[metalhogger]

I am looking for some tips on drilling 304 ss. I am using a haas vf 3.

drill sizes are 7/16 and 3/8 dia. black oxide precision twist drills (standard jobber length).

current setup is 55 sfm .005 feed per rev. flood coolent, peck full out at increments of 1 drill dia.

I am drilling thru 1-1/4 hot roll plate.

I have had some success. but i also have had a few drills burn up in the hole
mostly at between 1" depth and greater.

I dont have a lot of holes to do but i need to get a handle on drilling ss 304

thanks
Mike

[Geof]

Try cobalt drills and increasing your peck distance.

Stainless work hardens so every time you peck the drill has to punch through a work hardened surface, increasing the peck distance reduces the number of times it has to do this.

If the chips are coming out of the hole nicely you might be able to go to 2 or even 3 diameters.

Another thing with stainless is that just when the drill is breaking through it get very hot necause there is not much metal below the cut to act as a heat sink. Try to arrange your peck distance so you pull out a little bit before break through so the hole can fill with coolant and cool off.

[TOTALLYRC]

Try cobalt drills and increasing your peck distance.

Stainless work hardens so every time you peck the drill has to punch through a work hardened surface, increasing the peck distance reduces the number of times it has to do this.

If the chips are coming out of the hole nicely you might be able to go to 2 or even 3 diameters.

Another thing with stainless is that just when the drill is breaking through it get very hot necause there is not much metal below the cut to act as a heat sink. Try to arrange your peck distance so you pull out a little bit before break through so the hole can fill with coolant and cool off.

Hi Geof, just to clarify, you are saying that if I am drilling a 1 inch deep hole using a 3/8 drill, I would set the q value to say 0.475", so the second peck would finish at 0.950" and the hole would fill and then the final peck would only have to cut 0.050"???

I will be doing some stainless work in a few weeks and would like to be on top of it.

Mike

[Geof]

Yes that is what I am getting at; although you have to consider your R distance; your numbers will work if R is 0.


EDIT

You can always try a trick I have used; clamp the part down firmly to a sacrificial piece of aluminum so the drill never breaks through, it goes into the aluminum which acts as a heatsink.

[TOTALLYRC]

Thanks for the tips.
R, Q, F, they are all the same to me. LOL

Mike

[Mooser]

I've had pretty good luck with MA-Ford HI-TUFF, series 205 drills. Been drilling through 304L 1/4H sheets, (mind you only .250 dia and .093 thk) but one drill will do several hundred holes before needing to be touched up where my cobalt drills were only doing about 30-40 holes.
Found that the feed had to be fairly aggressive to keep ahead of the work-hardening, flood coolant, no-peck (thin material). If you machine dwells at all on the bottom of the hole before pecking out it might be an issue.

Prior to this I was using cobalt drills, the point of the drill seems to be what normally fails and then the thing melts on the next hole. because my material was thin I went through with a c-drill and that seemed to help, guess it's the near zero sfpm at the center of the drill bit that really suffered
Mooser

[syamin]

Mike, When drilling SS the best you can do is program a feed per revolution, Start the feed about 1mm over the surface, do not peck and do not dwell. Use cobalt or Carbide tipped Hss bits. Use a hard surface to support, plenty of coolant. The trick is to try to always cut the exact amount of materal and avoid rubbing of the tip against metal. By doing this the heat is carried out by the chip and material will not harden with work.

Santiago Yamin
Mexican Aerospace Components.