[artin5]

Hi guys,
I have to drill a series of holes .060" diameter X .380" deep in SS304. Anyone have experience with this? I am planning on using 3000rpm and using a feed rate of 1.5in/min while pecking .030". Any feedback on these numbers?

thx

[pushchin]

I've just completed a job in SS304. The stuff is ugly to work with, but not the worst. Your best bet on getting good numbers is to contact a local industrial supplier. I can't comment on your numbers as my parts got 1.5" holes. A few things I can suggest are:
1/ SS304 is sticky and gummy. Your tools must be sharp!
2/ does not work harden, but the feed must be aggressive enough to cut not grind.
3/ use LOTS of coolant and keep the tool cool.
4/ have lots of spare drill bits handy. If there is any sign of wear, replace the bit. Cobalt bits work better than HSS as they can take a bit more heat. Coatings help with lubricity.
5/ did I mention lots of coolant? neat oil lubes well, but does not cool as well as a water based coolant.

I suggest you try some sample holes in a scrap piece until you get the speed/feed/bit/coolant combination right. When you establish these parameters, write them down and keep in a safe place.
Hope some of this helps.

[artin5]

Thanks for the tips. I plan on using flood coolant for this job. I ordered the shortest length drills possible, i think it should be ok.

[kalmah]

I drill SS316 every week. It's more difficult to drill than 304.

First question:

What kind of lubricant do you use: The cutting parameters are so different if it's cutting oil or water soluble oil.

1) 3'0000RPM is very low cutting speed. If I compute the cutting speed it's 13m/min. It's TO low !!! YOu should go at 9000 RPM

If you use cutting oil:
Use this cutting parameters:
n = 8000 RPM (with carbide tool) n = 4000 RPM with HSS tool
Vf = 200 mm/min
Pecking cycle = 0.2xD if you use emulsion oil, 0.5XD if you use cutting oil.

If it's not possible to go higher than 3000 RPM, reduce the feed proportionally.
Use a smooth coating for your drill.

Of course, do a center hole before drilling

I think that you can have a tool life higher than 1000 hole with carbide drills

[artin5]

Hi kalmah,
Thanks for the tips.

1- the coolant that i use is water soluble.
2-I have maximum 7000rpm
3-Wouldn't the higher rpms work harden the 304? I don't really need agressive feeds for this job, it's only for 5 pieces.

thanks again

[kalmah]

OK. IN my experience, it's not good to turn at the maximum of spindle.
With 6000RPM, it doesn't work harden. Austenitic stainless steel work harden whatever the speed. Of course it's very local.

Use 6000 RPM
Vf = 80mm/min

Pecking cycle = 0.2xD

Of course it's not the optimal cutting parameters if we consider the cost per hole, but you have only 5 pieces to drill.

It should work without problem

[artin5]

Hi everyone,
Just to let everyone know how the drilling turned out. might help someone. Here are the final parameters are used to drill the SS304 with a .060" drill .400" deep.

1-Stub Length HSS drill with black oxide finish
2-6000 rpm
3-Feed 2.5 ipm
4-Flood coolant
5-Peck .015"

i managed to do 15 holes (the whole job) without breaking the drill. Hope this helps.