the lower range of the recommended feed to help "float" the chips out (on a vmc). I have also had to increase sfm on T304 plate to get the chips to break...in essence, get the chip really hot and thermally shock them to get them to break...900 sfm makes the chips come out glowing red - just keep the lights on inside the cabinet or you'll be too scared to watch the fireworks .

I was thinking of Mitty the other day, so in memory of him, I threw in as many emotioncons as possible. RIP Mitty.

Steve

Although it seems "counter-intuitive", ... the heavier chips generated by higher feed rates, actually helps "carry" the heat away from the tool.


.

I suddenly got buried in work, so I never did get a chance to just play with feed rates on drills, but I still plan on it. I will post my results.

Originally Posted by SteveinAZ

I was thinking of Mitty the other day, so in memory of him, I threw in as many emotioncons as possible. RIP Mitty.

Steve

I loved that guy's posts, you knew he very likely was going to say something that would make you laugh.

Not to mention the occasional pics of the local hotties that he was likely charming to death and would would sneak in a snap shot of every once in a while (I still remember the one of his metal supplier).

Mitty, I'm sure your making chips on some of the coolest machines and cracking everybody up up there in machine shop heaven, sprinkle some chips down on us every once in a while.

Paul T.
Power Technology

I got an education from this thread. I drill a lot of holes in 6061 plate 1-2" deep, HSS 118 drill bits. I was following the book feeds and had stringy chips and had to peck to keep things cool. I played with the feed and stopped pecking altogether, feed went up 1000% in some cases and absolutely everything is working better. The chips are broken up and a part that used to run 45 minutes takes 4 minutes now.

Drilling sounds better now. Light feeds and pecking had a lot of ringing (rubbing) and I was just used to hearing it.

One of my first CNC jobs was drilling a bunch of deep holes in 4340 with standard HSS tools. I was forced to peck frequently and stay around 30 SFM to get any sort of tooling life at all. I sharpened a lot of drills and cut a couple twisted off bits out with carbide endmills. It made me overly cautious about drilling.

Originally Posted by PaulT

I loved that guy's posts,
Not to mention the occasional pics of the local hotties that he was likely charming to death and would would sneak in a snap shot of every once in a while (I still remember the one of his metal supplier).

Paul T.
Power Technology

I almost forgot about that! She was hot as hell! Mitty was my kinda guy!

The chips are broken up and a part that used to run 45 minutes takes 4 minutes now.

Slight improvement, huh? Isn't it amazing how one of the most basic operations of machining, (drilling a hole), has been overlooked by so many of us? What a time saver. I am so glad I wasn't too embarrassed to ask this question of such basic fundamentals. I would have never guessed a drill could handle such loads.

As a side note, I recall once that wanted a drill to run at 2 inches per minute. Somehow, when I programmed it, I fat fingered it at 20.0 inches per minute. Needless to say, I about crapped my pants when it drilled that first hole. The first thing that went through my mind was that I forgot a feedrate altogether, and it went at a rapid feed, but then I saw it later as I checked my program. Anyway, to my surprise, the drill survived, and drilled the hole through the part. It was a thin part, but still, it had some awfully thick chips in the flutes when it was done. Even though that feedrate was beyond too fast, it should have given me a clue that I've been babying drills for years.

Originally Posted by Garwood

The chips are broken up and a part that used to run 45 minutes takes 4 minutes now.

Drilling sounds better now. Light feeds and pecking had a lot of ringing (rubbing) and I was just used to hearing it.

Awesome.

Out of curiosity, how about milling?

Ill bite on that one. Drill spinning and chips get thrown against od of hole, hence flute spiral drags them out more efficiently. Part spinning, drill stationary and the chips will sit there on the drill - Hole bottom only to be moved by vibration and more chips pushing against them. Some of that is offset by being a horizontal - not vertical process.

Myself, im really growing to like cobalt Hss drills. I never see anything nasty enough to warrant carbide - or have the machinery to run carbide drills. They just hold up so much better in nasty stainless than normal - good plain Hss does. Whats more i can happily tweak them + sharpen them on a std bench grinder.

Originally Posted by Metalcutter

Standard drills Screw machine length. The chip load for a drill is .016 times the drill diameter per flute.
Both flutes is about 3% of the tools diameter. Now... Multiply that by the rpm = feed rate in inches per minute.

Quick and Dirty... @ 3000 rpm the feed rate for a drill is the decimal equivalent times 100. .250 diameter drill would be 25 inches per minute. If the rpm is 300 then that drill would be feeding 2.5 inches per minute. And if the rpm was 600, then 5 IPM.


This is good for most all materials which are strong enough to support the drilling process. OFHC Copper has trouble drilling and needs to be fed at about 1/3 the rate.

It's petty much all proportional.

Regards,

Stan-

I just want to thank you for posting your formula here. I have been under-feeding my drills in my cnc's worse than I could have imagined. You have helped me to cut my cycle times by 1/3 on some of my parts.

Originally Posted by allen mullis

I just want to thank you for posting your formula here. I have been under-feeding my drills in my cnc's worse than I could have imagined. You have helped me to cut my cycle times by 1/3 on some of my parts.

And I also want to thank Stan for the drilling formula that I read on the internet about 12 years ago. I remember when I first used the quick and dirty 3kRPM-move-the-decimal-over-two-places-and-that's-your-feed method. I was scared to turn the feed rate overide up to 100, but I did, and it worked great, and it's been working great since. I even printed the essay Stan wrote, and it sits in my file cabinet in case I become senile and can't remember the impossibly simple formula.

