What's new
What's new

Recomended drill for inco 718

tay2daizzo8

Hot Rolled
Joined
Nov 8, 2013
Location
north of Bean town
drilling 718 32-40 hrc. I need to make a .375 hole, 4.800 long thru. 7pcs

no coolant thru

I was thinking doing it from both sides then reaming thru to reduce walk out(.002tir)

Can anyone suggest a drill/reamer for me


Thanks
 
Spot the hole (you didn't specify what the surface condition was). Drill .005-.010 undersize then you have to run an end mill bore straight through. At that depth it might be a special from someone. Welcome to the world of 718. We do this all the time. Drill to get the hole in, end mill bore for T/P / straightness, If need be ream for size after the end mill bore. Do not ream directly after drilling. If the hole is not straight the reamer will just follow it.
 
Spot the hole (you didn't specify what the surface condition was). Drill .005-.010 undersize then you have to run an end mill bore straight through. At that depth it might be a special from someone. Welcome to the world of 718. We do this all the time. Drill to get the hole in, end mill bore for T/P / straightness, If need be ream for size after the end mill bore. Do not ream directly after drilling. If the hole is not straight the reamer will just follow it.

Bore a 3/8 hole nearly 5'' deep? ............not to mention finding an end mill that long being a challenge.
 
Bore a 3/8 hole nearly 5'' deep? ............not to mention finding an end mill that long being a challenge.

Hope you can get coolant down in the hole, I just ran 3 pcs a few weeks ago .297 dia hole with an OSG powder metal drill 1.500 deep. I resharpened the drill several, several times. Bit of a learning curve if you haven't ran it before. Some of the times when the drill really would cut good I could move a lot of material with. Key is don't work harden it. I did this on my prototrak mill so I could feel the drill as it started to dull. No coolant. I bought 3 new drills sent 1 back after multiple sharpenings. Listen to your drill for an squealing, you need to pull it out or your just work hardening your work piece. I hope you have plenty to spend on tooling. OSG rep compared it to drilling thru a high speed tool blank.
 
drilling 718 32-40 hrc. I need to make a .375 hole, 4.800 long thru. 7pcs

no coolant thru

I was thinking doing it from both sides then reaming thru to reduce walk out(.002tir)

Can anyone suggest a drill/reamer for me


Thanks

THIS IS LATHE WORK

Assuming your lathe is properly aligned,......
Use solid carbide drill, coolant through, no discussion, no substitute.
Use (Blake} coaxial indicator to indicate drill within .001 OR LESS, Indicate .375 pin in two places then install drill), eliminate any coolant leaks so as to direct all available pressure to cutting tip.
Drill pilot hole about .125 deep using spot drill with same angle as drill, if pilot drill has different angle make it greater, not smaller, you want drill to start cutting with entire cutting edge or center, not outer edges of flutes.
If drill has 140 degree cutting edge use 140 degree pilot drill.

Pilot drill must cut same size hole as drill following it.

After pilot hole is done, critical issue is to set drill into position as follows:
Run spindle at low RPM, feed drill into hole at high feed rate, this prevents vibrations and potential for chipping edges of drill on entry and before it is confined by pilot hole.


N2(PILOT DRILL)
T606
G97 S815 M3
G0 G54 X0 Z.1 M8
G1 G99 Z-.125 F.002
G4 P1.
GO Z.125 M9
G53 X0 Z0
M1

N3(DRILL)
T808
G97 S500 M3
G0 G54 X0 Z.1 M8
G1 G99 Z-.1 F.012
S815
Z-5. F.002
G4 P1.
S500
G98 Z.125 F50. M9
G53 X0 Z0
M1

This assumes you are drilling bar stock, if you are drilling slugs and drill will be breaking thru, you must slow down RPM and feed rate before breaking thru to avoid chipping drill.
If breaking thru, stop while still in solid, dwell (YOU MUST DWELL TO UNHOOK CUTTING EDGE FROM CUT BEFORE PULLING BACK), pull back about .03, slow down RPM and feed rate to 75% and continue drilling thru.

