304L stainless speeds and feeds advice please. I had them very wrong.

[Jaxian]

I have in my limited time moving from manual to CNC machining done almost all aluminum. Some other stuff but nothing in the stainless steel realm.

So I got a job to make a base for a tool for the prototype shop at a large company. They wanted stainless. I checked the feeds and speeds and was a bit shocked at how low they were listed in my generic charts and even the defaults of G Wizard.

I then read the thread in here on the 4340 machining and knew I had done things very wrong and am hoping you guys can give me some direction.

I have another job coming up to make 12 plates for a lumber company for one of their saws. Like 12" x 12" x 1". They want them out of stainless. More stainless jobs now seem to be coming out of the woodwork so I need to get much better at it than I am now.

Here is the setup. Machine is a Doosan DNM5700 12k. Here is the material they gave me. Was told 304L, seems to match what it says on it. Flame cut but was told they had a new "process" that would keep the heat affected zone very small. Not really an issue as I squared it up on the manual mill as I didn't have time to learn how to MDI it on the CNC.

The raw material, 304L I believe:


Very basic shape. Some slotting, a recessed area, chamfered edges.

Finished product:


This took, using my feeds 2hr 15min. This is, based on what I have seen here, WAY too long.

Now the feeds and speeds, DOC, I used and SFPM:

Spot drill with 4 flute spot/chamfer 3/8" HSS
450 rpm, 44SFPM, .0012FPT, 2ipm feed (this broke the tip off)

Drill 31/64" (.4836), carbide, 550rpm, 69SFPM, 2ipm, 0036ipr (this seemed to work, full retract, .120 peck, long stringy chips that wrapped around the drill. Made squeaky noises.)

Endmill IMCO 67215 1/2" 4fl carbide (Slots), 1635rpm, 214SFPM, 5.5ipm, .0008ipt, .0033FPR .100 DOC, full width slot, conventional milling, finish pass full depth like .020 radial around the slot. (tried slotting at 11ipm to start, exploded my first endmill, got real conservative after that. This job was due the next day, no time for experimenting. This took 1 hour.)

Endmill 3/4" 3fl carbide (circle), 1177rpm, 224SFPM, 4ipm, .0011ipt, .0034FPR, helical in 2*, .250 DOC, 2D adaptive .2 optimal load, climb mill, stepdown was .4 max. (I don't see a stepover number in Fusion360. This took 18 mins to rough alone.)

Chamfer bit 1/2" 4fl carbide, 1200rpm, 157SFPM, 4ipm, .0017ipt, .0033FPR, like .050 on slots, .100 on circle, .150 on edge, used multiple passes on edge. (at 60" for all plus 4 passes on the edge this took 10, 4, 38 minutes respectively)

Got the job done. Second 1/2" endmill looks worn. Didn't break anything else so delivered the job. No way I can slack like this doing a dozen 1" plates. Any help would be appreciated.

Downloaded IMCO S&F chart, numbers come out MUCH higher than the ones I exploded the endmill on so a little leery of trusting them. I have almost no stainless to test on but I did find a few drops at the machinery place to mess with. I need to up my game a lot to get with the program. Thanks guys.

Paul B.

EDIT: Was running lots of flood coolant.

 

[JP Machining]

Tell them to shove that flame cut crap where the sun don't shine... Or atleast to cut it considerably oversize and then conventionally mill it so the teeth of endmill are more flaking it off rather than hammering it in. I prefer plate sawed on the large stainless I work on. Been hacking away on some 3" thick plates last few days and have some 6" and 4" to do yet.

Speeds and feeds, mfg charts are there for a reason. For general profiling I like Maritool variable flute endmills and his speed feed chart is pretty well spot on. For 1/2" 4fl I'm running 1" doc .030" radial step at 3000 rpm and 30 ipm. Can run same specs but maybe .700" depth and .020" radial on a necked version hanging out 3" overall from collet face. Coolant is a must on stainless, in steel some times is better dry but stainless use coolant.

