Turning 1018 Steel Feeds and Speeds
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    98

    Post

    Another project I am working on are some tensile specimens for my department here at school. I need to make about 250 of them. I know how to set up and run the machine (Gildemiester CTX 410 with less than 20 hours on it) However, I don't know much about turning steel. Basically I am just looking for some speeds and feeds.

    The parts are 7" long, 3/4" diameter and is a dogbone with the center being 2" wide at 1/2" diameter with .375" radii bringing it back out to the stock dimension. I am running a 50 someodd degree neutral tool for roughing and a 35 degree for finishing. Though have toyed with the idea of just running the 50 degree one and saving the tool change even though the machine changed tools in the blink of an eye. I find my finises to be better with the separate finishing tool.

    .075" DOC
    .007 IPR
    235 CSS

    I am getting stringy curly chips. Should I push it harder. Or just take it easy.

    Thanks,
    Husker

    DOC and Feeds and Spindle speeds would be greatly appreciated to see if I am in the right ball park.

  2. #2
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,914
    Post Thanks / Like
    Likes (Given)
    3298
    Likes (Received)
    2852

    Post

    I'd leave the DOC where it is, but increase the speed to around 800sfm and the feed to .012 ipr for starters. You have to push 1018 pretty hard to get the chips to break. A .010 feed will usually break them when turning with a O or 5* lead angle tool, but if your diamond is in the neutral position then its 27.5* lead angle will be thinning the chip, hence the need for a heavier feed.

  3. #3
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    98

    Post

    800sfm would be running about how many rpm on the .5" diameter?

    2200?

  4. #4
    Join Date
    Jun 2001
    Location
    WI
    Posts
    656
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    2

    Post

    800 SFM on .5 dia. = 6111 RPM. Yes 1018 will be stringy. A lot depends on the specific toolong you have available. Negative rake tooling will help, as will the style of chipbreaker. As suggested more feed on the rough turning tool, up to .015 depending on your tooling. At 6000 rpm the tool is gonna FLY across that part I haven't made any tensile test specimens since tech school. We had to polish the .500 diameter and the radii at the ends...supposed to stop the specimen from breaking at a tool mark in the finish. But that was on flat belt SBL's. Your machine should be capable of a good enough finish "as turned". Stay with the separate finish tool to hold the size and finish. Using a .03 nose radius tool and .01 feed should yield a 125 finish. You probably want better than a 125 so .005 to .007 range ... even less if you are using a .015 nose radius.

  5. #5
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    98

    Post

    How do you figure the tool life will be at that speed?. I can only run up to 5000 rpm though. I'll play with it. But thanks for the advice.

    Husker

  6. #6
    Join Date
    Jun 2001
    Location
    WI
    Posts
    656
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    2

    Post

    Was never involved in any sort of "production" runs, but I'm guessing a couple inserts will do your whole batch.

  7. #7
    Join Date
    May 2005
    Location
    Ohio
    Posts
    385
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    88

    Post

    I finish 1018 around 1000 sfm. Since you are limited to 5000 rpm I'd run at a constant rpm of around 4500 for the whole part (for finishing). You'll likely see surface finish better at the larger diameters than at the smaller diameter. I use a steel grade insert...Sandvik VNMG 331 PF 4015 with good tool life.

    Rough at about 600 sfm with the feed rate suggested (.015).

  8. #8
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,402
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    98

    Post

    Was going to start cutting them today but am having problems getting the tail stock to engage. I am all programed and ready to go. Other than the fact that the tail stock will not register as engaged agianst the part. When the tailstock is in this state it locks most functions of the machine out. Basically the only M code that will activate is M54 which retracts the tailstock. So after a few hours on the horn with a DMG applications engineer (whom I met when he set up the machine) I have made some headway with the tailstock. I can at least get it to come out of alarm and sometimes reference into home position. But as far as getting a program to run with it engaged I have not had any luck yet. Hopefully service will be coming to visit soon. It's too bad really becuase a service guy was just here this morning (before I had the issue with the tail stock) working on a sprint 20 that we have on show for applictions testing.

  9. #9
    Join Date
    Dec 2013
    Location
    NorCal
    Posts
    58
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    23

    Default

    I know this is an old one, but it's all I'm finding on turning 1018.

