[floman]

Hello all,
I am in need of some advise on machining 303 stainless steel. I have machined plastics and aluminum, but no stainless. I will be using a RoboDrill CNC mill with 24000 spindle max.
I am starting with a 3"x3"x.375" thick block of 303. The rough finished part will be 2.5"x2.5"x.250 thick. It will have a 1.5"x1.5" square milled through the .250" thick material in the center. There will be chamfers on o.d and i.d of 45 degrees by .050". I will also be milling small .125" wide slots about .500" long and .150" deep on all 4 sides. one more thing , I need to engrave the part number on it , .010" by .010" wide.
I will be using carbide 4 flute end mills in standard sizes of 1/2", 1/4", 1/8", 1/16"
Not sure what to use for the engraving.
Anyway thats a little info on my project. If more info is needed please let me know.
I need feeds and speeds of course but also WOC and DOC of cut would be great.
Dry or Wet?
Thanks in advance for all the help!

[txcncman]

Start with a copy of Machinery's Handbook and become familiar with the milling speeds and feeds section. Then get the recommended cutting speeds and feeds from your tool supplier for the tools you plan to use. Use an engraving tool for engraving.

[fizzissist]

Use the same cutters that you'd use for aluminum, but that are designed for stainless. Also use the same speeds and feeds, WOC and DOC that you'd use for aluminum, but adjusted for stainless.

If you start burning up or breaking the cutters, just slow down till they stop burning up or breaking.

Some tools last longer cutting dry, some like it wet.

I know a guy who will be happy to generate your program and specify cutters, along with the appropriate data to run the job. He's not cheap, but in the end, it's efficient cost wise to pay for the expertise. He goes by txcncman, and he's pretty good.

It'll save you a lot of time not having to buy a Machinery's Handbook and go through all that literature.... He's already done that.

[zero_divide]

Hello all,
I am in need of some advise on machining 303 stainless steel. I have machined plastics and aluminum, but no stainless. I will be using a RoboDrill CNC mill with 24000 spindle max.
I am starting with a 3"x3"x.375" thick block of 303. The rough finished part will be 2.5"x2.5"x.250 thick. It will have a 1.5"x1.5" square milled through the .250" thick material in the center. There will be chamfers on o.d and i.d of 45 degrees by .050". I will also be milling small .125" wide slots about .500" long and .150" deep on all 4 sides. one more thing , I need to engrave the part number on it , .010" by .010" wide.
I will be using carbide 4 flute end mills in standard sizes of 1/2", 1/4", 1/8", 1/16"
Not sure what to use for the engraving.
Anyway thats a little info on my project. If more info is needed please let me know.
I need feeds and speeds of course but also WOC and DOC of cut would be great.
Dry or Wet?
Thanks in advance for all the help!

You can punch in your numbers and get a very good starting point here
FSWizard

There is also a desktop application that does the same and even more here
HSMAdvisor : Download

For slotting stainless you will have to use coolant.
Pick cutters with ALTiN coating that can handle alot of heat.
Here is a sample calculation->FSWizard

If you CAM package allows to use Hi Speed Machining, then the strategy is alot different.
Whenever your cutting speed gets above 400-450 SFM you have to ditch coolant and run it dry with airblast to clear the chips and cool the cutter a bit.
Here is a sample calculation for HSM speeds and feeds ->FSWizard

[UUU]

Beware that you might get distortion as you reduce the thickness of your block. I've done some preliminary machining on a bit of 6" x 1.25" x 0.375" stainless 303 bar (I've got 4 foot of it to get through).

I've taken this bit down to 0.250" thick in the mill, and have done some rough cutting and shaping by hand. It has bent this way and that quite a lot during this process.

I've tried to minimise the distortion by taking roughly equal amounts off each side, to get close to size, then finishing cuts.

[mflux_gamblej]

Slow down your speed, increase your feed. Stainless is bass-ackwards stuff. Unless you have thru tool and high pressure coolant, forget about running fast. You're lookin at 0.03" depth, 900 RPM (+/- 100 depending on machine / clamping), and 10 IPM with a half inch 4 flute carbide cutter (using old school flood coolant).

Rule number 1 = if you're making blue chips, or if your tool gets red (turn off the lights and look) you're going to go thru $200 in endmills and get nowhere.

blue chips = bad.