 

[Mydrrin]

The biggest thing about 316/304 stainless is heat removal. Then chip removal. Heat makes it hard and busts tools. Request it water jet cut. Make sure you have coolant and more coolant; through coolant is best. I usually go slower speed higher feed.

 

[litlerob1]

Goodness, a couple things to point out. Your chip load is way too low on MOST stuff. The SFM is changing from Carbide tool to Carbide tool, it shouldn't really,(depending on coatings).

If it were me, I would run 200 SFM on all the Carbide tools, I would not run HSS if your goal is to get faster.

Spot with a "Spot Drill" not a Chamfer Mill, if HSS under 50 SFM only deep enough to be effective.
Drill 200 SFM, .005-.0075" per rev. chip load.
1/2" Endmill 200 SFM, .003 per flute chip load. (this one shook you up, because it broke, it broke because you are rubbing instead of cutting)
3/4" Endmill 200 SFM, .0035 per flute chip load. (your time on this one seems decent, but a little slow)
1/2" Chamfer Mill 200 SFM .0125" per flute chip load while Roughing, .002" for Finishing. (same depth parameters)(Roughing should sound like a Buzz)

The general problem is too low on the feed, you can't give the cutter a chance to rub 304L, it needs to cut.

R

 

[adamm]

Goodness, a couple things to point out. Your chip load is way too low on MOST stuff. The SFM is changing from Carbide tool to Carbide tool, it shouldn't really,(depending on coatings).

If it were me, I would run 200 SFM on all the Carbide tools, I would not run HSS if your goal is to get faster.

Spot with a "Spot Drill" not a Chamfer Mill, if HSS under 50 SFM only deep enough to be effective.
Drill 200 SFM, .005-.0075" per rev. chip load.
1/2" Endmill 200 SFM, .003 per flute chip load. (this one shook you up, because it broke, it broke because you are rubbing instead of cutting)
3/4" Endmill 200 SFM, .0035 per flute chip load. (your time on this one seems decent, but a little slow)
1/2" Chamfer Mill 200 SFM .0125" per flute chip load while Roughing, .002" for Finishing. (same depth parameters)(Roughing should sound like a Buzz)

The general problem is too low on the feed, you can't give the cutter a chance to rub 304L, it needs to cut.

R

The numbers in the OP aren't rubbing. When I have time, I run a 4 flt 0.5" 0.030CR TiAlN coated carbide endmills at 0.001/flute chip load, and they last forever cutting 304 stainless. If I hit feed hold in the middle of a cut, THEN it rubs, and that is the end of the end mill (like when I think I'm going to hit a hold down clamp, etc). If I dial up the feed to 0.002 or 0.003/flute as the literature for the endmill says, it will run that way, but not last nearly as long. I think the fear of "rubbing" that is posted here frequently is vastly over stated. On a CNC machine with the cut programmed to move continuously, it probably isn't rubbing.

 

[litlerob1]

The numbers in the OP aren't rubbing. When I have time, I run a 4 flt 0.5" 0.030CR TiAlN coated carbide endmills at 0.001/flute chip load, and they last forever cutting 304 stainless. If I hit feed hold in the middle of a cut, THEN it rubs, and that is the end of the end mill (like when I think I'm going to hit a hold down clamp, etc). If I dial up the feed to 0.002 or 0.003/flute as the literature for the endmill says, it will run that way, but not last nearly as long. I think the fear of "rubbing" that is posted here frequently is vastly over stated. On a CNC machine with the cut programmed to move continuously, it probably isn't rubbing.

This is true in theory, meaning if it's cutting it's cutting right? The exception is that 304 will get hot in front of the cutter. There isn't really another explanation as to why the 1/2" Endmill broke.

While cutting 304 the chipload is more important than anything, so long as teh spindle speed isn't outrageous. So if the spindle is running so slow that it will not heat up the material than .001" is fine. For getting the job done faster, it is NOT.

 

[Jaxian]

Ok, so let me see if I have this through my thick head before I go and test . It would seem that my SFPM is not too bad, the IMCO chart says you can push around 300SFPM so I am not too far out at 225SFPM.

