Drilling 17-4 Rc35

First 17-4 parts. Cutting the overall shape and putting slots in went well. I used a cobalt U size drill to start the slots. Today, I need to put a couple U sized holes 1.5" deep. The drill broke on the first hole (did two holes yesterday without issue). I was running it 225 RPM, 22mm/min (just under 1 IPM), flood coolant, ER25 collet on a Speedio. Material report says HB313 which I believe to be around Rc35. Any advice?

I don't memorize the letter sizes, and I don't care enough to look it up. You don't mention the condition of the material so that doesn't help. It would help if we knew what style of Drill, Peck amount and if the hole is through or not. It would also help to explain what "Drill broke" means exactly, like in half?

R

U is .368". The material is in the annealed state. Hole is blind, but it drilled a couple through holes yesterday in .750" thick material. It pecked once yesterday when the first hole didn't go through, so I went back and finished it. I was planned to peck this hole once, but it didn't make it that far. Drill is cobalt jobber from McMaster. Tip is pretty mangled. I heard a pop and stopped it a second or two later.

I need to ream it to be .375". I have a cobalt reamer for that. A local place has carbide 9.3 and 9.4mm drills for 80 each. I thought cobalt would be able to do this though.

Thanks

feed per rev is just under .004" Maybe not enough?

If you're running it on a Speedio, buy a coated carbide drill.
If you buy crap tooling thinking you're saving money, you're wrong a lot of the time.
A .368" carbide drill isn't going to break the bank, it will pay for itself in no time.
BUT
if that's the only drill I had, I would run it around 30-40 sfpm with a .006" ipr feed for starters with flood coolant.

Broken drill looks like too much feed.

I would increase your speed a bit and cut back the feed, myself.

Now were cooking. Annealed can be pretty gummy, unless you have TSC I wouldn't use Carbide. And I would peck Drill it for sure. I would at least double the RPM, 21 SFM is really slow, and I would jack the chipload up to .0057" but only with the RPM increase. At that super slow RPM you need about 10 miles of Rigidity. I would definitely change to Stub length/Screw Machine 135º split point Drill.

As a rule of thumb, in the Annealed condition-I treat it like 304.

R

I'd be around 50-65sfm, (approx 540-700rpm), and approx .003/.004 per rev., flood coolant, and you should be good. 35rc isn't anything to be scared of.

I found this older thread: link

Based on recc's from that thread, I should be about .007" per rev. I also saw 35-50 SFM. I'm going to get a couple more cobalt jobbers and try again. 400 RPM, .0064" per rev pecking maybe 1/2". Thanks for the help.

17-4 in condition A can be a little unpredictable. No were near as bad as 304,
but it can vary a bit.. And it still has its sticky stainlessy properties.
Again not as bad as 304... Nothing sucks more than 304...

One thing I have found in workhardening stainless.. You have to be careful with
your pecks.. That chip is nasty, and if you rapid out of the hole without
cutting the chip off first, you can rip the cutting edges off of the drill...

Generally pretty easy to add a dwell (But don't let it rub of course ).. I longhand it when
I have to, feed back out .020" or so, then rapid, or fast feed back in to the same
point..

If I'm only doing a couple holes, I'll just turn the rapids way way down.


Another thought.. Stainlessy stainlesses can be nasty when you break out the back side.
Sometimes its productive to make sure everything is nice and cool down at the bottom
before breaking through, you may have damaged the drill on the through holes...

Another random though.. Speedio.. Are you out of the hole long enough to get coolant
into the hole before it goes back in.. Another little thing I do when I long hand my
drill cycles.. Not always, depends, I'll come up quite a bit further than my clearance
plane to make sure I get a new batch of coolant down into the bottom, and it also
leaves a bit more room for any chips on the drill to go away...

Quick story.. Lathe, and not stainless. 1-5/16" drill in 4140 I think it was.. Going
almost a foot deep.. Just a twisty drill, it was only 40 parts.. If I ran full
rapids, the bottom of the hole and the end of the drill would melt down.. If I ran
25% rapids, everything came out great.. Of course a well meaning employee saw the
rapids turned down, and turned them up and I ended up with a melted drill...

