Another Stainless Cutting Question

[JMFabrications]

Ive have my CNC for about 6 months now, but I have only been machining aluminum. I am now in the need to make some custom exhaust flanges from 1/2" 304 SS. After searching around I found some baseline numbers, but so far I have managed to ruin 3 new 1/2" cobalt drill bits, and a $60 end mill within an hour.

Heres my setup:
Drilling 3 bolt holes, as well as 2 start holes, all holes are 1/2".
Using a 1/2" Cobalt Machine Length bit, no coating.
RPM=600
IPM=2
Peck Drilling .125"
Overall depth of each hole needs to be .70"
I originally started out by not peck drilling, but after switching it seemed to make the drill bit last a few more holes longer. Right now the bit will only last about 10 holes. Should I not be drilling such a larger diameter hole at once, maybe drill a 1/4" hole, then go back over it with the 1/2" drill? I also have a centerdrilling step in the program.

Next problem is the milling:
Contour slotting at a depth of .60"
Niagara Cutter 1/2" Cobalt Fine Pitch Roughing EM, TiCN Coated
RPM=1000
IPM=2
Flood Coolant
I was able to cut for a good 10 minutes and didnt notice any problems, then the EM just snapped. I cried for a bit after realizing how much that bit cost, then i got over it. Time to order some cheap EM's from ENCO to practice on.

Every feed/speed calculator ive used tends to give me different results. I use Mastercam for my parts, but their feeds arent always the best either. If anyone has some good info, or can recommend me some better Feeds/Speeds, I would greatly appreciate it.

Thanks,
Jim
JM Fabrications

[lakeside]

drill 290-390 rpm 3.5 imp .2 peck end mill spi Z-carb 4 flute 2500 rpm .1 deoth of cut 16imp

[Runner4404spd]

i just got done machining stainless tubes for a client. the one thing i found was that stainless hardens right near the cutter. you need to take a large enough cut to get through that and remove material. i was using HSS endmills and cobal drills on these tubes. also the other problem with machining 304 is that if your setup isn't very rigid you will have problems, by that i mean any backlash in the table and backlash in the spindle all has to be taken out to ensure a good cut.

[fpworks]

Jim,
Personally, I try to use only carbide tools for stainless. (although not required) I've just found that it ends up being less hassle in the long run and I get better performance while I'm at it.

For short run work with carbide tools, Garr tools have a great bang for the buck.

The first thing that I notice is that your feedrate for milling is too slow. I would start with 0.002 chip load, but you shouldn't have a problem with 0.003 chip load.

[mxtras]

To remind you which SS is which when quoting a job:
304 - she's a whore
303 - she's for me

Scott

[JMFabrications]

Thanks for all the help guys, I just realized I wrote the wrong material for the end mill, I am actually using a 1/2" TiCN Carbide End mill, not Cobalt. Its the ELITE series from Niagara......and I snapped it pretty quick. Luckily I bought 2, so im gonna give it another shot. Do you think I should do more then 1 pass instead of doing a single -.60" pass? Im gonna bump up the speed to about 6 IPM and maybe 1500 rpms.

FYI the chart for Carbide Niagara Cutters is here:
http://www.niagaracutter.com/solidca...edfeed.html#ss

[fpworks]

According to their chart, it looks like your feeds are correct. However, I didn't see any adjustment feeds for serrated (roughing) endmills, which you can take much higher chip loads and depth of cuts. You can be conservative, and go 0.3" deep with a 0.002 chip load. The low feed rate really bothers me in stainless. (work hardening)

FWIW, I have broken 12mm carbide roughing endmills trying to slot 15mm deep in H13 tool steel...the salesman swore it would work, so he was embarassed. I was going ~3000rpm and ~30 ipm. We changed it back to making the cut in two passes and it worked great.

Good luck!
Justin

[kalmah]

I think that coated carbide drill is the best. Of course the drill need to be conceived for drilling of austenitic stainless steel. IF you use internal coolant it's still better.

Here is the cutting parameter for diam 0.5" (without internal coolant)
n = 1600 RPM
Vf = 200mm/min
Pecking cycle = 0.25"

I'm not sure that the drill I use is sold in USA.

For milling, I prefer coated carbide end mill with fine chip breaker

[JMFabrications]

So I just bumped up the speed to 6 IPM and 1500 RPMS doing a .30" deep pass, and I burnt up the end mill pretty quick. No more practicing on the good end mills, i gotta get something cheaper till I figure this out. Someone suggested 4 IPM @ 800 rpms. Ill give that a shot.

[ajl6549]

If you start out at 30 - 40 sfm and .004 - .006 ipr for hss drilling and 100 - 200 sfm and .006 - .008 ipr for milling with coated carbide. you should be o.k.

P.S. thats about 267 rpm / 1.34 ipm for your drill and 1145 rpm / 5 ipm for your carb. e.m. depth of cut depends on your set-up but .1" to .2" is'nt out of the question. Remember stainless is tuff on tools regaurdless, so check tooling frequently.

[little bubba]

I'll throw in my two cents just for fun. First I almost puked when you said that you paid 60 bucks for a half inch cobalt endmill. Then you said that it was carbide, still a bit pricy. At 130 sfm, I would say you are right in the ballpark. Since you are concerned about the tooling cost, drop down to about 100 sfm and the endmill should last for quite a while. At 1000 rpms and 2ipm thats .0005 chipload, not enough in 304.

You said you are slotting, so your tool is buried, then I wouldn't go more than about .200 depth per pass.

As for the drill, in work hardening stainless, I've found that a split point will out perform a non split point by a huge amount. Also at 600 rpms or about 78sfm, thats a bit high, I would knock that down to 40 or 50sfm. Also, you really shouldn't need to peck until you hit about 2X diameter.

One more thing, just because its a pet peeve of mine, since you're new to the game, you're thinking RPMs and IPMs. Get out of that mindset, what you really need to know are Surface speed and chip load. If you communicate in SFM and chipload, nobody has to get out the calculator to figure out what is going on, and it will make your life easier in the longrun. Quick example, you find that 1000rpms and 5ipm works for you with this particular cutter. Next time you see this material you need to use a 3/4" cutter, you've got 1000rpms in your head, not going to work. If you have SFM in your head, 2 second calculation and done.

[kalmah]

Originally Posted by JMFabrications So I just bumped up the speed to 6 IPM and 1500 RPMS doing a .30" deep pass, and I burnt up the end mill pretty quick. No more practicing on the good end mills, i gotta get something cheaper till I figure this out. Someone suggested 4 IPM @ 800 rpms. Ill give that a shot.

It's very strange. Are you sure that it's carbide end mill.
I use fine pitch roughing end mill (carbide ). At 1700 RPM and 6 IPM with a depth of 1xD there is any problem.