Now you guys said the IPT is low, the IMCO chart says .0025-.0035, so as you noted it would appear I am WAY off with the .0008 - .0011 for the end mills. The IMCO numbers do seem pretty close to the Maritool charts too so they seem like solid numbers.

So the consensus would be that rpm is probably OK but kick up the feed until I hit that IPT number? Not drop rpm and leave feed alone to get there. I really want to get the cycle time lower so would lean toward faster feeds. That exploded endmill just caught me off guard. After all the aluminum I had forgotten you needed to really pay attention to this stuff, I just run everything as fast as I feel comfortable.

I put the numbers in to G Wizard for the 1/2" IMCO carbide as you guys said and at 250SFPM, it says 1910rpm and 12.606ipm with a .0033ipt. This would get me done in a third the time. As an aside with those numbers it also says .0066IPR, 2.4752MRR, and 3.71hp used. If those sound like good numbers I will go run them and see how things work.

I have a Maritool order arriving tomorrow but should have more than enough time to order up some roughers before that job shows to test the S&F's. Might try 3/4" or even 1" for peripheral roughing. My machine is pretty stout for a generic VMC and I have a lot of extra tool holders.

Thanks for helping me with this guys.

Paul B.

 

[litlerob1]

Sounds good.

Make sure you aren't re-cutting chips. Because 304 is so unpredictable, I would run 200 SFM, and not above, but that's on you. I have run 300 in a heat-next day didn't work sooo?

Cutting burnt chips will kill you and the cutter fast.

R

 

[Jaxian]

Cutting burnt chips will kill you and the cutter fast.

R

I am wondering if that wasn't the cause of the catastrophic failure of the first endmill. If you look at my photo of the part in the first post it might have been my setup.

The part was clamped in a vise along the long edge with the slot parallel to the vise jaw. Standing facing the part the cut was conventional milling the lower slot from left to right. Problem is that on a Doosan all the flood nozzles are on the right side of the spindle.

The endmill died at the .700 level depth cut at about the 8" mark, or basically where it was at a point that no coolant could get down into the bottom of that slot in front of the endmill for cooling or chip clearing.

Going to have to pay more attention to the features and coolant nozzle positions. They are like 3 fire hoses so I just assumed it got everywhere. But what you say seems to explain it. I hope that's right and I can turn up the wick.

Awesome, thanks for all the help !!

Paul B.

 

[Rstewart]

Make sure you drill the ends of the slot just off the finish profile. This will take some of the load off your endmill in the corners.

If you have some good carbide drills I might even rough drill the whole thing and just finish profile.

 

[adamm]

This is true in theory, meaning if it's cutting it's cutting right? The exception is that 304 will get hot in front of the cutter. There isn't really another explanation as to why the 1/2" Endmill broke.

While cutting 304 the chipload is more important than anything, so long as teh spindle speed isn't outrageous. So if the spindle is running so slow that it will not heat up the material than .001" is fine. For getting the job done faster, it is NOT.

I run at 196 sfm, so not far from your numbers. If the coolant stays on it, no problem. I also run deeper DOC, somewhere around 0.25 to 0.30 deep, so maybe I'm just trading feed for DOC?

I am wondering if that wasn't the cause of the catastrophic failure of the first endmill. If you look at my photo of the part in the first post it might have been my setup.

The part was clamped in a vise along the long edge with the slot parallel to the vise jaw. Standing facing the part the cut was conventional milling the lower slot from left to right. Problem is that on a Doosan all the flood nozzles are on the right side of the spindle.

The endmill died at the .700 level depth cut at about the 8" mark, or basically where it was at a point that no coolant could get down into the bottom of that slot in front of the endmill for cooling or chip clearing.

Going to have to pay more attention to the features and coolant nozzle positions. They are like 3 fire hoses so I just assumed it got everywhere. But what you say seems to explain it. I hope that's right and I can turn up the wick.

Awesome, thanks for all the help !!

Paul B.

My mill also has all the nozzles on the right hand side. I had to pipe a nozzle over to the left side to get enough coolant coverage to keep the end mills happy in stainless. My experience is that any interruption to the coolant that allows heat to build is the end of the endmill. As soon as the chips get orange in the cut, or the washed away chips are blue, that's about the end.

