What's new
What's new

Machining 304 SS?

klew408

Plastic
Joined
Oct 6, 2017
Hi All,

Long time lurker here, first time posting
I am having problems machining 304 stainless steel.
Material thickness is .090 20in x 7in sheet and need to drill some .248 (6.3mm)holes in it.
I currently burning up my drills and having to perform my cut through using a 1/4, 4fl Endmills at a really slow feed in multiple passes.
Any recommendations on tools and feeds and speeds? Any help is appreciated, Thanks!

background
-rookie programmer on Mastercam
-Machining for 2 years
 
Stainless work hardens if the drill slips at all, then you are finished. So you need low rpms and a high feed rate to keep the chip coming out of the hole.
 
Backing the 0.090 material with anything?
As soon as you get deflection you will get uneven cutting, most likely a nice burr when you break thru
 
I am using a durostone backing board and clamping all around the perimeter, burrs are significantly present but manageable. I would like to improve the cut too.
 
I think he wants to burn up fewer drills, not a higher number of more expensive drills.

I already burned an OSG drill... no bueno
Looked up recommended speeds and feeds but my machine caps out at 10000 rmp.
 
Without looking at a chart anything over 2000 rpm your going to be welding drill tips.....and the ss changes into a new harder material
 
Yeah 10k in 304 seems crazy high speed for any cutter material I know of, and I loves me some crazy high speeds. I mean, Morse recommends 75 SFM... in solid carbide. So 1100 rpm and 3.3 IPM.

That's solid carbide. In HSS probably 600 rpm and 2 ipm.

If you feel like you're running out of RPM at 10k I can only imagine...
 
.09" thick material 20" long X 7" wide. You need to use a Bridge clamp or 2 across the 20", that part is going to vibrate and bounce around like a Fremont St. Hooker without it.

Do you have through spindle coolant?
Do you have access to a punch?

Get down to 100 SFM with a carbide drill, thats about 1/2 what the manufacturer is going to recommend. But unless your set-up is tight, tight you'll need it. You can't go too slow with the spindle, once you get good holes then speed it up.

I would use this drill::Guhring, Inc. - Tool List. Don't spot, don't peck. Eventually it'll look like your drill is punching holes, which it should.

R
 
Yeah, with that size you are going to need clamps across it at least. If there are quite a few to do I might probably make a plate to clamp the part, that has clearance holes for the drill. If all you are doing is drilling. Maybe bar clamps, and drill in sections, and work your clamps along the part.

Personally I would think cobalt drill would be better. I drill SS at 40 sfm and1 IPM. It's not fast, but the drills don't break either. One of the main mantras of the machine shop, "slow is fast"
 
I would 2nd the search idea. I think there is a new thread "Help Drilling 304" a least once a week.

10k rpm is insane. How ever you came up with that number is unbelievable. Get a good coated cobalt drill. Guhring or OSG, use their speeds and feeds. No spot, no peck.

As far as clamping, I would suggest a sandwich plate.
 
Just drilled around 900 holes in 304 using .024" (0.19" deep) and .035" (.07" deep) drills. Used Guhring .024" drills and they worked but only after clearing chips after every hole. I used Guhring's feed's (.0003" IPR) and ran the small drills at 10K per Guhring's recommendations. For the 0.035" drills I used these: McMaster-Carr. I know these are bit smaller than what you are working with but if I had to do it again in a bigger size I'd go straight for a carbide drill (most likely Guhring) and use their speeds/feeds. Running Qualichem XC 250C without through coolant.
 
10000 rpm ?. Is this a router ?.

This is a good question - it would help to know the machine (and condition) you're using, as well as tooling setup (collet/drill chuck/?), coolant and concentration, etc.

Ditch the Durostone backer, it's abrasive and if you're using HSS drills they'll be dulled further by it. Use Al or another sheet of SS. Better clamping for stability will help, and I'd second using a cobalt split point drill, stub ideally held in a good collet chuck. I'd go with 500-600rpm to start, around 2 to 3ipm. Faster feed is better as long as you can control the stock and tool, don't want to pull the stock up and break the drill.
 
304 that is cold rolled or finished can be 2x harder to machine than annealed or stress relieved 304
.
the difference is hugh and is often the reason there is such a big difference in how different people machine 304 cause they are machining different metal hardnesses.
 
I have found a standard drill point does not work well drilling thin walled materials and a Flat Bottom Drill is the way to go. The Flat Bottom Drill works off of the 2 outer points giving you a truer hole (which should help drill life significantly) and leaving less of a burr. If it is short run then I would just modify a Cobalt Drill you have in house with a flat bottom.

If you have a lot of holes to drill then I'd go with a Carbide 2 Flute Flat Bottom Drill/Counterbore Tool. Any flat bottom drill should work well, the ones I have had the best luck with in drilling thin walled materials in stainless is Kyocera's:
2ZDK63S - Kyocera - Shop ToolHIT
*Run at 150 SFM and .002" IPR
 
Hi All,

Material thickness is .090 20in x 7in sheet and need to drill some .248 (6.3mm)holes in it.

What kind of coolant are you using? Oil? Water-soluble? If you're mixing water and something try upping your percentage. Whenever we run stainless around here we find much happiness in a higher concentration of coolant to water.
 








 
Back
Top