    Machine: Haas SL30
    Material: 2" 1018 Solid Round
    Insert: Iscar CNMG 432-GN IC8025
    Feed: Tried 0.008 to 0.02
    RPM: Tried from 800-3400, also tried CSS
    DoC: Tried 0.075, 0.100 & 0.125
    Roughing angle: 0

    I'm having a tough time getting chips to break and it just wads up into a stringy mess and does bad things. They'd chip fine if it were just a couple straight cuts to the OD, but it tapers to a 60deg point like so > and it starts wadding up after the first couple passes. It does seem like more rpm is the way to go, but I've had a couple big chips in the insert at higher rpm and I'm hesitant to get aggressive with it again.

    Not seeing how to upload files, but the 'back to square one' code is below. Any advice would be much appreciated.

    %
    O00072
    (PROGRAM NAME - Expendable Tip P2)
    G20
    (TOOL - 4 - 80 DEG. INSERT CNMG-432)
    G0 T0404
    G18
    G97 S800 M03
    G0 G54 X1.8424 Z.086 M08
    G99 G1 Z.056 F.01 M31
    Z-1.6125
    X2.03 Z-1.7749
    X2.0724 Z-1.7537
    G0 Z.086
    X1.6549
    G1 Z.056
    Z-1.45
    X1.6577 Z-1.4525
    X1.8624 Z-1.6298
    X1.9049 Z-1.6086
    G0 Z.086
    X1.4673
    G1 Z.056
    Z-1.2876
    X1.6577 Z-1.4525
    X1.6749 Z-1.4674
    X1.7173 Z-1.4461
    G0 Z.086
    X1.2798
    G1 Z.056
    Z-1.1252
    X1.4873 Z-1.3049
    X1.5297 Z-1.2837
    G0 Z.086
    X1.0922
    G1 Z.056
    Z-.9627
    X1.2998 Z-1.1425
    X1.3422 Z-1.1213
    G0 Z.086
    X.9046
    G1 Z.056
    Z-.8003
    X1.1122 Z-.9801
    X1.1546 Z-.9589
    G0 Z.086
    X.7171
    G1 Z.056
    Z-.6379
    X.9246 Z-.8176
    X.9671 Z-.7964
    G0 Z.086
    X.5295
    G1 Z.056
    Z-.4754
    X.7371 Z-.6552
    X.7795 Z-.634
    G0 Z.086
    X.3419
    G1 Z.056
    Z-.313
    X.5495 Z-.4928
    X.5919 Z-.4716
    G0 Z.086
    X.1544
    G1 Z.056
    Z-.1506
    X.3619 Z-.3303
    X.4044 Z-.3091
    G0 Z.086
    X-.0332
    G1 Z.056
    Z.0119
    X.1744 Z-.1679
    X.2168 Z-.1467
    (***FINISH***)
    G97 S1600
    G0 Z.0404 F.01
    X-.0384
    G1 Z.0104
    X1.6525 Z-1.454
    X2.0216 Z-1.7737
    X2.0641 Z-1.7524 M09
    G0 X10.0 Z5.0 M05
    M30
    %

  10. #10
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    8,932
    Post Thanks / Like
    Likes (Given)
    941
    Likes (Received)
    2762

    Default

    Make sure you use an insert with the proper chip breaker for the feed range and depth of cut you intend to use. Just slapping any old insert on is not good enough.

  11. Likes Mtndew, corndog liked this post
  12. #11
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,307
    Post Thanks / Like
    Likes (Given)
    2683
    Likes (Received)
    1889

    Default

    Quote Originally Posted by corndog View Post
    I know this is an old one, but it's all I'm finding on turning 1018.

    Machine: Haas SL30
    Material: 2" 1018 Solid Round
    Insert: Iscar CNMG 432-GN IC8025
    Feed: Tried 0.008 to 0.02
    RPM: Tried from 800-3400, also tried CSS
    DoC: Tried 0.075, 0.100 & 0.125
    What grade and coating is your insert?
    800-1000 sfpm for roughing and finishing. Or max rpm if your part is small.
    d.o.c. ranging from .05-.25 depending on your HP.
    1018 cuts like butter, I don't get how people struggle with it.

