Machining 321 Stainless Steel

[Dtuck]

Drilling a hole pattern in 2" thick 321 Stainless and tools aren't lasting. Carbide reamers getting chewed as well as drill bits. Any materials, speeds or feeds to recommend? High speed steel the only one going past one hole so far. Suggestions? Thanks.

 

[bill1898]

You have not indicated the diameter of hole you are drilling. This is very important as the drill penetration rate may be limited by its strength. My experience in drilling 300 series ss is that the cutting edge needs to be be moving at a vigorous pace in order to avoid work-hardening. A chip load of 0.002 inches per revolution is an absolute minimum. For carbide drills a starting point might be 300 sfpm. Assuming a 1 inch dia. double fluted, carbide drill, the spindle speed would be about 1200 rpm and the penetration rate about 4.8 inches per minute (@ 0.002 inches/flute x 2 = 0.004"/rev.). Coolant should be used only if you can GUARANTEE that it will be deluging the cutting area CONSTANTLY! For a hole this deep a so called "woodpecker" action could be helpful in clearing the chips created providing there is no time dwell between the forward advance of the spindle and its retraction. You need a good rigid spindle for this operation and the closer the cutting edge is to the spindle bearings the better the results. It is assumed that the workpiece is held rigidly. For reaming you need to leave at least 0.015"/side to remove in order for the reamer to work efficiently. I hope this is helpful to you. If the units I use sound archaic to you I must confess to being an older man and will let you do any conversions required. Good luck.

 

[MFredriksen]

Try cobalt bits. I work a lot with stainless 304/308 and these are the only ones that actually last longer than one hole. Try cutting fluid and a low speed.

 

[mrainey]

There's some useful feed and speed information here.

http://www.precisiontwistdrill.com/techhelp/help_pages/jobber_length_amg.asp

Software For Metalworking

http://mrainey.freeservers.com

 

[unclesyd]

Here is a little information on machining 321 several years back.
We were attempting to make fiber spinnerettes from 321 SS where we encountered some problems with tool wear. This was a serious problem as were attempting to drill and flat bottom 640 1/8" holes 3/4" deep. The problem was random as some material machined without any problems. It ended up that the problem blanks were from one heat. Checking the MTR and laboratory analysis revealed the Ti be at the max on MTR and slightly above by actual analysis. Metallurgical examination reveal inclusion like areas of Titanium Nitride. This was what was tearing our tooling up.
Several years later we had the same problem with 430 Ti SS in the same process.
Blanks for this process were cut from annealed plate.

You might want to check your MTR's for Ti on the high side.

 

[Dtuck]

Thanks for all your input so far. At 50 surface feet per minute we're getting five holes per high speed steel bit. I'm not ruling out the inclusions of TiN as acouple of pieces couldn't even be drilled. Thanks for all your help.

 

[droogeh]

I use sandvik 880 (U) tipped drills with 2020 grade tips in 321 stainless and other 'difficult' to machine materials (including c22 and c276 hastelloy). They work very well. Through coolant is a must but you can achieve tip life of about 4metres to an edge. Of course this will all depend on diameter and depth of hole. An example of use is a 25mm drill in 321 to a depth of 80mm:- 70m/min spindle speed , .033mm per rev feed, 30bar pressure coolant. We try to keep the swarf like tin foil (as opposed to what is usually told to you by tool reps. ie. heavy feed to introduce chipping) , we found that this was better in keeping the drill from trapping thicker pieces of swarf in the cutting area and causing clogging and tip failure.

 

[saberblue]

You may want to take a look at the fluids in use as well -- I test in 316L and can see a 50%+ change in the torque necessary to turn a tap or as much as 30% change in the thrust necessary to drive a drill -- as a standard practice I drill ream and tap holes thru holes in 3/4 in stock and measure HP, thrust and torque necessary to do the job -- fluids and make a major difference.

If the only issue here is to optimize tool life and hole quality look for a cutting oil 150+ Visa with Cl and active S



A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com

 

[AutoDrill]

Old post, but this might be helpful to you or others...

Vibration will kill carbide most of the time. See if you have the part / tools securely set-up and can you use drill bushings or guides?

Also, speed / feed rates can be guessed at quite reliably by checking the following web site:

http://www.multi-drill.com/drill-speed-chart.htm

Reaming is approximately 2/3 of the drill speed on RPM. Feed is dependent on material, cut amount, etc.

Good luck!

Regards,
Joe Agro, Jr.
(800) 871-5022
01.908.542.0244
Automatic / Pneumatic Drills:

http://www.AutoDrill.com

Multiple Spindle Drills:

http://www.Multi-Drill.com

V8013-R

 

[unclesyd]

AutoDrill,

Please click on this link thread404-230305 and see if you can assist the OP with his problem.
Read the whole thread to understand exactly what his problem is.

thanks

 

[dicer]

Carbide tipped drill. Don't remember SFM but I'd still keep it under 60. Peck drill it. I used to have to drill 3 inches with an under .250 drill through 321, that was some years ago. Can't remember the feeds and speeds. It took awhile to do. I would never use a highspeed anything on it. Maybe cobalt. And then SFM is cut in half. 321 likes to be cut slooooo

http://wwwww.

And with sharp tools. .001 to .0015 chip loadish not over .003 for tool life if memory serves. Look it all up in a machinerys handbook.

 

[T00lman]

321 Stainless is nasty stuff to drill. I recently had an application to drill 321 SS that was hardened and annealed according to the supplier to RC 32-36 (340Bhn max)We were drilling 2mm (.0787") diameter holes 10mm (.393")deep. Running "Walter Titex" A1249XPL-2 HSCO coated (XPL is a very hard coating) drills at 10M/Min (33 SFM) and 0.025MM/Rev(.001"/rev) = 40mm/min (1.57"/min) and getting 40 - 50 holes per drill before the drill broke.
This speed and feed seemed a little agressive so we slowed it down to 8.8 M/min (29 SFM) and 0.016mm/Rev (.0006"/rev) =23mm/min (.91"/min) Hole count went up by 29 %
Slower & HSCO, seems to be the way.