What's new
What's new

Deep (5.5xD) holes with coolant-thru drill in turning center

Oldwrench

Titanium
Joined
May 21, 2009
Location
Wyoming, USA
Back in 2017 Matt@RFR posted this:

We run a 10mm 10xD Mitsubishi TSC drill in 4140PH at 375 SFM and .010 IPR. 3" thru, no peck, no spot, 300psi. One drill is good for about 600 of those parts. They'll go much faster, just depends on your tool life needs.

I found Matt's really clear and specific recommendation with a PM search. We are ordering two turning centers with 290psi coolant to drill .3906 blind holes 5.5xD deep in 41L42 and not have to peck. We'd have to use an 8xD drill (MWS03906X8DB) because I can't find anything between 5xD and 8xD.

Reading the directions in the Mitsubishi coolant thru drill catalog, they seem pretty adamant about using a 2-3xD guide hole using a flatter point (MZS03906MB), slowing down near the bottom and then again prior to leaving the hole. Now I totally get the need to slow down to protect the corners of a carbide tool from vibration-induced chipping, but a guide hole would require a second coolant-thru drill and would occupy another turret station already committed to another tool.

Trueness is not awfully important, but we do need to hold the runout to no worse than an ordinary drill starting in a 90° spot. Since the thru-coolant carbide drill would be a lot stiffer than HSS, could we just start the hole from a faced end with maybe a very small spot just to make sure it doesn't start on a tit?

I have to wonder whether applying TWO expensive drills will really end up with a lower cost per hole over several thousand parts, versus our current peck method with HSS drills and external coolant. Can Matt or anyone chime in with experience relevant to this? Thank you.
 
Back in 2017 Matt@RFR posted this:



I found Matt's really clear and specific recommendation with a PM search. We are ordering two turning centers with 290psi coolant to drill .3906 blind holes 5.5xD deep in 41L42 and not have to peck. We'd have to use an 8xD drill (MWS03906X8DB) because I can't find anything between 5xD and 8xD.

Reading the directions in the Mitsubishi coolant thru drill catalog, they seem pretty adamant about using a 2-3xD guide hole using a flatter point (MZS03906MB), slowing down near the bottom and then again prior to leaving the hole. Now I totally get the need to slow down to protect the corners of a carbide tool from vibration-induced chipping, but a guide hole would require a second coolant-thru drill and would occupy another turret station already committed to another tool.

Trueness is not awfully important, but we do need to hold the runout to no worse than an ordinary drill starting in a 90° spot. Since the thru-coolant carbide drill would be a lot stiffer than HSS, could we just start the hole from a faced end with maybe a very small spot just to make sure it doesn't start on a tit?

I have to wonder whether applying TWO expensive drills will really end up with a lower cost per hole over several thousand parts, versus our current peck method with HSS drills and external coolant. Can Matt or anyone chime in with experience relevant to this? Thank you.

You need to use the same point angle on your spot as your drill with carbide. OR maybe eliminate the spot and use a stubby 2xD drill as a pilot? Unless you need the spot tool for other stuff. No idea about your tool life or which is better, but if the spot angle doesn't match it will cause problems...

edit: I would not start a 8x drill without a pilot or bare minimum a spot, carbide or not
 
We use a lot of the the MWS drills from Mitsubishi in the lathe and I've found their catalog isn't the best reference at times. I would either call their tech line or see if there is a Mit rep n your area and see what they say about pushing the 5xD that extra .2" that you need. I've had pretty good luck with calling them in the past.
 
You have to spot drill one way or the other, right? No way would I try to start an 8xD drill without something already there. So instead of spot drilling with a spot drill, spot drill with a stubby .3906" drill that has the same tip angle as your 8xD and go 1/2-1 diameter deep. Still only 2 tools, but you get a good piloted hole then run the long drill.

Regards.

Mike
 
If its in a lathe just do your own drilling without a canned cycle. Drill 5x deep. Then back out maybe .01" and drill 1/4 more deep. Then back out .01" and drill 1/4 more deep. Just for a little safety when getting that deep. Most coolant thru drills have a long washout when they grind the flute. Meaning flute length may be 3" but the gash doesn't totally finish until 3.5 or 3.6 inches.

Since we are talking about Mitsubishi drills, I don't know what magic dust they sprinkle in the carbide or in the coating but I get incredible tool life. I've literally drilled thousands of holes in 8620 steel and could not see any wear whatsoever. I run it conservatively but still I am very impressed. I dont sell them so I am not biased. Just saying, they rock !!!!
 
Try Iscar's SumoCham with the HCP-IQ cutting head. They promote running them up to 12XD without even spotting. (BTW, I am not involved with Iscar:D) I have also used Kennametal's KenTip FS drill in .375" dia. at 8XD without spotting with excellent results. Kennametal is slightly cheaper than Iscar ($200 for the body; $50 per tip). The main thing is, you need a point designed to center with such a long drill body.:typing:
 
We use a lot of the the MWS drills from Mitsubishi in the lathe and I've found their catalog isn't the best reference at times. I would either call their tech line or see if there is a Mit rep n your area and see what they say about pushing the 5xD that extra .2" that you need. I've had pretty good luck with calling them in the past.