  13. Likes Philabuster liked this post
  14. #12
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,557
    Post Thanks / Like
    Likes (Given)
    5925
    Likes (Received)
    2126

    Default

    Lose the G97 and go with G96 constant-surface speed. I may be wrong, but I think the GN chipbreaker on that insert is kind of heavy. Try moving to a lighter chip-breaker if you can.

  15. #13
    Join Date
    Feb 2009
    Location
    Merrimac, Massachusetts
    Posts
    693
    Post Thanks / Like
    Likes (Given)
    606
    Likes (Received)
    220

    Default

    for stringy material like 1026 tube, DOM and 1018 I run Walter CNMG431 in WPP10S grade with an MP3 chip breaker

    1018 around 1000sfm .012 feed .06 depth of cut (Haas ST-10)

    These inserts break chips in DOM like a dream as well I run a bunch of parts in 2.5"x .375 wall DOM with the WNMG431 version on a 1" bar breaks chips like a dream and leaves an awesome finish.

    20130207_135418-1024x768-.jpg

    Jason,

  16. Likes corndog liked this post
  17. #14
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    5,452
    Post Thanks / Like
    Likes (Given)
    106
    Likes (Received)
    2032

    Default

    Anyone notice a 10 year old thread got bumped?

  18. Likes alliancefab liked this post
  19. #15
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    7,790
    Post Thanks / Like
    Likes (Given)
    9754
    Likes (Received)
    8437

    Default

    Quote Originally Posted by Dualkit View Post
    Anyone notice a 10 year old thread got bumped?
    But at least this time it was for somebody actually asking a question, not some nitwit trying to sell something.

  20. #16
    Join Date
    Feb 2009
    Location
    Merrimac, Massachusetts
    Posts
    693
    Post Thanks / Like
    Likes (Given)
    606
    Likes (Received)
    220

    Default

    Quote Originally Posted by Dualkit View Post
    Anyone notice a 10 year old thread got bumped?
    I did right after I posted. But Bobw is right at least he isn't selling something.

  21. #17
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7,236
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1931

    Default

    Quote Originally Posted by huskermcdoogle View Post
    Another project I am working on are some tensile specimens for my department here at school. I need to make about 250 of them. I know how to set up and run the machine (Gildemiester CTX 410 with less than 20 hours on it) However, I don't know much about turning steel. Basically I am just looking for some speeds and feeds.

    The parts are 7" long, 3/4" diameter and is a dogbone with the center being 2" wide at 1/2" diameter with .375" radii bringing it back out to the stock dimension. I am running a 50 someodd degree neutral tool for roughing and a 35 degree for finishing. Though have toyed with the idea of just running the 50 degree one and saving the tool change even though the machine changed tools in the blink of an eye. I find my finises to be better with the separate finishing tool.

    .075" DOC
    .007 IPR
    235 CSS

    I am getting stringy curly chips. Should I push it harder. Or just take it easy.

    Thanks,
    Husker

    DOC and Feeds and Spindle speeds would be greatly appreciated to see if I am in the right ball park.
    .
    .
    7" long and 3/4 to 1/2" dia
    .
    feeds and speeds assume rigid parts, since that is a long length to dia ratio you will get chatter if you push to limits.
    .
    long stringy chips some material make long chips easy. often material is selected that makes nicer chips. real bad material often chip breakers and different feeds and speeds do little to stop long stringy chips. programming feed changes of
    G91
    -0.09 F10.
    G4 P1000
    -0.01 F0.1
    often the feed change rate will break chip. or a flat out pause delay of a second periodically often works too. some cnc have a chip breaking cycle

  22. #18
    Join Date
    Dec 2013
    Location
    NorCal
    Posts
    58
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    23

    Default

    Apologies if posting in this one is against the rules/etiquette. Definitely not selling anything!

