Coolant through drills real world speed and feed

Captdave · Feb 1, 2017

Was looking through several of the high end solid carbide coolant through drills and third recommended speeds and feeds for 6061 material.

For example, 3/8 drill running 10,000 rpm and 100 - 120IPM seems pretty common across several suppliers but what kind of tool life are going to get at that speed?

1/2 a second per hole as opposed to 3-4 seconds spread out over thousand of holes per week is pretty appealing

Currently we're using colbalt drills drilling .850" deep 3000 rpm 30 IPM with 2 pecks and swap them out at 5,000 holes for Sharpning.

Jashley73 · Feb 1, 2017

Captdave said:
Was looking through several of the high end solid carbide coolant through drills and third recommended speeds and feeds for 6061 material.

For example, 3/8 drill running 10,000 rpm and 100 - 120IPM seems pretty common across several suppliers but what kind of tool life are going to get at that speed?

1/2 a second per hole as opposed to 3-4 seconds spread out over thousand of holes per week is pretty appealing

Currently we're using colbalt drills drilling .850" deep 3000 rpm 30 IPM with 2 pecks and swap them out at 5,000 holes for Sharpning.

Although you didn't say what diameter your holes are, that's pretty good performance. Yeah, you may be able to go faster with carbide, but I would honestly have to break out the spreadsheet, to see if a carbide drill would actually be better/cheaper for you - And I sell carbide drills...

If you had hi-silicon aluminum, carbide would be better. If you had to drill a gazillion holes in wide-open production, then carbide would be better. If you had to go super deep, and needed coolant-thri, then carbide would be better.

But in a job-shop or low volume environment, what you're doing is going to be hard to beat.

Captdave · Feb 1, 2017

We have our own product line and drill/tap ~ 2,000 3/8-16 holes per week.

D Nelson · Feb 1, 2017

You also don't get aluminum all twisted around the bit .5 drill 1.5 deep 25 holes is 40 seconds all day long. Drill bit life is probably 6 months before resharpening

Sent from my iPhone using Tapatalk Pro

Mickey_D · Feb 1, 2017

One of the parts that we run regularly are gauge blocks and have drilled a little over 2 million stepped holes in 6061. Holes run from .359" to .485" and between one and two inches deep. Almost all of the drills that I use are Mitsubishi coolant through and run at around 6500 rpm and 60 to 70 IPM and 500 psi of Blaser 2000 Universal at around 8% concentration. I get about 3000 to 5000 feet of hole between sharpenings. I know that I could run a little faster but when I try I have ended up with chip marring in the holes, plus, knock on wood, I have not had a drill failure that would bork up some expensive reamers and facemills. Right now we are doing about 6000 holes per day.

zero_divide · Feb 1, 2017

Captdave said:
Was looking through several of the high end solid carbide coolant through drills and third recommended speeds and feeds for 6061 material.

For example, 3/8 drill running 10,000 rpm and 100 - 120IPM seems pretty common across several suppliers but what kind of tool life are going to get at that speed?

1/2 a second per hole as opposed to 3-4 seconds spread out over thousand of holes per week is pretty appealing

Currently we're using colbalt drills drilling .850" deep 3000 rpm 30 IPM with 2 pecks and swap them out at 5,000 holes for Sharpning.

I made a video of drilling 0.25" hole 2.0" deep at 10000 rpm and 150ipm.....
In one shot. Cut a 2 hour drilling job to 20 minutes.

Drills were parabolic HSCO Dormer no-coolant through. Just flood.

I am really sorry I lost it somewhere becauase nobody believes me when I tell.

Bigtoy302 · Feb 1, 2017

M.A. Ford Twister AL 5x. 3 flute no peck just flood. Much cheaper than coolant through. I use several of them.

Tonytn36 · Feb 2, 2017

I don't run anything that big, but the Walter Ø3.0 mm coated carbide thru coolant drills we switched to are running around 320,000 holes 1/2" deep no peck. 15k rpm / 3400 mm/min feed. These are in the $80-$90 range price wise. That is $0.00028 / hole which is _very_ inexpensive.

dodgin · Feb 2, 2017

Mickey_D said:
One of the parts that we run regularly are gauge blocks and have drilled a little over 2 million stepped holes in 6061. Holes run from .359" to .485" and between one and two inches deep. Almost all of the drills that I use are Mitsubishi coolant through and run at around 6500 rpm and 60 to 70 IPM and 500 psi of Blaser 2000 Universal at around 8% concentration. I get about 3000 to 5000 feet of hole between sharpenings. I know that I could run a little faster but when I try I have ended up with chip marring in the holes, plus, knock on wood, I have not had a drill failure that would bork up some expensive reamers and facemills. Right now we are doing about 6000 holes per day.

We just switched one production job we have over to Mitsubishi solid carbide drills. Running about 450-500 SFM and .012 IPR, which with those drills is about 6k RPM and 60 IPM (in mild steel). Sales rep wouldn't guarantee us any numbers, but he estimated we might start seeing wear around 10k holes. Nice thing about the Mitsubishis is that they'll take them for regrind pretty much as many times as you have an intact drill to send. The Sandvik rep told us 3 regrinds max and then you're on your own after that.

Mtndew · Feb 2, 2017

Captdave said:
Was looking through several of the high end solid carbide coolant through drills and third recommended speeds and feeds for 6061 material.