This is based on personal experience of drilling .281 diameter hole, 4.5" deep in 10 pcs using one Titex drill.
Each drill was resharpened in house 2 more times and each time used to drill another 10 pcs .
Without original coating, subsequent use produced more wear on tip and surface finish was not as smooth but was acceptable.

Higher then 80 FPM surface speed will fry the cutting edge, higher feed rate will chip cutting edge starting at center point where surface speed is significantly lower then at the outer edges of flutes.

You can try all other cheaper approaches, when you're done wasting time and money, you'll come back to what works,..... you're welcome.
 
Oh, I have to correct my own G code, at the end of drilling add G0 in front of G53.
It is good idea to pull drill out of the hole at pace approximately equal to 25% rapid move.

The reason is, as drill gets deeper into the hole, chips will not be flushed out at the same rate as when drill is half way in, as a result flutes are packed with chips, chips are being compacted by rotation of part, friction arranges particles in one pattern.

Sudden and fast change of direction will put potentially damaging stress on drill, particles of chips will be forced to realign inside flutes while being compacted by fast pace motion in opposite direction and friction from spinning part, you want to take the change of direction in an easy pace that allows particles of chips to realign and loosen up so that drill doesn't jam and break.

I am currently running .277 diameter carbide drill 5.5 inches deep into 303 SS, making 230 holes with each drill, in one continuous move.

Inconel 718 will crumble as you cut it, no need to worry about strings of chips, 303 is acting in similar fashion and I only get strings on first part after installing new drill.

Price of drill is not an issue here because alternative is far more costly and ineffective, you may want to look into Mitsubishi tool catalog as well, there is a guide at beginning of chapter listing solid carbide, coolant thru drills that describes techniques I outlined and used almost 8 years ago without ever being aware of Mitsubishi catalog and drills I am using in the past few weeks to drill 303 SS parts.
 
Guys, any of you know of a good place that repairs bullshit meters?
Mine went off at around 7'clock tonight and hasn't stopped since... :toetap:

Spot the hole (you didn't specify what the surface condition was). Drill .005-.010 undersize then you have to run an end mill bore straight through. At that depth it might be a special from someone. Welcome to the world of 718. We do this all the time. Drill to get the hole in, end mill bore for T/P / straightness, If need be ream for size after the end mill bore. Do not ream directly after drilling. If the hole is not straight the reamer will just follow it.

To the OP, man, you'll have one bitch of a time drilling that thing without through coolant, and I don't care if you're trying it from both sides.
Even then you have 2.5" of material to go through, and only when you get to the second side will you know that any misalignment just killed the whole shebang.

Guhring does have Firex coated 20X drills that can do it from one side, but they are coolant through for a very good reason.
I know you don't want / can't have it wired out, but seriously, you really should find someone with TSC.
Drill U/S with a stubby 9.1mm for approx 1".
Push a 3/8 endmill in there for maybe .800 or so, then take a 20X 9.5mm drill,
slowly feed down to .5 deep and then start drilling all the way through, keeping the tool guided by the top of the hole.
You will get a bit of a walk, but that's the best choice I can imagine.

Nonetheless, all of that above is WITH a coolant through drill in both instances.
 
"My Google" found this, world of knowledge in there, it all works as claimed, no guess work.

https://www.mitsubishicarbide.com/mmus/catalog/pdf/b/b095a.pdf


I also noticed that some suggested doing the job on VMC, using end mills to prep pilot hole, reaming .... etc.
Now the reason why this is lathe work and there can be no argument against it.
Spinning drill can drill a hole at any location on work piece, strait or at the angle relative to other features on work piece.
It means that round work piece clamped in a wise or indexing head would have to be perfectly lined up with spindle to produce hole concentric to OD of the work piece, this concept is equal to pissing into the wind, with equal result.

