Drilling 304 Stainless

Num1bigguy · Mar 28, 2018

Hi I am new here. I browsed a few posts, but was curious that if I posted some specifics if the answers would vary slightly. I currently have a piece of 1/2 inch thick by 33" wide by 38" long piece of stainless attached to my sacrificial aluminum subplate, in my FADAL 6030 circa 1995 Machine. I need to drill and ream 410 .755 holes in this plate and there will be 20 more plates to do if I can pull this off. I am for the most part used to programming/cutting aircraft grade aluminum, that we use for prototype plastic injection molds. I programmed this job trying to baby things a bit, because of the toughness of the stainless. My center drill made it through all 410 hole locations with no issues. My first drill to be a pilot is a 3/8 drill. Next it steps up to 23/32 drill and finishes holes with a .755 reamer. There is also a critical chamfer on all holes for welding later. The 3/8 drill did about 10 holes successfully at which point it began to sound worn. I removed the drill and sharpened a fresh edge on it and it failed again 1 hole later. Lather, rinse, repeat, with same result. I've read posts saying use this drill or this coolant. My machine does not have a coolant thru spindle. I use extreme-cut 250c coolant kept around 8%. Does anyone have some information that may help me to get to the dance? I also have 4 other machines to stay on top of daily so it would be ideal to not have to babysit the machine. I'd like to be able to walk away from the machine and have it not go to crap as soon as i turn my back to it. I would like to avoid using something other than my machines coolant. I've been able to keep this coolant at the proper mixture, and with skimming the coolant lasts for years. I don't want to contaminate it. Any information is greatly appreciated as I'm currently stuck.

Specifics
5/8 Drill depth
.100 peck
450 rpm
2 IPM
flood coolant, and machine is enclosed
I was trying to get by with my ding dong brand drill bit, at least for the show and tell for today when customer comes to check on progress, or lack thereof. Thanks in advance.
Also I've only been programming for about 5 years and I'm using Cimatron 12 and also using their automated drill for these toolpaths.

DMF_TomB · Mar 28, 2018

Num1bigguy said:
Hi I am new here. I browsed a few posts, but was curious that if I posted some specifics if the answers would vary slightly. I currently have a piece of 1/2 inch thick by 33" wide by 38" long piece of stainless attached to my sacrificial aluminum subplate, in my FADAL 6030 circa 1995 Machine. I need to drill and ream 410 .755 holes in this plate and there will be 20 more plates to do if I can pull this off. I am for the most part used to programming/cutting aircraft grade aluminum, that we use for prototype plastic injection molds. I programmed this job trying to baby things a bit, because of the toughness of the stainless. My center drill made it through all 410 hole locations with no issues. My first drill to be a pilot is a 3/8 drill. Next it steps up to 23/32 drill and finishes holes with a .755 reamer. There is also a critical chamfer on all holes for welding later. The 3/8 drill did about 10 holes successfully at which point it began to sound worn. I removed the drill and sharpened a fresh edge on it and it failed again 1 hole later. Lather, rinse, repeat, with same result. I've read posts saying use this drill or this coolant. My machine does not have a coolant thru spindle. I use extreme-cut 250c coolant kept around 8%. Does anyone have some information that may help me to get to the dance? I also have 4 other machines to stay on top of daily so it would be ideal to not have to babysit the machine. I'd like to be able to walk away from the machine and have it not go to crap as soon as i turn my back to it. I would like to avoid using something other than my machines coolant. I've been able to keep this coolant at the proper mixture, and with skimming the coolant lasts for years. I don't want to contaminate it. Any information is greatly appreciated as I'm currently stuck.

Specifics
5/8 Drill depth
.100 peck
450 rpm
2 IPM
flood coolant, and machine is enclosed
I was trying to get by with my ding dong brand drill bit, at least for the show and tell for today when customer comes to check on progress, or lack thereof. Thanks in advance.
Also I've only been programming for about 5 years and I'm using Cimatron 12 and also using their automated drill for these toolpaths.

.
1) hss drills dont do well in 304SS (cobalt or carbide better)
2) 30 sfpm is 120rpm per inch dia so 3/8 drill id be under 400 rpm
3) drilling 304 requires coolant
4) resharpened drill lasting 1 hole probably not resharpened properly or hard spot in metal or work hardened and you have trouble getting through it

doug925 · Mar 28, 2018

Wow, that's 8200 holes.
I would look to ghuring, iscar, etc, for a tailor made drill.
IMHO, preferably a carbide, or carbide tipped drill, made for 300 series SST.
Speak to the tooling reps, and ask for "bullet proof" (read: conservative) SFM and IPR recommendations, aimed at a predictable tool life.

You should be able to skip the center and pilot drills.
The time ($$$$) savings of the removing the center drill and pilot drills from the program, should pay for the carbide drills!
Also, you could probably shoot right for your Ø.755 with the drill alone.