    Quote Originally Posted by Mtndew View Post
    What grade and coating is your insert?
    800-1000 sfpm for roughing and finishing. Or max rpm if your part is small.
    d.o.c. ranging from .05-.25 depending on your HP.
    1018 cuts like butter, I don't get how people struggle with it.
    Not sure what the exact coating is, but here's the family of insert: ISCAR Cutting Tools - Metal Working Tools - CNMG-GN : 5593939 - CNMG 432-GN

    I'm not seeing the IC8025 grade. If the grades are numerically close in type, this would be the closest: ISCAR Cutting Tools - Metal Working Tools - Grade : IC815

    It's a 30hp machine. I can get chips to break on the very OD with DoC from 0.050 to 0.100, but it seemed worse going beyond that. I agree it cuts like butter....just a giant string of butter that likes to wad up and ruin parts/inserts. I could probably run all day if I added a couple/few interrupts to manually remove wads, which I may have to do in order to run today and tomorrow.

    Quote Originally Posted by Jashley73 View Post
    Lose the G97 and go with G96 constant-surface speed. I may be wrong, but I think the GN chipbreaker on that insert is kind of heavy. Try moving to a lighter chip-breaker if you can.
    I'll tinker with CSS some more today, but the max rpm is 3400, so it's like a race to get to the center before it wads up. Also, I noticed that when I set the rpm to 1000 CSS in mastercam, it's actually running at 2000. Suppose I'm not fully understanding how it works..

    Quote Originally Posted by alliancefab View Post
    for stringy material like 1026 tube, DOM and 1018 I run Walter CNMG431 in WPP10S grade with an MP3 chip breaker

    1018 around 1000sfm .012 feed .06 depth of cut (Haas ST-10)

    These inserts break chips in DOM like a dream as well I run a bunch of parts in 2.5"x .375 wall DOM with the WNMG431 version on a 1" bar breaks chips like a dream and leaves an awesome finish.

    20130207_135418-1024x768-.jpg

    Jason,
    Thanks for that Jason. I'll google around, but can you recommend a place that has them in stock and will ship overnight? Edit, this one? CNMG432 MP3 WPP1S Grade Carbide Turning 476111 - MSC As overpriced as MSC is, they have a warehouse nearby and parts get here quick. I'll give these a shot.

    Can someone explain how changing the roughing angle may help, as well as what a safe angle is to use that doesn't cause the backside of the tool to interfere with the material?

    Again, apologies for posting in an old thread and thanks very much for the replies.

  23. #19
    Join Date
    Feb 2009
    Location
    Merrimac, Massachusetts
    Posts
    693
    Post Thanks / Like
    Likes (Given)
    606
    Likes (Received)
    220

    Default

    Quote Originally Posted by corndog View Post
    Apologies if posting in this one is against the rules/etiquette. Definitely not selling anything!

    Thanks for that Jason. I'll google around, but can you recommend a place that has them in stock and will ship overnight? Edit, this one? CNMG432 MP3 WPP1S Grade Carbide Turning 476111 - MSC

    As overpriced as MSC is, they have a warehouse nearby and parts get here quick. I'll give these a shot.

    Again, apologies for posting in an old thread and thanks very much for the replies.
    MSC is your best bet for overnight ( even though I dislike them ) a 431 with the smaller radius will be better for breaking the chip. that one you linked is the 432.

    Jason,

  24. #20
    Join Date
    Dec 2013
    Location
    NorCal
    Posts
    58
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    23

    Default

    Quote Originally Posted by alliancefab View Post
    MSC is your best bet for overnight ( even though I dislike them ) a 431 with the smaller radius will be better for breaking the chip. that one you linked is the 432.

    Jason,
    I know it's bad form, but I was in feeling the pressure and had already ordered the 432 when you posted this. Anyway, just wanted to thank you and the other folks for bringing up the insert type. That Walter insert with the MP3 chip breaker has made all the difference. The best success I had was with a program similar to the one I posted, but with a CSS hi/low of 2000/3000 and 0.060 DoC. With the Iscar insert I was using, I *could* get a good part, but I'd have to stop the machine a bunch to clear the rats nests. Sometimes it'd take me ten minutes to get through the program, versus 80 seconds right now. And with that Walter insert, it clears all chips except for the very center and it's not enough to do anything. The finish is great and the insert life it muuuuuuch better. Just for fun I snapped a pic of the difference in chip breakers between the two. Thanks again!


  25. Likes alliancefab, ARB, Finegrain liked this post

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
  •