Results 1 to 20 of 51
Thread: Trouble slotting 304!
08-12-2011, 11:32 AM #1
Trouble slotting 304!
I'm working on half-done 304 parts for another machine shop due to them having some machinery problems at the moment. All I have to do on these is rough and finish a profile and chamfer.
The tool is an MA Ford 3/8" 4 flute with Altima coating, 7/8" LOC, .015" radius corners, hanging about 1.3" out of an ER-25 collet. Runout is .0006". The big extension is necessary to clear fixture clamp bolts. The 3/8" diameter is necessary because the fixture won't hold up to a 1/2" or larger endmill at any reasonable chip load.
The parts are .360" thick and I'm going around them at about .130" step downs, anywhere between 5% stepover and full slot due to the shape of the parts. 220 SFM and .002" IPT. Pretty much in the middle of MA Ford's recommendation. LOTS of coolant right at the cut.
The parts are made from 304 sheared flat bar, and I have some concerns whether the material is already work hardened from shearing. Any comments on that?
The parts have been faced on four sides. I'm wondering if the other shop work hardened these while facing, but wouldn't they have had tooling issues from that?
The cut sounds good, spindle load is very consistent right up until the endmill suddenly gets all the corners knocked off of it. So how would you guys go about cutting possibly work hardened 304? I'm not sure that's the problem, but it's definetely an unknown factor. 180 SFM? Lower? The last endmill ran 4 parts...roughly 96" of cutting at the above step downs. No chatter is evident.
I have 55 parts to go and 3 roughing endmills left. The parts need to ship on Monday...
08-12-2011, 11:56 AM #2
Man I feel your pain! I had a job a while back with the same circumstances, it was 304 SS plate (Bar stock was 4 times the price!) but they were 3-1/2" square and I had to face mill all sides about an 1/8", drill and tap a bunch of holes from all sides and it was a nightmare! And you're absolutely right about work hardening, it's very easy to do with that crap. We sent the blocks out after I milled them square and had them solution annealed and that seemed to help but it still wasn't fun. If you can switch the machine to some kind of cutting oil that would help but if you can't run your coolant real strong. I would strongly recommend a carbide roughing end mill and then a finish mill with light cuts, you should be able to get through it with one rougher and finish but at worse case scenario you would need two roughers but they are priced reasonably well. Good luck and keep us informed of your results and methods.
08-12-2011, 12:04 PM #3
The only carbide roughers I have, have a ridiculously long LOC (3/8 x 1.75). There's just no way I'm going to get anything else over the weekend. Maybe I'll try those once I break all my other endmills...
08-12-2011, 12:10 PM #4
I have G-wizard software. I find that the feeds and speeds are not really all that important (or correct), but the deflection calculations are great when you are breaking end mills.
.08" max depth of cut
It is saying to reduce your depth of cut.
08-12-2011, 12:12 PM #5
08-12-2011, 12:54 PM #6
Plunge cut the slotted part with a carbide EM, .1" step over, will be better than taking lots of .08" passes. HSS roughers work best with high depths of cut.
Work hardened 304 cuts better with carbide.
I would lock those long carbide roughers away, you will just snap them.
08-12-2011, 01:05 PM #7
Ok, 4 passes is .090" DOC, so I'll try that in the morning. If that goes well I'll try to go up to, say, .0025" IPT and try and make some time back up. I could actually take .080-.090 passes in the full slot area only, then go back to my .130 DOC (or more) on the much lighter areas.
Coolant is at 12% already.
I would lock those long carbide roughers away, you will just snap them.
08-12-2011, 01:07 PM #8
Stainless is a nasty material to cut, if you are going to make the bottom 0.08" of the cutter do all the work, this is also the most fragile part of the cutter, the cutters won't last.
You need to do something like this.
Profile the OD in several light cuts at 1/2 depth of cut, this uses lots of the cutter and gives the guys at the end a break.
