Solid carbide drills breaking- looking for recommendation

[wmpy]

I am looking for recommendations for a new drill to try in my application.

axial (end working) live tool holder in a lathe
max 3000 rpm
no through coolant available
3 mm holes x 0.593" deep
4140 annealed material
no spotting- drilling into flat face of part
flooding the drill with water-soluble coolant with a pretty good blast
currently using YG-1 3XD Dream Drills (DH423030K). These are solid carbide, non-coolant through drills. Despite being 3XD drills, there is plenty of flute length to get the depth I need. The 5XD just seemed to be too long, and I was worried about them breaking.

I am getting inconsistent tool life. Some drills last 2000-2500 pcs. With 4 holes per part, that's 8-10k holes. I'm happy with that. Other drills break after 50-200 pcs. There doesn't seem to be any inbetween.

I checked the last drill for runout and measured it at .0003" at the tip. I thought that was ok.

The drills always break in the part, so I know it's not some random chips snapping the tool when it's out of the cut.

My program looks something like this:

S3000 (93sfm)
G00 Z0.05
G01 G98 Z-0.05 F5. (0.001667 ipr)
Z-0.119 F9. (0.003 ipr)
G4 U0.1 (short dwell)
W0.01 (short retract)
Z-0.238
G4 U0.1
W0.01
Z-0.357
G4 U0.1
W0.01
Z-0.475
G4 U0.1
Z-0.1 F50. (retract to just below beginning of hole)
Z-0.45
Z-0.593 F9. (finish depth)
G4 U0.1
Z0. F50.
G00 Z0.1

Does anyone see any problems with my current setup? I'm thinking that the drills I'm using might suffer from some inconsistencies. What are your favorite drills for an application like this?

 

[Milland]

Brand of drill? Coated, bare?

Is the live holder newish, or been rebuilt recently? Even with good TIR, the bearings may be loose under load, and spindle deviation may cause issues.

I think I'd try shortening depth of peck, while increasing feed a bit, and ensuring I've cleared chips before feeding at speed (not rapid) to about +.1 Z from each previous depth, then feed at cutting rate until next depth.

 

[Mtndew]

Does anyone see any problems with my current setup?

Other than severely limiting yourself with the max rpm of 3000 (should be triple that), the only thing that I can think of is that you're not spotting it. Even a tiny center drill spot .03 deep will help. But in a live tool lathe, you might not have the space to use one.

 

[Mtndew]

What I would do is try a stubby split point coated hss drill. You'd be able to feed it faster and not worry about it breaking.

 

[Orange Vise]

Some drills last 2000-2500 pcs. With 4 holes per part, that's 8-10k holes. I'm happy with that. Other drills break after 50-200 pcs. There doesn't seem to be any inbetween.

Could be the edge prep on the drills.

One experiment you could try is to "break in" the drills in a VMC by turning a piece of scrap material into swiss cheese.

A VMC will generally provide more controlled conditions than a live tooled lathe. Drill 1000 holes to slightly dull the edges and stress-test the tool before moving it to the lathe and see if that gets rid of the anomalies. Sure beats running a lathe unattended overnight, only to scrap the entire lot because a drill broke at 7pm.

 

[wmpy]

Brand of drill? Coated, bare?

Is the live holder newish, or been rebuilt recently? Even with good TIR, the bearings may be loose under load, and spindle deviation may cause issues.

I think I'd try shortening depth of peck, while increasing feed a bit, and ensuring I've cleared chips before feeding at speed (not rapid) to about +.1 Z from each previous depth, then feed at cutting rate until next depth.

The drills are from YG-1, and they are coated.

The holder isn't new and hasn't been rebuilt recently, but it seems to be in good condition. I was checking it out yesterday and it had a couple tenths of play.

I'm pecking every 3 mm at the moment and pulling back 0.01" every time except for right before the last depth where I pull out almost all the way. I never rapid with the drill in the part. Fastest I have it going is 50 ipm.

 

[wmpy]

Other than severely limiting yourself with the max rpm of 3000 (should be triple that), the only thing that I can think of is that you're not spotting it. Even a tiny center drill spot .03 deep will help. But in a live tool lathe, you might not have the space to use one.

I have the turret positions, but I'm not sure if I have another holder. It might be worth trying if I can find one.

 

[wmpy]

What I would do is try a stubby split point coated hss drill. You'd be able to feed it faster and not worry about it breaking.

I had started out running this job with HSS drills from OSG, and while they didn't break, tool life wasn't great. I might have to revisit this method.