 

[guest]

I've got a kennametal 3/4" indexable that would make short work of that center circle, might consider indexables for that and the chamfer if you have them. Cheaper to run than solid carbide end mills and you can push them harder.

 

[Finegrain]

Coolant is a must on stainless, in steel some times is better dry but stainless use coolant.

Don't be so sure! HSM parameters with no coolant worked well for me on my last 304 job -- 3/8" 4-flute EM, 500 SFM (5000 RPM), 80 IPM, .025" stepover, 0.6" axial DOC.

Regards.

Mike

 

[Mtndew]

Goodness, a couple things to point out. Your chip load is way too low on MOST stuff. The SFM is changing from Carbide tool to Carbide tool, it shouldn't really,(depending on coatings).

If it were me, I would run 200 SFM on all the Carbide tools, I would not run HSS if your goal is to get faster.

Spot with a "Spot Drill" not a Chamfer Mill, if HSS under 50 SFM only deep enough to be effective.
Drill 200 SFM, .005-.0075" per rev. chip load.
1/2" Endmill 200 SFM, .003 per flute chip load. (this one shook you up, because it broke, it broke because you are rubbing instead of cutting)
3/4" Endmill 200 SFM, .0035 per flute chip load. (your time on this one seems decent, but a little slow)
1/2" Chamfer Mill 200 SFM .0125" per flute chip load while Roughing, .002" for Finishing. (same depth parameters)(Roughing should sound like a Buzz)

The general problem is too low on the feed, you can't give the cutter a chance to rub 304L, it needs to cut.

R

I was thinking the same thing.
304 likes a good moderate feedrate, don't be afraid to feed a little faster than your'e used to.

 

[DMF_TomB]

I have in my limited time moving from manual to CNC machining done almost all aluminum. Some other stuff but nothing in the stainless steel realm.

So I got a job to make a base for a tool for the prototype shop at a large company. They wanted stainless. I checked the feeds and speeds and was a bit shocked at how low they were listed in my generic charts and even the defaults of G Wizard.

I then read the thread in here on the 4340 machining and knew I had done things very wrong and am hoping you guys can give me some direction.

I have another job coming up to make 12 plates for a lumber company for one of their saws. Like 12" x 12" x 1". They want them out of stainless. More stainless jobs now seem to be coming out of the woodwork so I need to get much better at it than I am now.

Here is the setup. Machine is a Doosan DNM5700 12k. Here is the material they gave me. Was told 304L, seems to match what it says on it. Flame cut but was told they had a new "process" that would keep the heat affected zone very small. Not really an issue as I squared it up on the manual mill as I didn't have time to learn how to MDI it on the CNC.

The raw material, 304L I believe:
View attachment 222860

Very basic shape. Some slotting, a recessed area, chamfered edges.

Finished product:
View attachment 222861

This took, using my feeds 2hr 15min. This is, based on what I have seen here, WAY too long.

Now the feeds and speeds, DOC, I used and SFPM:

Spot drill with 4 flute spot/chamfer 3/8" HSS
450 rpm, 44SFPM, .0012FPT, 2ipm feed (this broke the tip off)

Drill 31/64" (.4836), carbide, 550rpm, 69SFPM, 2ipm, 0036ipr (this seemed to work, full retract, .120 peck, long stringy chips that wrapped around the drill. Made squeaky noises.)

Endmill IMCO 67215 1/2" 4fl carbide (Slots), 1635rpm, 214SFPM, 5.5ipm, .0008ipt, .0033FPR .100 DOC, full width slot, conventional milling, finish pass full depth like .020 radial around the slot. (tried slotting at 11ipm to start, exploded my first endmill, got real conservative after that. This job was due the next day, no time for experimenting. This took 1 hour.)

Endmill 3/4" 3fl carbide (circle), 1177rpm, 224SFPM, 4ipm, .0011ipt, .0034FPR, helical in 2*, .250 DOC, 2D adaptive .2 optimal load, climb mill, stepdown was .4 max. (I don't see a stepover number in Fusion360. This took 18 mins to rough alone.)

