Recommendations for drilling 17-4

kapps · Sep 5, 2015

I have some 17-4 (presumably PH). I've been able to square up the block with carbide no problem but I'm having issues drilling. Feeds and speeds recommendations seem to be all over the place. I first tried HSS with too high a sfm and it quickly melted. Using a stub 5/16 carbide drill, I went with 60 sfm but only .001 chip load and it started getting ugly after a few holes. Work piece was also quite hot. I've seen recommendations for feedrate everywhere from .001 to .006 for drilling this stuff. My gut tells me I should be around .003-.004 ipt with this size drill but I want to make sure before ruining one. Anyone have recommendations?

Krovvax · Sep 5, 2015

For 17-4 your sfm is way too high i would start at 25 sfm 0.004 ipm dont rib it or its going to go bad quick.

Bobw · Sep 5, 2015

kapps said:
I have some 17-4 (presumably PH).

There in lies the first part of the problem... What condition is it actually in?

In the solution treated state (what a lot of times is called annealed, but its actually not)
17-4 behaves a lot like a 300 series... Its generally harder but you run into the gummy thing and
a bit of the work hardening thing... Once you heat treat that stuff it will act more like an alloy
steel (4140,4130,4340)and should be treated approximately like you are cutting an alloy steel of that
particular hardness.

Diezel · Sep 5, 2015

I've heard a lot of machinists talk about 17-4 like it's a major PITA.
However, at my first job in a machine shop I did quite a few jobs with this stuff.
I've always cut 17-4 exactly the same way as I cut 303 and it's always worked very well for me.
If I can find one of the old programs I will post an excerpt.

zero_divide · Sep 6, 2015

Your SFM is about right.
Feedrate is way too low, though.
Last time I ran it with these parameters:

Speee=57 SFM
Feed=0.005 ipr

With good flood.
Can up SFM by 150% if through coolant is used. Most problems I had was with subsequent tapping. This shiat refused to be tapped with regular coolant and demanded tapping oil.

In yourcase you would be rubbing the help outta it at 0.002 ipr. Hence workhardening and the ugly results.

gregormarwick · Sep 6, 2015

Do you know the condition? There is a large difference in hardness between H900 and H1150 for example.

DMF_TomB · Sep 6, 2015

gregormarwick said:
Do you know the condition? There is a large difference in hardness between H900 and H1150 for example.

.
i agree. different condition and hardness make a big difference in how it machines.
.
like trying to drill a hand file. obvious if a file is in annealed condition it is easier to drill rather than at 65 C rockwell hardness

Krovvax · Sep 6, 2015

zero_divide said:
Your SFM is about right.
Feedrate is way too low, though.
Last time I ran it with these parameters:
View attachment 148623

Speee=57 SFM
Feed=0.005 ipr

With good flood.
Can up SFM by 150% if through coolant is used. Most problems I had was with subsequent tapping. This shiat refused to be tapped with regular coolant and demanded tapping oil.

In yourcase you would be rubbing the help outta it at 0.002 ipr. Hence workhardening and the ugly results.

I dont want to be a smartass but i think you miss the part he said HSS twist drill. His sfm is way to high and you gave him the sfm/fees for a carbide drill.

kapps · Sep 6, 2015

Thanks guys. I initially started with HSS but moved on to a carbide drill with, as I suspected, too low a feed. I only have 12 holes so I have no issue going with a much lower SFM to get through it. 4 of the holes will be tapped 3/8-24 so once the 5/16 carbide drill has made the hole, I plan to go back with HSS to open them up to the proper diameter for the tap.

As for hardness, a file works fine on it and my carbide endmills have no problem cutting it. It doesn't act very gummy nor too hard. I just have no clue whether it's PH or not.

alphonso · Sep 6, 2015

Just finished a job on 17.4 cond, H1075. holes for 3/8 x16. Used a 5/18 cobalt drill at 733 rpm(24fpm) F2.2. .1 pecks. Flood coolant. 16 holes 1.031 deep. No problems. Threadmilled because of blind hole.

If this had been H1150, I would have doubled the rpm and feed. You really need to know what condition of material is, otherwise you're just shooting in the dark.

litlerob1 · Sep 6, 2015

Diezel said:
I've heard a lot of machinists talk about 17-4 like it's a major PITA.
However, at my first job in a machine shop I did quite a few jobs with this stuff.
I've always cut 17-4 exactly the same way as I cut 303 and it's always worked very well for me.
If I can find one of the old programs I will post an excerpt.

Try machining 17-4 PH 1075 where the OD of the parts less than .5", and has three Datums (OAL and HEX) and 2 features on each side that are drilled-tapped bolt circle (0-80x.125 deep), and a bore that is .075" thru +.0002-0.0. I hate 17-4 if I had to drill some big ass holes I probably wouldn't bitch so much, but the chips man the chips. I always say, I would like this job a lot more if it weren't for chips and chatter.

Robert my ±2

michaelwatson5 · Oct 31, 2023

kapps said:
I have some 17-4 (presumably PH). I've been able to square up the block with carbide no problem but I'm having issues drilling. Feeds and speeds recommendations seem to be all over the place. I first tried HSS with too high a sfm and it quickly melted. Using a stub 5/16 carbide drill, I went with 60 sfm but only .001 chip load and it started getting ugly after a few holes. Work piece was also quite hot. I've seen recommendations for feedrate everywhere from .001 to .006 for drilling this stuff. My gut tells me I should be around .003-.004 ipt with this size drill but I want to make sure before ruining one. Anyone have recommendations?

Use Cobalt drills, 50 sfm and .001-.002 chip load peck about .05 to start and go from there.

VTM · Oct 31, 2023

That Is an 8yr. Old post. :dopeslap:

And the OP hasn't been around for 4 years? :nutter:

mhajicek · Oct 31, 2023

michaelwatson5 said:
Use Cobalt drills, 50 sfm and .001-.002 chip load peck about .05 to start and go from there.

Think OP was waiting eight years for an answer?

LOTT · Oct 31, 2023

Hey, sometimes it takes a minute to get things dialed.

Search

Largest Manufacturing Technology Community on the Web

Search

Recommendations for drilling 17-4

kapps

Cast Iron

Krovvax

Hot Rolled

Bobw

Diamond

Diezel

Aluminum

zero_divide

Stainless

gregormarwick

Diamond

DMF_TomB

Diamond

Krovvax

Hot Rolled

kapps

Cast Iron

alphonso

Titanium

litlerob1

Diamond

michaelwatson5

Plastic

VTM

Hot Rolled

mhajicek

Diamond

LOTT

Stainless

Similar threads