Results 1 to 8 of 8
  1. #1
    So CA Machinist is offline Aluminum
    Join Date
    Jun 2008
    Location
    Covina, CA USA
    Posts
    56

    Default milling 1018 steel

    Hey guys:

    I've got a little problem. I'm trying to get the most life out of my 5/8" insert cutter (Mil-Tec). I'm using the largest radius they offer. I'm pocketing 1018 steel. (.194" deep). I've tried running dry, coolant, but it's not directly on the inserts. I was cutting .0625" depths at 8500 rpm & 105 ipm.

    I'm down to 7500 rpm .045" depths and 90 ipm.

    I'm helical plunging at 12 ipm. If I run it dry after maybe 6 or 7 parts, i'll get a spark show during the helical plunge. I can't run more than maybe 19 parts total. This is a piece of steel that is 6" long x 2.75" wide.

    Do I take .025" depths of cut? They won't let me order inserts. I got this tool for free. I have to wait until monday for the rep. I'll hook him up on some items here for some tooling. I'm using the recommended grade insert for the material.

    Any and all info is greatly appreciated.

    Thanks,

    Ron - Ontario, CA

  2. #2
    g-coder05's Avatar
    g-coder05 is offline Stainless
    Join Date
    Mar 2006
    Location
    Zhongshan China
    Posts
    1,732

    Default

    You didnt say how many inserts in the tool so i cant figure the chip load. your best bet is to machine the part going full depth since this minimizes how many times your corners see action basicly more passes equal more linear feet your cutter has to travel. Have you considered a variable helix carbide mill? Im seing around 1000 liniear feet before my 1/2" varimills give out at 4200 rpm 39" per min.

  3. #3
    So CA Machinist is offline Aluminum
    Join Date
    Jun 2008
    Location
    Covina, CA USA
    Posts
    56

    Default

    I'm sorry...it's a 2 flute insert cutter.

    Ron

  4. #4
    Perry Harrington is offline Titanium
    Join Date
    Oct 2006
    Location
    Boulder Creek, CA
    Posts
    2,349

    Default

    You didn't mention the size of the pocket or the radius of the plunge. With non-centercutting tools, the arc of the helical plunge has to be at least twice the diameter of the tool, so the center of the tool is never plunging. If your arc is smaller than 2x the diameter, you'll be mashing the metal out of the way instead of cutting it. Your other option is to pre-drill a clearance hole and plunge the cutter over the center of that and go to town.

  5. #5
    PaulT is offline Stainless
    Join Date
    Mar 2002
    Location
    Brisbane, CA, USA
    Posts
    1,663

    Default

    Ron-

    In mild steel with carbide, my rule of thumb for RPM would be:

    RPM = 4 x SFM / DIAMETER = 4 x 400 / .625 = 2560 RPM

    Some inserts will do better than 400 SFM in mild steel, but even if you figure 800 SFM your RPM seems way too high.

    I'd find out what SFM is recommended by the manufacturer for these inserts in steel, but if you can't find that info try knocking your RPM down to around 3000 and see how it cuts.

    To figure a ball park feed rate and chip load, I use the rule of thumb:

    Chip Load = DIAMETER/200 = .625/200 = .003125

    Feed Rate = RPM x Chip Load x Num Flutes = 3000 x .003125 x 2 = 18.75 ipm

    That's a starting point RPM and feed rate, if the machine can handle it bump up both and see how it reacts, but I don't think you'll be able to get back up to 8000 RPM and have the inserts live very long.

    Paul T.

  6. #6
    So CA Machinist is offline Aluminum
    Join Date
    Jun 2008
    Location
    Covina, CA USA
    Posts
    56

    Default

    Sorry about the lack of info.

    The pocket is 5.4" x 1.8"

    I'm going to run it at .150" depth @ 25 ipm & 4500 rpm and see what happens
    With the other side of the inserts. With coolant

    Ron

  7. #7
    Bobw's Avatar
    Bobw is offline Diamond
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    4,925

    Default

    I would knock the SFM down a bit, 1300sfm is pushing it, you could get away with that with a narrow engagement, but not with full slotting. I would knock it down to under 800sfm, and probably start out at about 5-600. Feed maybe .003 per tooth full depth.

    Also I much prefer a straight ramp than a tight helix into the material. You end up plunging at a steeper angle than you intended on the inside of the helix, seems a little tougher on the tools. If you ramp the 5" across, you'll be at the bottom in a single pass, no need to feed to slower on the ramp than you are going to cut the pocket.

    Also dry, at those speeds your inserts will be nicely shattered pretty quick.

  8. #8
    So CA Machinist is offline Aluminum
    Join Date
    Jun 2008
    Location
    Covina, CA USA
    Posts
    56

    Default

    I put my rpm back to 6,000 and i'm cutting .055" depths. @ 72 ipm

    I called Mil-Tec directly. I told him I would do a full depth cut..but I don't have any change if something really bad happens. I know it's not major machining or anything...but I just don't have the resources to get new tooling as much as other places.

    Thanks for your help guys.

    The cutter is holding up pretty well so far.
    I made my arc as big as I could for the pocket..I think that helped the most.

    Ron

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
  •