Page 1 of 3 123 LastLast
Results 1 to 20 of 51
Like Tree6Likes

Thread: Trouble slotting 304!

  1. #1
    Matt@RFR is offline Stainless
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    1,062

    Default 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...

  2. #2
    dylskee's Avatar
    dylskee is offline Cast Iron
    Join Date
    May 2011
    Location
    Central MA USA
    Posts
    452

    Default

    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.

  3. #3
    Matt@RFR is offline Stainless
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    1,062

    Default

    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...

  4. #4
    ewlsey is online now Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    4,697

    Default

    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.

    G-Wizard says:

    170 SFM
    .0018"/tooth

    .08" max depth of cut

    It is saying to reduce your depth of cut.

  5. #5
    dylskee's Avatar
    dylskee is offline Cast Iron
    Join Date
    May 2011
    Location
    Central MA USA
    Posts
    452

    Default

    Quote Originally Posted by Matt@RFR View Post
    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...
    Oh crap, I over looked the fact you had to have them Monday! The only thing I could suggest at this point would be to beef up your coolant and take light depths of cut. Don't go too light on the feed, the last thing you want to do is sit on that material too long! Another thing you could do it drill a series of holes to rough out the slot, drills can be easily sharpened. Do you have any cobalt roughers? If so, you could use the rougher after drilling the holes and then go in with your finish cut.

  6. #6
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    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.

  7. #7
    Matt@RFR is offline Stainless
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    1,062

    Default

    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.
    Tell that to the 200 slots they made in 304. That's actually the reason I'm surprised I'm having trouble with these parts, and also why I suspect work hardening prior to me getting the parts. We'll see what the weekend holds.

    Thanks guys.

  8. #8
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    Quote Originally Posted by ewlsey View Post
    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.

    G-Wizard says:

    170 SFM
    .0018"/tooth

    .08" max depth of cut

    It is saying to reduce your depth of cut.
    Think you are wrong there, that might be what it says but its still wrong.

    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

    Chamfer.

  9. #9
    Matt@RFR is offline Stainless
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    1,062

    Default

    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?

  10. #10
    ewlsey is online now Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    4,697

    Default

    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.

  11. #11
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    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.

  12. #12
    dylskee's Avatar
    dylskee is offline Cast Iron
    Join Date
    May 2011
    Location
    Central MA USA
    Posts
    452

    Default

    Quote Originally Posted by cncbrit View Post
    I would lock those long carbide roughers away, you will just snap them.
    Really? Are you recommending not using carbide on 304 SS? Believe me I'm not the best machinist by a long shot but that's a ridiculous statement! HSS is like dial up internet, the only people who use it are CHEAP! Carbide roughers are awesome and eat through SS like butter and I have NEVER had a HSS tool that would compare, EVER! That's like saying using a wiffle ball bat in the majors would be better.

  13. #13
    gregormarwick is online now Stainless
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    1,541

    Default

    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 likes this.

  14. #14
    DMF_TomB is online now Titanium
    Join Date
    Dec 2008
    Location
    NY, USA
    Posts
    2,369

    Default stickout past collet

    Quote Originally Posted by Matt@RFR View Post
    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...
    what i get with my speed and feed calculator
    304 SS (machinability rating 0.35)
    diameter .375 and 4 flute, carbide
    coolant flood
    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
    Attached Thumbnails Attached Thumbnails clipboard02.jpg   clipboard01.jpg  
    Attached Files Attached Files

  15. #15
    jvangelder is offline Aluminum
    Join Date
    Aug 2010
    Location
    Southern NH, USA
    Posts
    176

    Default

    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

    -Jacob

  16. #16
    red beard's Avatar
    red beard is offline Aluminum
    Join Date
    Apr 2006
    Location
    Grand Rapids, MI USA
    Posts
    192

    Default

    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.

  17. #17
    Dualkit is online now Diamond
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    4,417

    Default

    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.

  18. #18
    Matt@RFR is offline Stainless
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    1,062

    Default

    Go back to your silly screw machines and let the men talk about mill work Bob.

  19. #19
    cncbrit is offline Hot Rolled
    Join Date
    Apr 2011
    Location
    California
    Posts
    518

    Default

    Quote Originally Posted by dylskee View Post
    Really? Are you recommending not using carbide on 304 SS? Believe me I'm not the best machinist by a long shot but that's a ridiculous statement! HSS is like dial up internet, the only people who use it are CHEAP! Carbide roughers are awesome and eat through SS like butter and I have NEVER had a HSS tool that would compare, EVER! That's like saying using a wiffle ball bat in the majors would be better.
    I am saying a 3/8 carbide rougher with a 1 3/4 LOC is just the wrong tool to go at 3/8 stainless sheet, 3/8 carbide rougher with 5/8 LOC that would be my first choice. 3/8 HSS rougher with a TiAl coating would be my second. Stainless is a tough material to cut, sometimes you need a cutter that can take a bit of abuse.

    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 likes this.

  20. #20
    CBlair is offline Diamond
    Join Date
    Sep 2002
    Location
    Lawrenceville GA USA
    Posts
    4,994

    Default

    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.

    Charles

Page 1 of 3 123 LastLast

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •