Drilling a hole in 304 shouldn't be this hard!

[PoiToi]

Hi all, I'm ghaving a hell of a time trying to drill a hole in 304SS.

It's a .180 (#15) hole, 1.1"deep...
I've tried cobalt drills, pecking every .200" at 75 SFM (1600 rpm), and they lasted about 10 parts.
I just got 2 carbide drills that didn't last one part, at the recommended 200SFM and .003/rev feed. I tried pecking 3 times just to get some oil in the hole, I know carbide doesn't like pecking much.


anyone have any tips for drilling this hole?? Also, the material is quality Ugine material... so no issues there.


thanks!

[gizmo_454]

Hello,

Drilling 304SS is a walk in the park. I routinely run a job using a #10 (0.1935") drill in 304 using a Guhring GT100 high speed cobalt drill. I think the problem you are having isn't the drill, it's the SFM. My Guhring book calls out, for the drill I am running, 25 SFM and 0.002" IPR. I have been successful getting this drill up to about 45 SFM without any adverse effects, leaving the feed at 0.002" IPR. I am only going 0.900" deep, but I am using the 0.200" peck you are. I have been using the same drill now, without sharpening, for about the last 1500 parts and it's starting to look like it is going to need to be replaced.

If you have a large run of parts, and the job warrants it, and you have HP coolant, I would give the folks at Mitsubishi a call. Their drills are pricey, I'll give you that, but I have found no better carbide drill and certainly no better customer service in my area than them. Second to none in the Northern Michigan area! I use their MWS drills in 303, 304, and 316 all the time. Come to think of it, there is one running right now. 0.319" Diameter, drilling 1.300" deep, 2500 RPM, 0.006" IPR, no peck in 303SS.

Sorry for babbling. Just lower the speed with your cobalt drill and you should be good to go.

Good luck,
Mike

[michaelhobbs]

Hello.

What machining oil are you using? Also, what type of machine?

Regards,
Michael Hobbs
Blaser Swisslube, Inc.
704-299-1321

[MikeMc]

I agree with Gizmo....SF way too high. With Mitsu or Titex coolant through drills, we drill at 130-170 SF in 304 with the Ugine material and average about 4000-5000 holes. The drills are expensive, but that is a lot of holes.

[cbr_speedster]

Drop the pecks to .1 or less. That small of drill with a .200 peck is packing up down in the hole. Is the peck cycle a full retract?
I run coolant thru carbide at 125sfm / .004ipr all day long with no problems.

[gizmo_454]

Hello.

What machining oil are you using? Also, what type of machine?

Regards,
Michael Hobbs
Blaser Swisslube, Inc.
704-299-1321

I run KoolRite 2290 (semi-synthetic water based) in our Haas machines and Blaser's Vascomill 22 in our Citizen E32. Both work well in their respective machines.

Mike

[PoiToi]

Wow! thanks all for the replies!
This is on a Citizen A20 machine.
We just run regular old screw machine oil in all of our machines.
I'll drop that SFM way down and see what happens!

And unfortunately we don't have HP coolant on any of our machines.

I do have a standard uncoated carbide twist drill here i thought would do quite well, what SFM should I use for that?


And gizmo, where do you get a guhring book?? That sounds *so* damn helpful!!

[gizmo_454]

HP coolant would be nice. Unfortunately, I'm in the same boat you are...without any.

As to the uncoated carbide drill, without know the manufacturer, point type, etc., it is kind of difficult to nail it down. I would say a "safe" starting point would be 1200 to 1500 RPM and 0.0025-0.003" IPR. Again, just a guesstimate. I have heard that carbide does not like peck drilling. True. BUT...If you manually program the peck cycle, line by line, and have the drill stop not 0.010" above the bottom of the hole, but 0.030-0.050" above the bottom and then begin to feed, it will allow the chip time to get into the flute of the drill, instead of smashing it with the drill, breaking the drill. Yes, I know... It will add cycle time. Which is better? 1) A few seconds per part cutting air for the drill's safety's sake. Or 2) 5, 10, 15, 20 minutes or more replacing a drill because it broke from a chip at the bottom of the hole.

I have successfully peck drilled implant grade 316SS @ 32HRc using carbide drills. The above method was the only way that worked for me in that application. Ugly job!

As for the Guhring book... Call your tooling rep. If they deal with Guhring, they should be able to get you a book without any problems. Just remember, Guhring, like Mits., OSG, PTD, Morse, etc., only call out feeds and speeds specifically for their tools. In most cases, they very greatly between the different lines they sell. I only mentioned the Guhring book because I am using a Guhring drill. Also, the speeds/feeds they call out are "starting" points. They may have to be adjusted up OR down to fit your application.

Sorry again for babbling. I really try hard not to. Sometimes it just cannot be helped!

Good luck!
Mike