Also, you may want to rough with one tool and get a new one out for finishing.

This is not what the machineries handbook will tell you - but I learned from a stainless master (think nuclear weapons industry career machinist), and am pretty darn good myself now.


If your machine has high pressure coolant and can really run fast (10000 rpm) and you have trochoidal milling paths in your CAM, you might be able to go a different route here.

[Pondo]

303 stainless, any austenitic stainless steel is only minimally affected by heat.
The biggest problem is it work hardening on you - from pressure in the cut. This pressure comes from negative rake tooling, dull tooling, too small of a chipload, or too small of a DOC.
Cut it slowly, with a positive rake tool. Keep the chipload up (.004 minimum with an inserted cutter). Make sure the solid carbide tooling and HSS drills are sharp. Leave enough stock for a finish cut to take a decent chip - at least .005/side. When turning it, a common problem is the tool rubbing and causing work hardening in a semifinish cut or using a negative tool for roughing that leaves a work hardened surface behind.
Look for flank wear on the insert. If you see it, change the insert right away. If it is showing flank wear quickly, increase your chipload (as you would any time you see excessive flank wear).
If you keep the SFM down, the IPR/IPT up, and coolant in the cut, then it machines pretty well.

[Pondo]

Also, it's a good idea to rough everything in before finishing. It warps sometimes - a lot more than aluminum or most plastic does.

[Shane1234]

If you keep the SFM down, the IPR/IPT up, and coolant in the cut, then it machines pretty well.

I would say this is a general rule of thumb statement, but don't be afraid to try new stuff. I run my ss303 alot faster and dry if possible. 1/2" stubby variable 5 flute endmill at 1187 sfm (9000rpm), 100ipm, dry, .6" doc, .2" axial doc. With my 1.25" long 1/2" endmills, i run with coolant on a holder that shoots the coolant next to the flutes, same sfm & ipm, full doc, but axial I drop to .1".

[floman]

Thanks to everyone so far on all the information.
I will be starting these jobs in a few days and will apply what you guys have suggested and see what happens
If I have any issues I will post results here and see what suggestions you guys might have.

Our programmer has given me these speeds and feeds for the standard carbide cutters we use. All run with flood coolant at about 15%
All 4 flute except 1/16".
1/2" rpm 2400 F210mm/in
1/4" rpm 3800 F280mm/in
1/8" rpm 7500 F300mm/in
1/16" rpm 12000 F250mm/in

Sound good?

[Shane1234]

i would use a carbide that is coated with altain and only use square cornered endmills when finishing, use radius corners for hogging.

[floman]

Well after days of trouble we have finally got through one set of parts. Not knowing much about stainless we have had to run slow to get through the job. But i have just found out that the supplier set us 304 instead of 303. I have have a little about this but not much. How much difference ion maching is there between the two materials? Speeds and feeds slower? How about tapping M2x.4?
Thanks

[Shane1234]

i don't like 304 just because its so inconsistent. sometimes you feel like you ran into a chrome bumper.

as for your supplier sending you the wrong stuff, i would have contacted them about replacing it with the right stuff. 303 is easier to machine. heck, most of our suppliers will eat the cost of their mess up and send us the right stuff without taking back the wrong stuff.

[Mcgyver]

But i have just found out that the supplier set us 304 instead of 303. I have have a little about this but not much. How much difference ion maching is there between the two materials?

night and day imo, that is a brutal mistake of the supplier. 304 work hardens like crazy whereas 303 is a breeze - 303 is free cutting stainless, easy to machine.

[mflux_gamblej]

Did your client spec 303? Is it simply for ease of machining? 304 is more corrosion resistant and is high vacuum compatible - its a good material if you can cut it right and not have it warp on you when cutting or when heating (maybe in a cleaning step?) later.

To machine 304 you need to do some counter intuitive stuff... you need to feed the sh*t out of it at a low spindle speed. For example, I'll run a half inch 4 flute carbide endmill at 840 RPM, 0.040" depth, 9 ipm feed. You can increase the speed, then increase the feed proportionally if your cooling system can remove the heat so that you aren't making blue chips.

Your supplier owes you 303. 304 is the most common and cheapest stainless steel.