I routinely see experienced machinists posting basic questions about drill feeds and it makes me think there should be a sticky with Stan's essay. Who do we have to petition for that?

QB

And I also want to thank Stan for the drilling formula that I read on the internet about 12 years ago.

Is this something you could easily post, or is it repeat of what's already been posted?

Originally Posted by Question Boy

And I also want to thank Stan for the drilling formula that I read on the internet about 12 years ago. I remember when I first used the quick and dirty 3kRPM-move-the-decimal-over-two-places-and-that's-your-feed method. I was scared to turn the feed rate overide up to 100, but I did, and it worked great, and it's been working great since. I even printed the essay Stan wrote, and it sits in my file cabinet in case I become senile and can't remember the impossibly simple formula.

I routinely see experienced machinists posting basic questions about drill feeds and it makes me think there should be a sticky with Stan's essay. Who do we have to petition for that?

QB

Thank you QB, very nice of you to write. Twelve years is pretty good validation. Glad you're here,
and I'm happy to have helped.

I don't know when you stepped into this thread, but on the first page my second post down, outlines the experiment where this formula came from, if you wondered how it came to be.

Best regards,

Stan-

Originally Posted by zero_divide

Unfortunately that neat formula (.016" per Each inch of dia- no irony, i'm using 0.013" per inch ) works only for aluminum and other soft materials.

Try feeding any drill into a pre-hardened steel like that and quickly learn that the feed needs to be adjusted "accordingly".
Its possible to remember this next time. but add couple of other materials and stuff gets quite bulky and not so easy.

Off Topic: I am reducing Drill SFM by 1/2 from that specified for milling on same materials. Just based on the fact that drills' flutes spend all the time in the cut. Unlike end mills that at best only spend half a revolution cutting. Anyone else doing that?
I find that this reduces drill wear to almost nothing. (matters to me since i don't look at machines running)
The other day i drilled 50 2" deep 3/8dia holes in O1 with regular jobber and drill looked like new.

Eldar

Just caught this Eldar..

Actually the .016 is % of tool diameter per flute. I don't remember if I miss quoted it. Sorry if I did.

I don't know if you saw it, but I used this formula to drill a .013" hole 12 diameters deep in 316 SST.
I don't mind saying I was surprised it worked. I haven't tried Inconel yet.

Regards,

Stan-

Originally Posted by Metalcutter

Just caught this Eldar..

Actually the .016 is % of tool diameter per flute. I don't remember if I miss quoted it. Sorry if I did.

I don't know if you saw it, but I used this formula to drill a .013" hole 12 diameters deep in 316 SST.
I don't mind saying I was surprised it worked. I haven't tried Inconel yet.

Regards,

Stan-

Do try and tell me the results. seriously.
My material experience is limited by 6061 aluminum , A36 and 55RC pre-hardened steels.

But one example why 0.016 ipt per 1" of dia does not fit all is here:

Had to drill a .281Dia hole in 55RC Hardox 500 plate.Used carbide straight flute drill and went:

RPM: 796
APT:0.001 in/tooth
Feed: 1.72 in/min

Drill frigging broke!!!! almost instantaneously.

Reduced chipload to 0.0006 and managed to drill all 60 .750" deep holes with it.

I am always using .013" per flute per dia on T6061
and 0.00454" per flute per inch for mild and SS steels.

Anything harder requires substantial feed rate reduction. I know you guys don't believe in calculators but mine at least puts me in the ball park.
IE: the other day i was drilling a 5/16 10" deep hole in T6. calculator came up with 3900RPM and 35 IPM knowing the hole is deep i reduced feedrate to 30.
On the very first hole drill almost clogged up. Increased feedrate to recommended 35 and stuff sounded wonderful.

Anyway efficient pecking saves much more time that more aggressive feedrate.

Originally Posted by zero_divide

Do try and tell me the results. seriously.
My material experience is limited by 6061 aluminum , A36 and 55RC pre-hardened steels.

But one example why 0.016 ipt per 1" of dia does not fit all is here:

Had to drill a .281Dia hole in 55RC Hardox 500 plate.Used carbide straight flute drill and went:

RPM: 796
APT:0.001 in/tooth
Feed: 1.72 in/min

Drill frigging broke!!!! almost instantaneously.

Reduced chipload to 0.0006 and managed to drill all 60 .750" deep holes with it.

I am always using .013" per flute per dia on T6061
and 0.00454" per flute per inch for mild and SS steels.

Anything harder requires substantial feed rate reduction. I know you guys don't believe in calculators but mine at least puts me in the ball park.
IE: the other day i was drilling a 5/16 10" deep hole in T6. calculator came up with 3900RPM and 35 IPM knowing the hole is deep i reduced feedrate to 30.
On the very first hole drill almost clogged up. Increased feedrate to recommended 35 and stuff sounded wonderful.

Anyway efficient pecking saves much more time that more aggressive feedrate.

Ok..Zero_divide..

You've referenced my Post to ask a question. I'm 2 decimals off. I'm also OLD and get confused from time to time.

The chip load percentage is 1.6% of the drill diameter per flute. I'm quite sure of this, because I also say for both flutes taken together it's pretty close to 3% of the drill diameter. I guess I must have had another Senior moment. Please forgive me.

So on a 1" diameter drill the chip load should be near .030" per revolution including both flutes. Your
machine, of course, needs to be sturdy enough to work the drill.

Thank you for being patient. I really don't like leaving bad information. Some of this stuff is confusing enough without me adding to it. *sigh...

Best regards,

Stan-