Carbide drill breaking

S.Fee · Sep 8, 2015

Ok, so I have a proven program, has 3 holes spotted and drilled with .25" spot, .25" drill. Im on my 3rd part for the day and I ran two holes, but the drill was stringing; which usually means corners are chipped. I show my supervisor and he says ok, let's put a new one. I put it in and teach it. Go to run it, and it gets about .150-.250 down and blows up. My supervisor put a new drill in and went teach it, the offset changes .002 from what I had, so obviously I taught the tool right. We checked the spot for any push in or chips, everything is good. So we conclude it had to be bad carbide. Is this correct? Does this happen often with carbide drills?

DMF_TomB · Sep 8, 2015

S.Fee said:
Ok, so I have a proven program, has 3 holes spotted and drilled with .25" spot, .25" drill. Im on my 3rd part for the day and I ran two holes, but the drill was stringing; which usually means corners are chipped. I show my supervisor and he says ok, let's put a new one. I put it in and teach it. Go to run it, and it gets about .150-.250 down and blows up. My supervisor put a new drill in and went teach it, the offset changes .002 from what I had, so obviously I taught the tool right. We checked the spot for any push in or chips, everything is good. So we conclude it had to be bad carbide. Is this correct? Does this happen often with carbide drills?

.
carbide drills are often run at rpm and feed at the recommended maximum. if drill is not short and hole depth gets deeper and steel may have have hard spots or slag inclusions, plus drill bit may have runout or wobble, plus coolant may have trouble reaching drill tip all may require a reduction in feeds and speeds
.
try 70% rpm and 50% feed rate and see if drill stops breaking. also check drill bit runout as small drills with high runout break easy too. carbide drills that are noisy or loud often is a sign of dull and or high runout. sometimes metal sticks to cutting edge causing problems. coolant concentration often needs a higher concentration

david n · Sep 8, 2015

Well, first of all don't spot. Second are you using a good name brand carbide drill? Is the drill the correct style for your material? Are you using mfg'rs recommended feeds and speeds? Do you have good coolant flow? Good coolant mix? What kind of toolholder? Too little info on your part to give you a decent answer. I run lots of carbide drills in various materials. I run OSG, Nachi and Guhring drills. I get thousands of holes out of each brand.

DMF_TomB · Sep 8, 2015

carbide drills i use we get 45 minutes tool life. if i reduce rpm and feed i often will get over 60 minutes tool life.
.
i usually time how long to drill a hole. if a reduced rpm and feed takes a few seconds longer or a few minutes more per part with 50 holes BUT i do not have to dig out a broken drill bit out of a hole and replace a expensive drill bit, often it ends up being faster in the long run and cheaper to drill at slower rpm and feed

doug925 · Sep 8, 2015

david n said:
Well, first of all don't spot.

Carbide drills do not want a spot...typically.
If the point angles are the same, then it might be okay.
If however, they are not, I'd expect the drill corners to suffer quickly.

Just my $.02

Doug.

nomak_1835 · Sep 8, 2015

actually with carbide drilling and use of a spot drill you want your spot drill to be say a 140 degree angle and your actual drill angle to be 135. this will cause the tip to hit first and not the drill flutes fully engaged thus casing drill chipping and premature wear. Having this scenario creates the same environment as if drilling into a flat piece of material that has not been spotted where the point hits first and the drill flutes gradually increase their engagement into the material thus less stress on the cutting edges.

doug925 said:
Carbide drills do not want a spot...typically.
If the point angles are the same, then it might be okay.
If however, they are not, I'd expect the drill corners to suffer quickly.

Just my $.02

Doug.

PixMan · Sep 8, 2015

Most high performance solid carbide drills are a 140º point angle, and anything 8xD and under shouldn't require a spot unless it's on a lathe drilling on-center and there's a lump there at the center.

If you absolutely MUST spot, several suppliers offer a 142º spot drill. Worst case, use a common 120º but only make a spot that's less than 1/2 the diameter of the drill you intend to use.

litlerob1 · Sep 8, 2015

nomak_1835 said:
actually with carbide drilling and use of a spot drill you want your spot drill to be say a 140 degree angle and your actual drill angle to be 135. this will cause the tip to hit first and not the drill flutes fully engaged thus casing drill chipping and premature wear. Having this scenario creates the same environment as if drilling into a flat piece of material that has not been spotted where the point hits first and the drill flutes gradually increase their engagement into the material thus less stress on the cutting edges.

So don't spot and the drill tip will hit first, right? So KISS don't spot.

PixMan said:
Most high performance solid carbide drills are a 140º point angle, and anything 8xD and under shouldn't require a spot unless it's on a lathe drilling on-center and there's a lump there at the center.

If you absolutely MUST spot, several suppliers offer a 142º spot drill. Worst case, use a common 120º but only make a spot that's less than 1/2 the diameter of the drill you intend to use.

If in some case I need a spot or center dill, I usually only spot a tiny bit more than the diameter the web will create. Called a web right Pix?