Chamfer bit 1/2" 4fl carbide, 1200rpm, 157SFPM, 4ipm, .0017ipt, .0033FPR, like .050 on slots, .100 on circle, .150 on edge, used multiple passes on edge. (at 60" for all plus 4 passes on the edge this took 10, 4, 38 minutes respectively)

Got the job done. Second 1/2" endmill looks worn. Didn't break anything else so delivered the job. No way I can slack like this doing a dozen 1" plates. Any help would be appreciated.

Downloaded IMCO S&F chart, numbers come out MUCH higher than the ones I exploded the endmill on so a little leery of trusting them. I have almost no stainless to test on but I did find a few drops at the machinery place to mess with. I need to up my game a lot to get with the program. Thanks guys.

Paul B.

EDIT: Was running lots of flood coolant.

.
reduce settings like depth and width of cut and sfpm keeping ipt near recommended range and use coolant to avoid recutting chips your end mill will tell you more than any book, chart or computer program
.
i laugh cause a expert opinion i had a end mill once get yellow hot and melt throwing sparks in less than 3 minutes once listening to opinions. you are the one at the machine. look, listen etc
.
often you can get settings to work 80% and only scrap parts 20% of the time. if zero scrap rate is important you have to be more careful

 

[Matt@RFR]

Don't be so sure! HSM parameters with no coolant worked well for me on my last 304 job -- 3/8" 4-flute EM, 500 SFM (5000 RPM), 80 IPM, .025" stepover, 0.6" axial DOC.

Mike, normally I would be with you, but we just got done with a nightmare job in 304 that should have been a very easy part. We kept backing everything down until we got any tool life at all, ended up having to go from HSM to an indexable at 150SFM, and tool life was still miserable. I was running OSG list 1100 drills (supposed to be the best stainless drill other than coolant thru), suggested starting point is 50SFM, we ended up at 10SFM. The job took triple the time it should have and with all the tooling we burnt through, I think I paid $800+ for the privilege of making those parts.

This was our first job for that customer, and you could tell he figured we just didn't know what the hell we were doing. But a few days later he brought in one of our parts and another part he was getting from another shop, both had been bead blasted. The first part looked as you would expect, and our part just looked polished. Even bead blasting wouldn't touch the 304 from this run.

My Western Tool rep, along with a couple of their tooling reps, are all saying that this is becoming more and more common for some reason.

 

[DMF_TomB]

dont expect over 60 minutes tool life with 304. it aint like aluminum where tools last over 200 to 1000 minutes

 

[DMF_TomB]

some 304 has big hard spots or slag in it. you hit a big hard spot tool is gone in less than 1 second. quite common when cutting going good and bam suddenly you got sudden tool failure often all over in less than 2 seconds

 

[cyanidekid]

Tom and Matt beat me to it, yes, "304" is a vague general description of a wide range of possible alloys. what is sold as 304 is all over the map in terms of machinability.

also, if the foundry isn't extremely careful in processing the scrap that goes into the melt, it is likely to include a lot of carbide inclusions (chromium carbide), and other possible junk.

I just drilled some "304" that my customer had supplied (from McMaster) with 60 .125 holes, and it was horrible, everything going fine, one bit lasts 20 holes, next one, with no change in speeds and feeds, sparks on the second hole, and dead. It was from india.

 

[DMF_TomB]

Tom and Matt beat me to it, yes, "304" is a vague general description of a wide range of possible alloys. what is sold as 304 is all over the map in terms of machinability.

also, if the foundry isn't extremely careful in processing the scrap that goes into the melt, it is likely to include a lot of carbide inclusions (chromium carbide), and other possible junk.

I just drilled some "304" that my customer had supplied (from McMaster) with 60 .125 holes, and it was horrible, everything going fine, one bit lasts 20 holes, next one, with no change in speeds and feeds, sparks on the second hole, and dead. It was from india.

.
.
when a apprentice i thought talk of hard spots was excuse or made up .....after you hit hundreds if not thousands of hard spots over the decades you realize it aint a made up thing