New to solid carbide drills

FrankieB · May 26, 2021

Machine: haas sl30 lathe
Material: 4140
Drill size 6.7mm with through tool coolant

I know not to peck with a carbide drill, but any other best practice i need to know? Any speed and feed recommendations? The manufacture is recommending 6500 RPM and a feed of 0.007 IPR, this machine won’t spin that fast.
Thank You

mhajicek · May 26, 2021

I'd keep the chipload the same and run as fast as you can. If the drill is long, do a pilot with a stub drill first, put the long drill in at a low RPM, then speed up and drill.

Nerdlinger · May 26, 2021

If you spot the hole first make certain it is with a tool that has a GREATER tip angle than your carbide. So if, for instance, your carbide drill has 140 degree tip make sure to use something equal to or greater than that....142 is a common spot drill tip angle for this reason. Good luck!

fmari --MariTool- · May 26, 2021

Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

.007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.

Milland · May 26, 2021

If a blind hole you might program in brief dwell (.1 second or so) before retract. Doing the same before a peck is good too, but you might have to hand program.

If through you might slow feed a bit during breakout.

CAMasochism · May 26, 2021

fmari --MariTool- said:
Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

.007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.

The Mitsubishi MVS drills I use recommends between .0043-.0094 for 4340 with .0071 being right in the middle for that size range. I routinely drill with these drills in the 25-40xd range in various diameters from 5mm-10mm in a single shot, but the machine we use them with has 1000PSI coolant. The 10mm we feed at .012 per rev and it makes beautiful holes. They also say not to peck. The problem for him comes down to being limited by spindle speed. Spin it as fast as you safely can and from there you'll have to play with your IPR until you get the best results.

Op does need to clarify how deep because that does affect things.
What brand drill are you using?
What coating?

FrankieB · May 26, 2021

The depth is 1.125 and brand is widin with TiAIN coating.

FrankieB · May 26, 2021

Hand coding isn’t a problem, i had code everything i do on this machine.

Mtndew · May 27, 2021

FrankieB said:
Machine: haas sl30 lathe
Material: 4140
Drill size 6.7mm with through tool coolant

I know not to peck with a carbide drill, but any other best practice i need to know? Any speed and feed recommendations? The manufacture is recommending 6500 RPM and a feed of 0.007 IPR, this machine won’t spin that fast.
Thank You

In 4140 I typically go around 300sfpm for solid carbide drills. That comes out to around 4400rpm, and I agree with Frank, the .007 is a tad high... maybe kick it down to around .005ipr and send it.

FrankieB · May 27, 2021

I want to thank everyone for the recommendation, i went with 3000 rpm at 0.005 ipr.

escapethewrmhole · May 29, 2021

fmari --MariTool- said:
Who told you not to peck?! Nothing wrong with pecking. Even with coolant thru if your pressure isn't the greatest, or sometimes you let the filters get a little dirtier than it should adding a few pecks in your program will make it more reliable. If I am drilling 3.5" deep and my flute length is 3.8 or 3.9" long I will add a few packs starting at 2.75".

.007ipr in 4140 for a 6mm drill sounds very high. Drilling on a lathe where the drill is stationary is always worse than when the drill is spinning !!! I would start out with .0045 ipr.

Almost every manufacturer that I've seens technical guide tells you specifically not to peck. Heck even allied tells you not to on their spade drills.

CarbideBob · May 29, 2021

escapethewrmhole said:
Almost every manufacturer that I've seens technical guide tells you specifically not to peck. Heck even allied tells you not to on their spade drills.

The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
Bob

706jim · May 31, 2021

CarbideBob said:
The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
Bob

Somebody tried something and it worked. It then becomes gospel.

Look at the sfm values for diamond tools in Machinery's Handbook. They're all over the place! I figure that it's due to rpm limitations on whatever machine they were using at the time the data was compiled.

So there you go.

fmari --MariTool- · Jun 1, 2021

CarbideBob said:
The process of the how and by whom these "technical guides" are often written is interesting and sometimes scary.
Bob

Very hard to get and keep good technical cutting tool engineers. The good ones are making 6 figures in machines shops and not making technical guides.

DMF_TomB · Sep 4, 2022

FrankieB said:
Machine: haas sl30 lathe
Material: 4140
Drill size 6.7mm with through tool coolant

I know not to peck with a carbide drill, but any other best practice i need to know? Any speed and feed recommendations? The manufacture is recommending 6500 RPM and a feed of 0.007 IPR, this machine won’t spin that fast.
Thank You

pecking problems usually at high rapids drill tip don't like bouncing off beginning of hole
(longer drills whip or wobble more at higher rpm) so sometimes on peck drill doesn't
come completely out of hole
and
peck parameter that is how far from last peck rapids stop and feed begins. if deep
hole and chips still in hole and drill rapids in hole it pushes or packs chips to bottom
of hole and drill tip "hits" the packed chips at rapid their usually a crunch sound. if
peck parameter increased say from .050" to .150" away, bigger and deeper holes
there is little if any crunch sound on peck, but this increases time cause you add
feed rate time on each peck.
.
i am not saying always peck but deep holes i have often drilled 8" deep pulled
out than come back in to drill last few inches caused that stopped sudden tool
failures that were happening with no peck on deep holes

sinha · Sep 4, 2022

When the depth to diameter ratio is too high, pecking might be a compulsion. In fact, pecking with full retract might be needed. Through-coolant drills will, of course, have less problems, obviating the need for pecking in most cases.

Search

Largest Manufacturing Technology Community on the Web

Search

New to solid carbide drills

FrankieB

Aluminum

mhajicek

Diamond

Nerdlinger

Stainless

fmari --MariTool-

Titanium

Milland

Diamond

CAMasochism

Stainless

FrankieB

Aluminum

FrankieB

Aluminum

Mtndew

Diamond

FrankieB

Aluminum

escapethewrmhole

Aluminum

CarbideBob

Diamond

706jim

Titanium

fmari --MariTool-

Titanium

DMF_TomB

Diamond

sinha

Titanium

Similar threads