You want to spin the work piece instead of spinning the drill and here is why.
Toll such as drill, having angle on each of two flutes will be forced into center of spinning work piece because each flute deflection results in canceling of the other, therefore staying on center of spinning work piece.
Simply put, this results in hole being concentric to OD throughout the cut.

You want drill to be on center line so that as it gets deep into the hole, it doesn't rub with back end.
Long carbide drill will tolerate some bending if it's not 100% on center, but you want it as perfectly centered as possible so that cutting tip is not fighting to stay on center of spinning work piece which, as noted above, will force drill to center of work piece even if it is off center.

For sake of argument, consider this, if you hand grind a drill and one flute edge is slightly longer then the other but having same angle, meaning that drill point is not on center of drill, tip of drill will still be forced into the center of work piece providing drill is long enough to bend and confirm.
The resulting hole will still be concentric to OD but it will be oversize due to the fact that location of center point is shifted and longer flute acts as a boring tool while short flute edge cuts smaller diameter then it would when tho flutes are same length.

In days of conventional, cam driven, screw machines such as Acme Gridley, I could hand grind hand full of drills daily and rarely have one cut oversize. Back then drilling 1.5" deep hole required 2 or 3 drills depending on cam installed and each drill had to cut same size to not show steps or spiral marks.
Now days, I can only come close, lost the touch after so many years of not doing it.

My first encounter with super alloys and drilling deep holes has been result of other experts trying everything else first, the hard way then submitting to last result, which is "right tool for the job", concept that saves time, money, ensures success and breaks egos of leads and managers, I got the job done, got the credit, got the raise and ............. made no friends along the way, idiots hated my guts and got me fired from jobs in few cases.

In any case, I hope some useful information was offered here, I hate to see people do stupid things and suffer as a result of self inflicted wound.
 
so your cutting 718 but you're going to gripe about the cost of a drill? You've already lost.

This is a job for a hole popper, plain and simple. You're going to end up sending it out to EDM to have broken tools dug out of it, so you might as well have them do it from the start.

And the thing that always amazes me, why did you quote a job you have no idea how to do?
 
In looking back, I can't say that I am sure what configuration part we are talking about, is it round part or something that has to be done on VMC ? ,................ so let me start over,............

I wanna drill 1/8" hole thru block of marble 10." thick.
I was thinking flat head screwdriver and watchmaker's brass hammer, turning screwdriver 5 degrees with each hit,........ any suggestions ???, sweat dripping from my nose down screwdriver shaft can serve to contain dust and sparks :eek:,........... never mind:crazy:
 
ok smart ass(s) first off i didnt quote anything, secondly i wasnt griping about the cost just trying to find the cheapest solution that will work.

the part is 1.5 OD 4.8 long with a .375 hole thru

the part has been made this way before or so im told(except they other manufacturer has TSC)
I already suggested doing it the lathe but was shot down telling me the drill would walk.

Larry..who said i didnt know how to do this? i was simply looking for a recommended drill, not for someone to write a lathe program for me or to suggest EDM considering i clearly stated it was to be done in a VMC.

Thanks to all that took my inquiry seriously
 
the part is 1.5 OD 4.8 long with a .375 hole thru

the part has been made this way before or so im told(except they other manufacturer has TSC)
I already suggested doing it the lathe but was shot down telling me the drill would walk.

Ok, I think your real beef is not with the smartasses on this forum, rather the one who shot you down from doing it on a lathe.
Lathe = TSC with very little fuss.

For inco 718, Guhring 5511 series drill, ER32 collet with coolant nut+blocker.
Drill from both sides a tad under, ream through with a Garr 3fl carbide drill.
Take finished part, shove it up the asshole that told you to mill it.

On Edit: You can substitute Guhring with Titex, but I don't know which series to recommend.
YG-s are OK for most materials, unfortunately Inco is not one of them.
 








 
Back
Top