Plunge mill the slot, again 1/2 deep, actually I would do the first one 5/8 deep, subsequent ones at 1/2 deep, this make sure your not jamming the cutter into chips.
Finish profile the part at 7/16 deep
08-12-2011, 01:26 PM #9
The only plunge roughing I've done was in aluminum with an inserted endmill. Can you give me an idea of where to start with feeds/speeds with my 3/8" endmill?
Also, the part is .360" thick, so your depths aren't making sense. Were you thinking it was 1/2" thick?
08-12-2011, 01:32 PM #10
What is 1/2 depth of cut? 5/8? 7/16?
Did you read the OP's first post?
The parts are only .36" thick. Good luck saving time plunge milling with a .1 step on a 24" perimeter.
08-12-2011, 02:06 PM #11
Depths are for a 0.360 part, I an assuming you have them bolted to a sub plate type fixture.
You want the tip of the cutter past the bottom of the material. The tip of the cutter is fragile, and heats up quick. Thin sections of stainless heat up quick too.
Speeds and feeds I do not have. I was doing a part the conventional way and switched to plunging the slots, I remember being really happy with the tool life and time savings.
I am suggesting profiling the OD and only plunge milling the slots, or corners.
I also remember getting the darn parts waterjet cut to +0.1, was real happy with myself for that too.
08-12-2011, 02:56 PM #12
08-12-2011, 05:50 PM #13
I don't know if you're using cam software, it will be easier if you are, but you really should be running full depth/light stepover on a part like that, possibly with trochoidal in the area where it's full slotting. The material is too thin to cut it in small steps.
cncbrit liked this post
08-12-2011, 07:48 PM #14
stickout past collet
304 SS (machinability rating 0.35)
diameter .375 and 4 flute, carbide
type of cutting partial and full width up to slot cutting
stickout from collet 1.3"
at 210 sfpm thats 2139 rpm at 50% Feed thats 19.8 ipm
giving chip thickness 0.0023
100% max depth of cuts recommened
DOC 0.014" at 1.3" stickout from collet
DOC 0.023" at 1.0" stickout from collet
DOC 0.047" at 0.7" stickout from collet
in my opinion your DOC is too high for the length sticking out and your brittle carbide end mill is vibrating and chipping and loosing cutting edges
08-12-2011, 10:44 PM #15
earlier this year we did a fab job that had maby 1200 .370 wide slots full depth though 5/16 thick 304. We ran aprox 230sfm full depth 0.001ipt lots of flood coolant. Had very good luck. was a 5/16 iscar chatter free
Another portion of the job had a full width slot parting off sections of scrap from the above pieces to make gussets which we ran again at 230sfm but with .5 iscar chatter free mill. Made 752pc and i belive i only went though two mills
08-12-2011, 11:42 PM #16
If you're loosing the corners the stainless may be sticking to the end mill. You could try upping the coolant concentration to give it more lubrication.
08-13-2011, 05:02 AM #17
What does a person do that is being falsely accused of work hardening parts? I am the customer. I found out my wimpy Mycenter Zero wasn't really up to 304, that and cutter comp is an issue with the Yasnac controller. I was making a career out of this job.
08-13-2011, 05:04 AM #18
Go back to your silly screw machines and let the men talk about mill work Bob.
08-13-2011, 06:10 AM #19
Aluminum you can slap around, Steel you punch, Stainless you got to go at knees and elbows, try slapping it and you will break your fingers.
dylskee liked this post
08-13-2011, 06:17 AM #20
I have found through experience that HSS cutting tools can be very helpful in 304ss. I especially like to use the HSS roughers when cutting ss that has been burnt out with a plasma cutter. These tools are slow but they take the abuse of that cut edge like nothing else will.
Of course properly used the carbide tools will process faster but I have found they are more prone to edge chipping and can be harder to dial in. In the end you use the tools at hand that work the best for your job.
I hope the job is going better for you Matt, I have been in your shoes before. Some pretty good advice been givin so far, I hope it works out.