 

[Milland]

I'm pecking every 3 mm at the moment and pulling back 0.01" every time except for right before the last depth where I pull out almost all the way. I never rapid with the drill in the part. Fastest I have it going is 50 ipm.

Especially if you're usually deep in the part when the drill breaks, I'd pull almost all the way out with each peck, leaving ~.1 or so in the hole for stability. If the break depth is random, do it from 6mm on, otherwise from the beginning of break depth on.

 

[wmpy]

Could be the edge prep on the drills.

One experiment you could try is to "break in" the drills in a VMC by turning a piece of scrap material into swiss cheese.

A VMC will generally provide more controlled conditions than a live tooled lathe. Drill 1000 holes to slightly dull the edges and stress-test the tool before moving it to the lathe and see if that gets rid of the anomalies. Sure beats running a lathe unattended overnight, only to scrap the entire lot because a drill broke at 7pm.

Interesting. At this point I think I'd rather just try someone else's drill to see if they have the edge prep right.

Luckily (?) only one part gets scrapped when the drill breaks because the next tool comes in and gets trashed which stalls the spindle and stops the machine.

Maybe I should see if anyone makes a spindle speeding, through coolant version of an end-working holder for this machine.

 

[Mtndew]

Interesting. At this point I think I'd rather just try someone else's drill to see if they have the edge prep right.

My favorite carbide drills in order:
Sandvik 460 series for general steels---860 series for steel specific (VERY good drills)
Guhring (love their deep hole drills)
OSG (They have a nice range of drills that fall into lengths that Sandvik and Guhring sometimes don't carry)
Kennametal (their Go-Drill has a nice edge on them)

 

[wmpy]

Especially if you're usually deep in the part when the drill breaks, I'd pull almost all the way out with each peck, leaving ~.1 or so in the hole for stability. If the break depth is random, do it from 6mm on, otherwise from the beginning of break depth on.

I made the changes you suggested starting after the 6 mm depth. We'll see how it goes. It added 4 seconds to the part cycle time (1 s per hole), but I can live with that for now if it helps the situation.

 

[gustafson]

carbide are really going to hate any off center force. I would spot drill

 

[Milland]

I made the changes you suggested starting after the 6 mm depth. We'll see how it goes. It added 4 seconds to the part cycle time (1 s per hole), but I can live with that for now if it helps the situation.

Remember, if it makes things worse it's Mntdew's fault!

 

[Orange Vise]

Interesting. At this point I think I'd rather just try someone else's drill to see if they have the edge prep right.

Luckily (?) only one part gets scrapped when the drill breaks because the next tool comes in and gets trashed which stalls the spindle and stops the machine.

Maybe I should see if anyone makes a spindle speeding, through coolant version of an end-working holder for this machine.

Yea switching to a different drill will likely show that the original tool/brand was the culprit.

The VMC test would be mostly to satisfy your curiosity, but not the most efficient use of time.

 

[cnctoolcat]

That's pretty deep for a 3mm hole. I would say your inconsistent tool life is due to chips binding the drill in the hole.

I would throw a Titex or Guhring coated-cobalt drill at it for ultimate reliability. You will have to spot drill though!

ToolCat

 

[Kingbob]

I've had really good luck with these but I only do stainless and in a vmc and with coolant through so I don't l know if this recommendation helps.
I've gotten 20,000 before choosing to retire one of these guys. I know this is a coolant through but I'd bet the same drill comes solid.

 

[wmpy]

I've had really good luck with these but I only do stainless and in a vmc and with coolant through so I don't l know if this recommendation helps.
I've gotten 20,000 before choosing to retire one of these guys. I know this is a coolant through but I'd bet the same drill comes solid.
View attachment 392431

I have heard good things about the GODrills. I may give that a try.

 

[wmpy]

My tooling rep is pointing out that I'm using a 3xD drill to go 5xD and that I should be using a different drill. I had tried the YG-1 5xD drills when I was dialing in this job, but they had a tendency to walk, which was unacceptable. The 3xD drills appear to have enough flute length (0.770") for the depth I'm going, especially with all the pecks I've got. I was troubleshooting this with a YG-1 tech at the time, and he was o.k. with what I was doing. I don't know- maybe I've been pushing my luck. Looking at it, though, there seems to be plenty of room for the chips to evacuate.

If I have to move up to a YG-1 5xD drill, I'll have to add a spot operation to try to keep the drill from walking. I don't have any more live holders, so I'd need to source one of those. Hopefully a different brand of drill or the program changes I've made will solve the problem.

 

[Speedie]

Cobalt stubby is the only way to go with no spot, no coolant through. And no not 9000rpm...lol.