What's new
What's new

First time working with 303 stainless, would need some pointers


Nov 22, 2023
Hi everyone, I'm quite a new CNC machinist. So far I've made made simple parts using a HAAS TM1 mill. I'm the only CNC guy in the shop (as my shop is an automation one) so I have no one to turn to for advice. I learned everything myself from scratch.
I'm getting a job on 303 stainless steel. There are 25 parts, each one is 3.7" wide, 1.023" thick and 7" long. Stock size is 4" x 1.25" x 7.15".
I'd like to ask several questions, hoping you guys could help me out, I would greatly appreciate it.

1. When face milling, I supposed doing it without coolant like with steel and I'll run it only 80% of what I did on steel (1150RPM, 0.005 IPT and 0.07 - 0.100 DOC). Is that correct? My face mill is not the coolant-go-thru one.

2. When slotting, I use a 4FL carbide 0.5 endmill, 325 SFM, 0.002 IPT, 0.200" DOC. Would it be okay for the best tool life?

3. Please look the the pic below, in order to achieve the red circled dimensions and a better shinny finish, should I use carbide insert face mill or endmill?

4. I asked some people about 303 SS, they said it tends to warp. What does it mean and What can I do to prevent it?

5. To rough the stock, I'm planning to face mill 4 parts at a time, shaving it down from 4" to 3.7, leaving 0.04" for finish. Does it sound good? Or I should be using a 5/8 endmill to side mill it?

Any pointers, ideas or thoughts would be appreciated, thanks again.

Last edited:
Okie dokie...
1. For your face milling, .005 IPT sounds ok (maybe a little slow, but I'll bet you get a good surface finish if that's what you're after). 1150 RPM doesn't mean anything to us because we don't know the diameter of the cutter to convert RPM into surface speed (SFM). As far as coolant, I've never had problems running coolant when cutting stainless, but I've not done as many stainless jobs (or as many pieces per run) as others on this forum - just my $.02

2. 4-flt carbide endmill is likely an excellent choice for the large slots/open pockets on this part. If possible, I'd avoid the full-width slotting at .200"; instead I'd run full depth (axially) at stepovers of about .050" using an adaptive path (or even just straight lines if you don't have CAM software)

3. Probably either cutter would work. I'd rough the area out and then come in with a new, sharp cutter (probably with some kind of nose radius/bull end) to finish the floor

4. Warping (in metal) is caused by stresses that are pent up in the steel. When you cut material off one side of the block, the stress on the other side acts like a spring and turns your part into a potato chip. You can get metal stress-relieved (similar to, but not synonymous with, annealing) at a good heat-treating service. This relaxes the material so it's not so springy. Something else to minimize warp is take small slices and alternate sides. Instead of cutting a 1" bar down to 1/2" thick in one go, you might take 1/4" off each side, or 1/8" off each side twice (alternating between). This way the stresses can kinda cancel each other out, leaving you with a neutral piece of material.

5. Whatever floats your boat, man. I personally would square all 25 blocks (again, getting rid of the stressed "skin" evenly). Then I'd do the "bottom" (the side with the two open pockets and a few holes), then flip the part over and register off those pockets, clamp by the holes, and do the entire topside at once, profiling around the outside unhindered.
Always use coolant on stainless, or you get built up edge (the material sticks to the cotter).

Check HSMAdvisor for feeds and speeds.

I've been running 303 with TiALN coated endmills with air blast and haven't noticed any built up edges at all.
Hi mhajicek:
As you may know 303 has got sulfur in it to make is free machining.
If you've never cut it, it's unlike any other stainless except maybe 416.
It is super easy to cut...almost like Leadloy.
You can probably cut it with a butter knife...it's that easy to work with.

I've milled a ton of it and like triumph406, I don't always bother with coolant except for drilling, tapping and reaming.
I also use TiAlN coated cutters and just let 'er rip...almost like milling 7075 aluminum.
Rarely I will use MQL if I need a particularly nice finish.

I've also turned a ton of it, and in that process a flood application of straight cutting oil does wonders for the finish.
Here's a set of decorative finials for a 1930's era safe I cut from 303 for a buddy.
They were turned with oil

But it does warp like a bastard.
Here's a closeup of a stock remnant after wire cutting a rotor out of a slice of round bar:
You can see how it's collapsed the slot...that's stress release doing it's magic.
The rotors I made out of 316 didn't do that.


Last edited:
2. End mill choice- higher flute count usually work better, smoother in the cut and longer life. At least 5 flute if not more. And like Baja said bull nose helps too if you can get away with the radius.

Definitely use coated endmills (TiAln or AlCrN probably?), and in stainless I do use coolant. Most of what I cut is 304 and 17-4, so maybe it's just a holdover from them.
Interesting. I've always run coolant on stainless because I was told I'd get material adhesion. Experience trumps rumor though! How about for drilling and slotting?

Normally I run flood coolant on all materials.

The coolant 585XT has gone bad, so before I get to clean out the tank I had to run some 12L14 and 303 parts.So decided to run with air blast. And to be honest much prefer it to running with coolant. For drill and reaming I use oil applied with a brush. Cobalt drills could probably run dry. Slotting is ok as long as you can get enough air in the slot to evacuate the chips

I use a very carefully directed nozzle, so don't waste air. I have a 3hp compressor and 40 gallons air capacity
Thanks very much everyone for your input, I really appreciate it, especially Baja.
Im working on it now, so far it's been good.
One problem is when I cut this curve profile, using a 5/8 carbide endmill, 4 flutes, 0.030" stepover, 0.0069" IPT, 250 SFM, two 1.15" DOCs, and the tool was like screaming. Any thoughts? Thanks
Thanks very much everyone for your input, I really appreciate it, especially Baja.
Im working on it now, so far it's been good.
One problem is when I cut this curve profile, using a 5/8 carbide endmill, 4 flutes, 0.030" stepover, 0.0069" IPT, 250 SFM, two 1.15" DOCs, and the tool was like screaming. Any thoughts? Thanks
I'd turn your chip load down a ways. You could try .0015 IPT (light, yes, but I don't know your setup :D ) and work your way up from there.

I'm assuming (based on the two 1.15" deep cuts) that the curved surface is "standing up" and you're profiling it instead of surface milling it while laying down? That means your tool is hanging out a good 2.5" away from the toolholder, in addition to how far the tool holder hangs out past the spindle nose. Are you sure that your endmill flutes are long enough to cover the entire 2.3" total DOC without the shank contacting the part?

If you have tools available (and a machine with the beans to handle it), try stepping up in endmill size (like a 3/4 or even a 1"). If not, I'd say grab an insert cutter and hog your way down in multiple steps. Then profile the final surface with your 5/8" cutter (take like .015" @ your 1.15" DOC and slow your surface speed down to avoid chatter)