Facing 304 stainless

crgvettez · Aug 30, 2014

I am having a very hard time with feeds and speeds on facing 304 stainless.......my stock is 2.25x3 and I'm facing it down from .187 to .135 I have tried several combinations but no luck thus far.....I am using a 2.5 Mitsubishi face mill with 5 indexable inserts. I also have the ability to run flood coolant or airblast..... Any help would be greatly appreciated.....thanks most of my exp is with 4140 1018 and 6061 alum..... Never 304ss and thus far I am not a fan and the machine is cat 40 haas vf2

Jorgo · Aug 31, 2014

What does Mitsubishi recommend? I use a sandvic 245 facemill on our vf2 in 304. I don't remember exactly what speed and feed I use but it's something like 800sfpm and .009 chip load. Seems way to fast but it works good with good tool life. Definitely use lots of rich coolant. You definitely need full contact under your part ideally vacuum I think to fight vibration.
Jordy

DMF_TomB · Aug 31, 2014

parameters

crgvettez said:
I am having a very hard time with feeds and speeds on facing 304 stainless.......my stock is 2.25x3 and I'm facing it down from .187 to .135 I have tried several combinations but no luck thus far.....I am using a 2.5 Mitsubishi face mill with 5 indexable inserts. I also have the ability to run flood coolant or airblast..... Any help would be greatly appreciated.....thanks most of my exp is with 4140 1018 and 6061 alum..... Never 304ss and thus far I am not a fan and the machine is cat 40 haas vf2

.
you would have to give more information on speeds and feeds you are using. sometime though part vibration can destroy inserts. what tool life time are we talking about. 10 min, 60 minutes?, etc
.
what works on thick metal may not work as well on thinner metal

Atomkinder · Aug 31, 2014

304 sucks, plain and simple. However, telling us what your surface footage and chipload are currently will help a lot for determining how to change your process. Also workholding, how your inserts are failing, etc. Personally I'd be tempted to pick up a 3/4" stub .03" radius solid carbide AlTiN-coated end mill for that part if the inserts aren't cutting it (har).

I believe work hardening is your biggest enemy here, but without knowing more about your process it's hard to judge what's happening.

Krovvax · Aug 31, 2014

I had a similar job not so long ago. Tried alot of thing but was not able to get more than 10 part before the corner fail. Choose to not listen to the mfg recommendation and turn the coolant off and tool life jump from 10 to 35 part per corner. Might worth it to try.

crgvettez · Aug 31, 2014

It's only a 21pc and I'd really like to run them all without turning my inserts I started setting the job up on Friday and got one pc ran just wasn't happy with the finish or how the cutter sounded..... I'm doing a lot more than just facing but with all the other tools I'm using the Harvey catalog for the feeds and speeds on all the other tools and they seem to be cutting great.... The face mill is a 2.5 mitsubishi NSE cutter but from looking in the online catalog I can't even find the cutter..... It is an excellent finisher on all other matls that I've worked with but I don't think mitsubishi makes it anymore so I can't find feeds and speeds for it on stainless the last one I tried was 900 sfm with .0025 chip load...... And I did a finish pass and flooded with coolant but it seemed to be makin a lot of heat there was a lot of smoke comin off of it but no discoloration but it didn't feel too smooth either and I am honesty clueless with stainless idk if I need to feed harder or back off or take deeper cuts or what...... I only have .05 total to take off but I can't keep doing trial and error just hope someone could point me in right direction and give me a good starting point

CBlair · Aug 31, 2014

When in doubt slow it down, your RPM that is, I would run far more conservative esp as you only have a few pieces to do. I am not familiar with your insert so it is hard to say whether the geometry is a good fit for ss. I use a nice positive rake insert at slow speeds and have always had good luck with a finish pass of 0.01-0.02 DOC.

My actual s/f wouldnt be useful to you as I dont know what kind of insert you have.

Charles

Krovvax · Sep 1, 2014

I dont know what your cutter geometry is and what kind of insert it use but with my sumitomo 2.5 inch 45° cutter im usually running 1000 rpm 0.005 chip per thooth and i would take the 0.050 one pass. I did some roughing with this cutter last friday was taking 0.1875 doc with the same parameter and insert last for ever.

Stainless like to be feed hard if you rub it its going to make alot of heat and going to destroy your insert in no time.

Red James · Sep 1, 2014

I tried to follow mfg suggested speed / feeds on an 8 x 22" piece of 5/8 304 plate. Even called tech support. All I could do was burn corners off inserts. Finally went old school and turned sfm down to 250 and feed to 0.01 per tooth . . . finished four parts and did not roll inserts again.

DMF_TomB · Sep 1, 2014

304

Red James said:
I tried to follow mfg suggested speed / feeds on an 8 x 22" piece of 5/8 304 plate. Even called tech support. All I could do was burn corners off inserts. Finally went old school and turned sfm down to 250 and feed to 0.01 per tooth . . . finished four parts and did not roll inserts again.