For example, 3/8 drill running 10,000 rpm and 100 - 120IPM seems pretty common across several suppliers but what kind of tool life are going to get at that speed?

1/2 a second per hole as opposed to 3-4 seconds spread out over thousand of holes per week is pretty appealing

Currently we're using colbalt drills drilling .850" deep 3000 rpm 30 IPM with 2 pecks and swap them out at 5,000 holes for Sharpning.

I wouldn't even think twice about it. Get a coolant thru carbide drill for those and don't even look back.
Besides at $150 (before any discounts) you have nothing to lose.3/8 Inch, 14 Degree Drill Point Angle, 9858986 - MSC

1015SFPM and .02" IPR will make quick work of those holes.

Lastu · Feb 2, 2017

Mtndew said:
I wouldn't even think twice about it. Get a coolant thru carbide drill for those and don't even look back.
Besides at $150 (before any discounts) you have nothing to lose.3/8 Inch, 14 Degree Drill Point Angle, 9858986 - MSC

1015SFPM and .02" IPR will make quick work of those holes.

Those are some nice drills for sure!
But DAMN at those prices, we can get the same drill for $42, buying from our Guhring rep..

thesidetalker · Feb 2, 2017

Captdave said:
We have our own product line and drill/tap ~ 2,000 3/8-16 holes per week.

Sounds like you got nothing to lose on this one. Drill would pay for itself in the first week and last way beyond that.

Mtndew said:
I wouldn't even think twice about it. Get a coolant thru carbide drill for those and don't even look back.
Besides at $150 (before any discounts) you have nothing to lose.3/8 Inch, 14 Degree Drill Point Angle, 9858986 - MSC

1015SFPM and .02" IPR will make quick work of those holes.

These are what I buy. 5510 and 5511 series. Works great in our (job)shop. Over time got all the drill/tap sizes + various others. Sure saves a lot of time drilling 5x or more faster, and no pecking. I run the recommended speeds and haven't had issue.

Mtndew · Feb 2, 2017

Lastu said:
Those are some nice drills for sure!
But DAMN at those prices, we can get the same drill for $42, buying from our Guhring rep..

That's crazy! We typically get 15% -35% off of MSC's price,but getting that drill for $42 is amazing as we could get that for about $95. I wonder if it has to do with shipping overseas to the U.S.?

Jashley73 · Feb 2, 2017

Captdave said:
We have our own product line and drill/tap ~ 2,000 3/8-16 holes per week.

Are these holes thru or blind? How deep?

BROTHERFRANK · Feb 2, 2017

The Guhring 5514 is great in 6061 Aluminum. It's funny that Guhring doesn't list it in their drills for Aluminum recommendations but if you look at the feeds and speeds page for the 5514 it recommends 805 SFM, .016"/Rev for .25" Dia.. I think feed per Rev is somewhere around .010" for .125" Dia.. I know a shop that drills about a million holes a year in 6061, .200" Dia., .600" deep, no pecking, no coolant thru, 14000 rpm, 175 IPM. The holes are really nice and the drill makes tiny chips you can hear hitting the sheetmetal.

Mtndew · Feb 2, 2017

BROTHERFRANK said:
The Guhring 5514 is great in 6061 Aluminum. It's funny that Guhring doesn't list it in their drills for Aluminum recommendations but if you look at the feeds and speeds page for the 5514 it recommends 805 SFM, .016"/Rev for .25" Dia.. I think feed per Rev is somewhere around .010" for .125" Dia.. I know a shop that drills about a million holes a year in 6061, .200" Dia., .600" deep, no pecking, no coolant thru, 14000 rpm, 175 IPM. The holes are really nice and the drill makes tiny chips you can hear hitting the sheetmetal.

Yep, same as the drill I linked, with the exception of being coolant thru.
I rarely buy a carbide drill that isn't Guhring brand, and if I do, it's usually OSG.
I'm not saying that Walter and Mits aren't good, it's just that I haven't used them much in the past.

Captdave · Feb 2, 2017

Jashley73 said:
Are these holes thru or blind? How deep?

Blind holes .850" deep.

thesidetalker · Feb 2, 2017

Don't forget about some of those 3-flute drills people are makin'

Someone posted a video on here not too long back. Can't remember the mfg of the drill, but it was doing cast iron at 600 ipm? Had to get a running start of several inches to get to that speed haha

Mtndew · Feb 2, 2017

thesidetalker said:
Don't forget about some of those 3-flute drills people are makin'

Someone posted a video on here not too long back. Can't remember the mfg of the drill, but it was doing cast iron at 600 ipm? Had to get a running start of several inches to get to that speed haha

It was probably a video of the OSG Mega Muscle drill. Crazy feedrates indeed.

Mtndew · Feb 2, 2017

Here's a hole I did in some 4140 Annealed.
1/4" Guhring 20xD drill going 5-1/4 deep no pecking.
Deep hole drill - YouTube

Coolant through drills real world speed and feed

Titanium

Titanium

Titanium

Stainless

Stainless

Stainless

Cast Iron

Diamond

Hot Rolled

Diamond

Plastic

Stainless

Diamond

Titanium

Stainless

Diamond

Titanium

Stainless

Diamond

Diamond

Similar threads