Drill Breaking In 17-4 H1025

[McLaren]

 Anyone have thoughts on what I'm doing wrong? Drills are 27/64" Cobalt, 1" hole depth. One flute completely pops off. Next try was going to be back up to 33SFM and try no peck. I'm thinking maybe it's trying to recut chips on the peck? Machine is like 20HP and pushing ~10% spindle load so I didn't think I was over-torquing the drill.

LH Drill - 33 SFM, .0033" FPR, .250" Peck

RH Drill - 22 SFM, .0035" FPR, .150" Peck

 

[workmantm]

Use Carbide. I used to run a ton of 15-5 @ H1025. No manufacturer has S&F info for cobalt or HSS drills for these materials. I ran the Accupro solid drills hard and they held up great. Also had phenomenal success with Titex drills using thru tool coolant. 

[Machineguy]

1800PM, 4 IPM, PECK .100. flood like crazy.

This is just a start point.

H1025 is the best condition for this steel for machining.

Your peck was way to much. You can work harden this if you push too hard.

Carbide is the way to go as workmantm says

 

[Matthew Hajicek - Singularity]

Carbide drills all the way.  On the occasion I have to whip out a prototype or two with a cobalt drill I run 60 SFM.  That's in 17-4 H900.

[gms1]

This is what i am using in 15-5ph h1025 for one of my drills.

13.6mm sumitomo solid carbide drill  #MDW1306GS2 no thru coolant (they all say I should be using thru but I don't have that luxury on that particular machine)

Custom non-canned cycle that 1st pecks only .03 deep @ 3ipm. Subsequent pecks are .280" @ 3.5 ipm. 1" total drill depth.

This will last roughly 200-300 holes holding .005" true position over the course of 4-6 months in a non-temp controlled shop.

My tool reps told me I should be using thru coolant carbide and no peck whatsoever. I just haven't had a chance to get it on my coolant thru machines.

[mkd]

is it breaking when canned cycle returns to bottom of hole? I've had machine parameters set to close where the tip rapid collides with chip and breaks.

[Colin Gilchrist]

What kind of setup are you using to hold onto the tool? I wonder if the shank might be slipping, so the tool isn't getting a good "bite" into the material. What about run out? How concentric were the flutes? Did you happen to throw an indicator on the tool before running it? I always try to remember to sweep the shank, close to where I'm gripping the tool, and again on the flutes near the tip.

How many holes/parts do you have to cut? Are you confident on the H1025 heat treat? Any possibility that you've got hard spots, or the condition just isn't correct? The reason I ask is that you're getting the whole flute shearing away. You aren't just getting excessive wear of the tip, and this is a Cobalt drill, so it should be tough.

33 SFM seems pretty low. I'd go more like 65 SFM. Also, I usually shoot for 1% of the diameter, per tooth, for chip load. That would be closer to .008 per revolution. Using only .0035, you could be not generating enough of a chip, and causing the material to work harden.

Are you confident in the actual tool geometry does the tool have the correct cutting and clearance angles? I've had plenty of batches of bad drills...

My final tool trick to try is to hand-grind a .02-.04 corner radius on the edge of each flute, where the body diameter meets the tip angle. That sharp corner there can concentrate the heat in that area.

Speaking of heat, that is really hurting you. In harder materials like this, do not use more than 1/6th of the diameter for your peck value. That would be .07 per peck. Use .05 instead. The biggest reason is not chip packing / chip evacuation. It is the heat being generated. Yes, you need to clear chips, but you also need copious amounts of coolant, and you need to retract far enough above the hole to simultaneously cool the drill, and get some coolant down in the hole to cool the part. What is your Coolant concentration percentage? If you are running below 8%, then really consider bumping it up...

[McLaren]

 Thanks for the replies everyone! I found an OSG EX-SUS drill and was able to do it no problems at 33SFM, 1IPM and no peck. Seems like the jobber drill was just too long and trying to untwist under the load.

[Leon82]

Small spot first or spot > than the drill angle. Then drill and come back to chamfer