.
304 can vary a lot depending on how worked hardened it is from rolling when made. it also can be abrasive so i would expect shorter life than 1018 steel
.
i usually start at 600 sfpm and yes sometimes slowing down helps especially if getting part vibration. also max sfpm depends on depth and width of cut. if deep slotting at full width of cutter it is hard on any mill. i find if loosing insert corners in large pieces breaking off to ease up on feed and depth of cut. some inserts have problems over .006 ipt feed
.
wanting to machine faster and get good tool life and good finish........well it is nice to want things, most rarely get everything they want

Larry Dickman · Sep 1, 2014

we had a production run of 304 parts a while back. We had them double disc ground to thickness.

FOXFIRE · Sep 1, 2014

Don't worry, when you get it dialed in the next batch will be different. I hate 304.

brian.pallas · Sep 2, 2014

If all you've been cutting is steel and aluminum, did you buy a different grade of insert for the SS? What works well in steel or aluminum is not the best for stainless. For our facemills we keep 4 different grades in stock for the different amterials we work with.

Mtndew · Sep 2, 2014

304 can be a beeyoch.. if you let it.
Stable workholding and stable cutters are the first place to start.
As said above, don't that the cutter rub, or it will most likely be toast.
If at all possible.. see if you can use 303 SS for the job.

RevetsP · Sep 6, 2014

For me, with thin stuff like that, I would try to use a smaller hi-feed cutter 16 or 25mm (Ingersoll makes some nice small 90deg insert cutters that you can use either 90deg inserts or hi-feed inserts which really came in handy for me (SERIES 12J1D)) and keep the thing engaged in the material and ramp for depth. Then finish with with your favorite DOC and IPT. If I remember right for milling we ended up keeping the DOC about 70% of the radius and used the low end of the recommended IPT for the inserts. Very rich coolant is a huge plus! Keep the thermal shock to a min.

When machining stainless it was tricky maintaining the balance between feed and depth of cut. Not enough feed and the finish gets rough and tool life is unpredictable, too deep or not deep enough give the same issues. I'm sure everyone here has heard that before though... haha

snowshooze · Sep 6, 2014

Low speeds, high feeds and diesel for cutting fluid.
The faster your surface feet, the worser it gets. The stuff seems to harden ----- during---- the cut. Rule of thumb for 304.
Run slow and crowd. You will be surprised.
Good luck.

jjxtrider · Sep 2, 2018

304 and 316L is 90% of what I've been machining for 15 years now , it sucks plain and simple . I've had parts that I find a certain cutter ,insert , speed and feed that work the best and 2 months later the same parts only a different batch of bar stock and the whole setup changes. One thing that just kills corners is interrupted cuts or as the facemill just starts hitting the part and as it leaves the part . The newer HSM toolpaths help where the cutter enters at an angle and a steady increase in depth of cut . For a 2.5" wide part I'd prefer a 2.625" wide cutter but the std 3" will have to work ,but it's best to have the cutter barely wider than the part , just can't happen all the time.

Sfpm's I use are generally in the middle , high speed works sometimes but often burns up corners faster than slower speeds . So much depends on cutter(90,45,15 deg lead-in), insert shape /grade?cr , work piece rigidity , mill rigidity , high pressure coolant flood or air . Burying the cr at least 70% is best for surface finish and chip control to help the insert last .

.

precisionmetal · Sep 3, 2018

Nobody has mentioned it here (and I'm not happy to say this), but part of the "battle" will be that you're on a VF2. I have a SuperMiniMill, and recently had a fairly large (for me) 304 part to make. Around 10" diameter and 2.5" thick, with a lot of material to be removed. I ended up making some *very* rigid tooling that bolted directly to the table, and the part was bolted to it with a slew of 3/8" bolts. TiAlN rougher end mill, with very low rpm and a quite substantial feed rate is what ended up being "somewhat acceptable".

I realize the above does not directly solve your issue, however points being -- hold the part any way possible to make it rock solid, and drop the SFPM and increase the feed rate. On a Haas, the machine will definitely "complain" if you push the feed too much, but I think you may end up with more feed per tooth than you might expect.

As someone else mentioned, you might consider removing most of the material with a stub (coated) end mill, then just push that face mill across with low revs and a pretty high feed rate for your finish pass.

JMHO

PM

Larry Dickman · Sep 3, 2018

Poor bastards been waiting 4-1/2 yrs now to make this cut.

precisionmetal · Sep 3, 2018

LOL..... thanks Larry.

I >>> :nutter:

should pay more attention!

Facing 304 stainless

Plastic

Hot Rolled

Diamond

Titanium

Hot Rolled

Plastic

Diamond

Hot Rolled

Stainless

Diamond

Titanium

Aluminum

Hot Rolled

Diamond

Cast Iron

Stainless

Aluminum

Stainless

Titanium

Stainless

Similar threads