This.

I worked closely with a really good Mits rep for a few years. We ran into this a couple times before it just became default. If the size down has at least the flute length you need plus a little bit extra, you're good. Based on what the flute length of that 5X is I think you'd be fine going with that alone.
 
Also it drives me crazy. One vendors 5x drill has a different flute length than another vendors 5x drill. Same diameter. 5x is not 5x. Anyone else notice this???
 
I drill an .874” hole 4X deep in 4140 every day in a Takisawa lathe with an Iscar SumoCham (coolant thru). No pecking, no spot, but faced of course. I think we start a little slower then go for it. Thousands of holes. Two advantages to those replaceable-tip drills is 1) the tips are cheaper than buying a solid-carbide drill and 2) much easier to swap out...just twist the tip off and put a new one on...no need to touch off or even take the tool out.

I’ve never tried Mitsu drills but have heard they are amazing. Definitely look into the replaceable-tip design, though, from whoever you decide to go with!
 
For anything under 5/8 I almost always go with solid carbide. steel bodies that small are always kinda weak and unless drilling less than 3x diameter tend to walk too much. 3/4 and larger than solid carbide is just too much money.

For steel bodies and carbide tipped I like the Mitsubishi TAWNL style. Great tool life, almost never centerdrill. I always peck.
 
I drill an .874” hole 4X deep in 4140 every day in a Takisawa lathe with an Iscar SumoCham (coolant thru). No pecking, no spot, but faced of course. I think we start a little slower then go for it. Thousands of holes. Two advantages to those replaceable-tip drills is 1) the tips are cheaper than buying a solid-carbide drill and 2) much easier to swap out...just twist the tip off and put a new one on...no need to touch off or even take the tool out.

I’ve never tried Mitsu drills but have heard they are amazing. Definitely look into the replaceable-tip design, though, from whoever you decide to go with!

4x on a .874" drill is still pretty sturdy IMO. OP wants a .391"(?) at 5.5x. I would think that diameter (.874") would be stout enough (as you posted) to not need a spot or start hole.

Wait a minute... 5.5x is less than 2 1/4"... 8x would be about 3 1/8".... :willy_nilly: Sorry in my head I was thinking something different...

carry on :leaving:
 
Wait a minute... 5.5x is less than 2 1/4"... 8x would be about 3 1/8"....

Yes, the problem is: The part has a 7/16 hole .700 deep, then a 25/64 hole to about 2.9 deep. From the bottom of the 7/16 hole to the bottom of the 25/64 hole in question is about 5.63 drill diameters—IOW, likely more than a 5xD drill is rated for. The flutes would be obstructed unless we pecked it, and the whole point of a coolant-thru drill is to eliminate pecking. I can't make that hole any shorter, nor the 7/16 hole any deeper. The next-up choice from Mits is 8xD. Wading thru other online catalogs to find a 6xD drill is mental torture, as so far they seem to be universally user-hostile. I guess I could always shorten it but, hellooo extra cost...

I could be overthinking this, but extra tool overhang makes me cringe. Thanks very much to everybody for their input.
 
Try CJT's drills... Solid Carbide Drills, Coolant Fed On CJT KOOLCARB Inc.
They still make their carbide drills in the traditional screw machine length and jobber length.

Mitsubishi drills are definitely good, as others have said. I've never tested CJT directly against Mitsubishi but have performed limited testing against Titex, Kennametal, and Guhring with CJT edging them out.
 
I’m with Frank on drilling 5xD in one shot and then a few short pecks to get to the end. If the drill isn’t live, consider building or buying a double station tool holder to hold your start drill and long drill. You can also do that with a live tool but $$$.
 
I've recently done a couple jobs in 304 with a 15mm 8D Kennametal replaceable tip drill where I didn't really have the turret space for a separate spot drill. So what I did is spot it with my rough turning and facing tool, which is a C shape insert in the most common -5 degree (95 degree I believe for the more ISO inclined) orientation. That gives you just enough clearance to angle your facing cut a couple degrees in at the appropriate location, which results in a ~175 degree spot. That doesn't sound like a lot, but it's enough. Just slow the feed down to half or so for the first little bit. Obviously you need your tool height pretty dead on for this to work.
 
Just take the drill and half the speed / feed and divot the top of the hole to act as a spot. Then drill at the supplied speed and feeds.
 
Just take the drill and half the speed / feed and divot the top of the hole to act as a spot. Then drill at the supplied speed and feeds.

I do this many times when drilling with a 5x or 8x carbide drill. The first .09" I reduce rpms maye 20-30% and i reduce the feed per rev by 50%. Drill will walk much less. Then I back away .01" and put rpms and ipt to what I want and start drilling. Works fine in most cases. Great time saver.
 








 
Back
Top