But I am guessing the OP is having runout issues or workholding issues, because of the comment, "My supervisor put a new drill in and went teach it, the offset changes .002 from what I had, so obviously I taught the tool right." Begs the question what is he holding it in probably not a collet, .25" drill???

Robert my ±2

Mtndew · Sep 9, 2015

S.Fee said:
Ok, so I have a proven program, has 3 holes spotted and drilled with .25" spot, .25" drill. Im on my 3rd part for the day and I ran two holes, but the drill was stringing; which usually means corners are chipped. I show my supervisor and he says ok, let's put a new one. I put it in and teach it. Go to run it, and it gets about .150-.250 down and blows up. My supervisor put a new drill in and went teach it, the offset changes .002 from what I had, so obviously I taught the tool right. We checked the spot for any push in or chips, everything is good. So we conclude it had to be bad carbide. Is this correct? Does this happen often with carbide drills?

What material?
What carbide drill? Coated?
What speeds and feeds are you running it at?
What is the runout of the drill?

PixMan · Sep 9, 2015

Yep...a dearth of information.

I can picture a simple $10 Morse carbide twist drill in a Jacobs chuck, the kind of drill we buy to try drilling out a broken but hard bolt with the cordless drill, expecting to break it just as it gets through the bolt.

Blame the tool!

DMF_TomB · Sep 9, 2015

PixMan said:
Most high performance solid carbide drills are a 140º point angle, and anything 8xD and under shouldn't require a spot unless it's on a lathe drilling on-center and there's a lump there at the center.

If you absolutely MUST spot, several suppliers offer a 142º spot drill. Worst case, use a common 120º but only make a spot that's less than 1/2 the diameter of the drill you intend to use.

.
obviously depends on length of drill and part surface. i often machine castings and if i did not spot face or spot drill a rough surface i have often seen a carbide drill bit snap quickly.
.
my point is i have seen carbide drills at so high a rpm and feed that they are too sensitive to many things and break too easily. i have often timed drilled holes at a reduced rpm and feed taking a second or 2 longer but tool life is often easily increases often 200 or 300% and drill stops breaking. drill just gets dull in normal tool usage time amounts

Mtndew · Sep 9, 2015

DMF_TomB said:
i often machine castings and if i did not spot face or spot drill a rough surface i have often seen a carbide drill bit snap quickly.

Well that's just common sense.

adama · Sep 9, 2015

Alternative on ruff uneven surfaces is just follow the std drill specifications and used a shorter drill and at a reduced feed - speed intill the hole is established before ramping upto full feed + speed.

trampus · Oct 8, 2015

Material specs .

Mtndew said:
What material?
What carbide drill? Coated?
What speeds and feeds are you running it at?
What is the runout of the drill?

I was wondering when this would pop up. That should have been in the original question , according to me anyways . . .I love it when I am asked for a cycle time on a BP and nobody ever really has any concern in the office. To me that should be the second question , behind if it is or not a metric BP .

billzweig · Oct 8, 2015

Regardless of material, speed, etc. carbide drills, especially in smaller sizes, are very sensitive to run-out. Inaccurate drill chuck can be a problem. For really small sizes even small spindle runout an be a problem. On some jobs I need to drill holes as small as #85. After braking a number of drills, I do it now on a Leitz jig borer with the drill held in a collet. Total runout is under 2 microns (0.00008") - no more broken drills.

litlerob1 · Oct 8, 2015

trampus said:
I was wondering when this would pop up.

Really? As it was a month ago.

Robert

DMF_TomB · Oct 9, 2015

billzweig said:
Regardless of material, speed, etc. carbide drills, especially in smaller sizes, are very sensitive to run-out. Inaccurate drill chuck can be a problem. For really small sizes even small spindle runout an be a problem. On some jobs I need to drill holes as small as #85. After braking a number of drills, I do it now on a Leitz jig borer with the drill held in a collet. Total runout is under 2 microns (0.00008") - no more broken drills.

.
a offline tool setter with a 20X magnified display can help to see if a new drill in a tool holder has runout. i wipe tool holder taper clean before checking runout. often tool holder tapers pick up rust, oil, grease on taper effecting tool runout. it can be very hard to maintain low runout on all tool holders. ultimately you would need to put tool on machine spindle and measure runout there but that can often be difficult.
.
some machine spindle tapers them selves develop runout problems over time and we check ours with a 12" long test bar for runout and parallel alignment or tram monthly. often first thing we have to do is clean machine spindle taper as that gets dirt buildup too

Search

Largest Manufacturing Technology Community on the Web

Search

Carbide drill breaking

S.Fee

Plastic

DMF_TomB

Diamond

david n

Diamond

DMF_TomB

Diamond

doug925

Titanium

nomak_1835

Plastic

PixMan

Diamond

litlerob1

Diamond

Mtndew

Diamond

PixMan

Diamond

DMF_TomB

Diamond

Mtndew

Diamond

adama

Diamond

trampus

Plastic

billzweig

Stainless

litlerob1

Diamond

DMF_TomB

Diamond

Similar threads