You are going less than 1 Dia / depth, so flood coolant should work fine. (I can't speak to not wanting to contaminate you flood coolant, but you WILL NEED coolant on 300 series SST.)

Doug.

Mtndew · Mar 28, 2018

Does your Fadal not have the horsepower and torque to drill with a .735 or so drill?
I wouldn't even bother with a pilot drill to be honest, you're just making the part take longer and your 2nd drill would probably wear at the corners a lot faster with a pilot.
If you can't afford a cheap coated carbide drill, then get a coated cobalt drill.

Look at the replaceable tip drills, those would get you the most bang for the buck.
Seco,Iscar,Guhring and Kennametal all have good offerings.

With that many holes though, buying a GOOD carbide drill will pay for itself in no time.

doug925 · Mar 28, 2018

Mtndew said:
Look at the replaceable tip drills, those would get you the most bang for the buck.
Seco,Iscar,Guhring and Kennametal all have good offerings.

With that many holes though, buying a GOOD carbide drill will pay for itself in no time.

+1 on this!

YorkCNC · Mar 28, 2018

If for some reason carbide or replacable tip drills don't work out, try out OSG EX-SUS-GOLD drills. They are quite expensive but offer performance and life in 304 way beyond what seems like should be possible from a steel drill.

Larry Dickman · Mar 28, 2018

I think we almost made it a week without a new "Help drilling 304" thread.

I 2nd the OSG SUS Gold drills, for lower quantities they are the cats ass. For the op's quantities, we've used the Kennemetal replaceable tip carbide drills. No spot, no peck, just ram it through. They always come out on size within .0005 and dead on location. As good as if they were bored and reamed.

Num1bigguy · Mar 28, 2018

Mtndew said:
Does your Fadal not have the horsepower and torque to drill with a .735 or so drill?
I wouldn't even bother with a pilot drill to be honest, you're just making the part take longer and your 2nd drill would probably wear at the corners a lot faster with a pilot.
If you can't afford a cheap coated carbide drill, then get a coated cobalt drill.

Look at the replaceable tip drills, those would get you the most bang for the buck.
Seco,Iscar,Guhring and Kennametal all have good offerings.

With that many holes though, buying a GOOD carbide drill will pay for itself in no time.

I Don't see why it doesn't. I believe the machine has the 15hp 10,000 rpm spindle. I was merely trying to be on the conservative side because of the unfamiliarity with the material

Num1bigguy · Mar 28, 2018

Larry Dickman said:
I think we almost made it a week without a new "Help drilling 304" thread.

I 2nd the OSG SUS Gold drills, for lower quantities they are the cats ass. For the op's quantities, we've used the Kennemetal replaceable tip carbide drills. No spot, no peck, just ram it through. They always come out on size within .0005 and dead on location. As good as if they were bored and reamed.

I apologize for that. I assumed I'm not the first person to ask questions about drilling this material. I wish I could've spent the whole day browsing the forum, but the time isn't there for it while keeping 4 other machines running. To be perfectly honest I'd rather use a .020 ball and cut ribs all day than to be doing this stainless job. A big thank you to everyone that responded!

mmurray70 · Mar 28, 2018

Larry Dickman said:
I think we almost made it a week without a new "Help drilling 304" thread.

I 2nd the OSG SUS Gold drills, for lower quantities they are the cats ass. For the op's quantities, we've used the Kennemetal replaceable tip carbide drills. No spot, no peck, just ram it through. They always come out on size within .0005 and dead on location. As good as if they were bored and reamed.

+3. I would also choose a quality HSS drill over carbide. We used to use those OSG drills to do thousands of holes in 316 and I dont think I ever needed to sharpen one. Another good choice is Viking, sold from mcmaster as stub length drills. Not sure if they are available from mcmaster over 0.500 though.

I would also try and go through without pilot. I would try 275 RPM, 2.75 IPM, flood coolant and 0.150 or smaller pecks to control chips. If you cant get a quality HSS drill designed for stainless that size, maybe drill to 0.500 and open it up with a 3/8 EM. Hopefully be able to skip the reamer then. Reaming might be another issue of its own anyway.

litlerob1 · Mar 28, 2018

I would drop the Spot and Pilot right off away. Your Feeds and Speeds seem okay for HSS. If you are going to use Carbide get a 304 specific coating, 304 is soft crappy material that will stick to the Tool.

I am going to go against the other guys on this one and say stick to HSS. JMO you have no Coolant through, so you may need to Peck, and Carbide doesn't like Peck Drilling. It's more than half the diameter, soooo? But it's up to you. I like the OSG SUS gold Drills. You can probably hold pretty close to size with just the Drill, or you can also get a 19.1mm Drill from OSG.

R

HuFlungDung · Mar 28, 2018

For that depth, I wouldn't peck with a full retract, I'd use a high speed peck cycle (Haas G76) to provide a chip break if you merely want to break the chip coil, but you don't want to come down on top of a chip which is the danger when using a full retract.