CosmosK said:

I found this older thread: link

Based on recc's from that thread, I should be about .007" per rev. I also saw 35-50 SFM. I'm going to get a couple more cobalt jobbers and try again. 400 RPM, .0064" per rev pecking maybe 1/2". Thanks for the help.

Click to expand...

Last place I worked we ran tons of 17-4/15-5/13-8, drill were always Cobalt. Can't help on feeds/speeds though.

Got a couple new cobalt drills. Re-ran the ops with the slot, then changed drill in case the exit did something. Got through the holes, seemed fine:

400 RPM, .0064" per rev (39 SFM). I used chip breaking macro every 10mm (retract 0.5mm not full). I started making some sounds the last few mm, I assume chips getting bunched up, but got through the holes.

Thanks all for the help!

RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.

I have had good luck on my cnc lathe running 17-4 H900 around 43r using I think a letter Q carbide drill from MariTool. I am running like 170sfm .0015 feed and pecking every .100 flood coolant with a total depth of around 5/8. Just got through with a 120pc run and the drill is still good.

Carbide Screw Machine Drills (stub length) - MariTool

TCasals said:

RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.

Click to expand...

report says solution annealed.. HB 313 which is around 33-34 Rc. I had looked around for bar stock in H1150 and couldn't find any. This is my first 17-4 job, so I probably need to find a better supplier. I got this material from online metals. The report says Bollinghaus Steel, South Africa.

Yeah, I got a 4mm carbide drill and made some holes at 5200 RPM.. nice. It's a small job, so I'd like to get through it without the $80 drill. Seems to be working. Thanks

TCasals said:

RC 35 is usually what we get at H1100, are you sure it's in solution A? It definitely likes being cut in a hardened state better. You really shouldn't have too much trouble drilling it with a half decent cobalt drill. We use a macro to dwell exactly 1.5 rev before retract for the peck and that works great for us even deep skinny holes.

Click to expand...

That's why some organizations (like NASA) don't like 17-4/15-5 H1150, because you can't do a hardness test and determine whether it's annealed or heat treated. Not an issue with H1025 (or standard ht) or H900

Cosmo, just curious. In post #12 you said it sounds a little crunchy the last couple mm, you suspect it's chips. But you are using chip break Macro.

Why aren't you just Peck Drilling, to get the chips out of the hole?

Most of Machining, is generating a hard enough chips that it breaks off of the work piece. So the chips are hard. Even when they aren't hard, they're still the worst part of the Machining process (particularly when hole making). Get rid of them.

I understand trying to reduce cycle time, but not if one hole takes 8 hours, because your brain is stuck doing it a certain way. Sometimes we kick our own asses.

R

litlerob1 said:

Cosmo, just curious. In post #12 you said it sounds a little crunchy the last couple mm, you suspect it's chips. But you are using chip break Macro.

Why aren't you just Peck Drilling, to get the chips out of the hole?

R

Click to expand...

I didn't want to come down on a chip. I should probably have done full retract way back and blowgunned the hole between pecks. Time is not an issue. This job has eaten most of my week so far and it's not worth that much.

That is a reality also. Coming down on chips sucks too. But the breakage I see in your pictures looks to me like swarf in the same space as the Drill.

But a part of the basic geometry of a Twist Drill, is to help chips come out of the hole when the Drill comes out. Like I said, sometimes I get so stuck with the original intent or plan of attack that it ends up bad for me. When stuff starts to get difficult, I try and take a step back and ask myself if this is the bast way, after all.

R

triumph406 said:

That's why some organizations (like NASA) don't like 17-4/15-5 H1150, because you can't do a hardness test and determine whether it's annealed or heat treated. Not an issue with H1025 (or standard ht) or H900

Click to expand...

I suppose there's something to be said that we only ever see these figures on our HT certs when the material comes back, but I assumed cond. A was way softer. Definitely better ways to test it, but being obligated to charpy test our parts every time sucks too.

OP, I would suggest finding a different supplier than online metals if you are doing any volume, but getting 17-4 in anything other than cond. A has been a crapshoot for us so far. We've just gotten used to shipping directly to our HT vendor.