Tweak the feed higher and the rpm lower when experimenting. You can push a HSS drill pretty hard if you don't overheat it. Getting scared and backing off the feed and cranking up the rpm is the most common mistake.

Drilling the pilot hole is very bad for the drill that follows: it will have a bitch of a time stabilizing itself and will chip the cutting edges.

mhajicek · Mar 28, 2018

When people are recommending HSS here, I'd read that as "Cobalt". Same toughness as HSS but lasts longer, and only a few pennies more expensive. I've had to drill deep oil holes in some tough prehard steels (don't remember the specialty alloy that was giving me so much trouble) and the only thing that would do it was a cobalt drill. Carbide would snap, and HSS would dull and burn, Cobalt just sailed through.

tay2daizzo8 · Mar 29, 2018

with that size hole and that quantity you need to go carbide plain and simple.
heres what i do in 304. no coolant thru

iscar chamdrill .578 dia

G0G90G55X0.Y-.66S844M3T10
G43H9Z.1M8
G98G82Z-.8887R.1F5.3
Y.66
G80Z.1

your waisting money babysitting a spot and pilot that fail prematurly and dont need to be there to begin with.
hell you can probably get one on test, do the one piece you need, then decide of its worth it

Dupa3872 · Mar 29, 2018

If he's going to drop the pilot drill he better have the right drill for this or he will run into location troubles. This guy is running aluminum all day and as we know 304 is a much tougher dog. My 2 cents...Is sick with coated High speed or cobalt and change the drill out before it gets dull. 304 will work harden so a dull drill at too high a speed is trouble. People gave real good advice on speeds and feeds take it.

Use a short 135 degree split point drill. This material will rip the lip right off the drill as it rapids out of the hole while pecking so watch your chip load and go easy as you can on the feed rate to keep it thin. If your location is critical I would think about drilling it under size then dropping in with an end mill after the drilling and circle milling it undersized then reaming with carbide. Use a carbide 45 degree cutter and circle mill your weld Prep's

Circle milling might add time but will assure you are on location and getting a good hole for reaming. If you are doing this many parts It will also assure you wont be fighting / baby sitting this all day and can walk away to do other things while it's running.

Good luck

Make Chips Boys

Ron

exkenna · Mar 29, 2018

Lots of good advice here whether you go with M42 or Carbide.
One thing: solid carbide in the larger diameters is expensive, you're paying for all that material in the shank that's not doing any work.

Indexable drills are horrendously expensive but there is one tool that's reasonably priced and very robust. It's the Komet clone from Ultra-Dex. Uses a beefy WCMX style insert in the $8-9 range. It's a roughing drill and may go a little oversize so the reamer should go right through to finish at .755

The drill is only $130 and while it's not the latest technology it's still a solid performer and a worthy investment. Here it is:

UD- :cloud9:

-2D-75 - Ultra-Dex USA

Mtndew · Mar 29, 2018

exkenna said:
Lots of good advice here whether you go with M42 or Carbide.
One thing: solid carbide in the larger diameters is expensive, you're paying for all that material in the shank that's not doing any work.

Indexable drills are horrendously expensive but there is one tool that's reasonably priced and very robust. It's the Komet clone from Ultra-Dex. Uses a beefy WCMX style insert in the $8-9 range. It's a roughing drill and may go a little oversize so the reamer should go right through to finish at .755

The drill is only $130 and while it's not the latest technology it's still a solid performer and a worthy investment. Here it is:

UD-75-2D-75 - Ultra-Dex USA

That's a hell of a price!

Num1bigguy · Apr 13, 2018

Thank you everyone for the advice. I settled on a tool from Ingersoll. Its a pricey insert but has been very reliable. With having their tech in house we were able to work on speeds and feeds together. We settled on those in the titanium range. It appears this plate is a bit harder than what its supposed to be.

Ox · Apr 13, 2018

Is this tool a re-badged ChamDrill?

Or something different?

Are you going straight to full D in one hitch?

Got a link?

--------------------

Think Snow Eh!
Ox

Rapid_Tech · Apr 15, 2018

I'm not sure what that Ingersoll drill looks like but I'd really look at a flat bottom indexable drill like an Iscar DR or Sandvik 880.

I personally use an .75" Iscar DR drill in all types of materials including 304SS and it never even flinches. In stainless I usually run 2000rpm & 2ipm in a Haas VF2 without TSC. If the hole is really deep, 2"+, I'd peck every .5" but under that I just go straight in. Insert life is really good and the finish looks almost like it's reamed.

Drilling 304 Stainless

Plastic

Diamond

Titanium

Diamond

Titanium

Plastic

Titanium

Plastic

Plastic

Stainless

Diamond

Diamond

Diamond

Hot Rolled

Stainless

Stainless

Diamond

Plastic

Diamond

Aluminum

Similar threads