Turning 18" D2 Steel plz help speed/feed/doc
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 29
  1. #1
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Turning 18" D2 Steel plz help speed/feed/doc

    Hello, 1st post from a self taught CNC Lathe operator...

    I run a Haas SL30 Lathe, I need to turn a bunch of patterns from 18" D2 steel(4" thick) and it is taking me so long it is TORTURE...
    Since I am self taught I never really learned how fast to turn parts or how hard I can run my machine.

    I have my RPM(CSS) set at 415 and a max spindle RPM of 600. This is where im unsure because my chuck is only 12" so I need to use a jig plate to hold large parts and I am afraid if I turn at high RPMs that the part may come loose.

    I currently have my depth of cut at .05 and my feed set at .01 IPR. I use CNMG 432 inserts. I usually have to change my insert every hour or so, is that too long?

    I work in a job shop that does all prototype work, no production.

    Please give me some tips
    Last edited by FleetFarmer; 04-08-2021 at 08:05 AM.

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,204
    Post Thanks / Like
    Likes (Given)
    2461
    Likes (Received)
    3084

    Default

    I used to run an SL30. If your setup is rigid enough (and only you are going to know that), I would goto an LNMX style insert. https://www.mscdirect.com/product/details/63920201

    These are in the toolholder tangentially, allowing higher feed and doc. Can't recommend a coating as I have been away from that for a long time now. Hopefully someone can help you out.

  3. #3
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    368
    Post Thanks / Like
    Likes (Given)
    85
    Likes (Received)
    109

    Default

    I think your cutting parameters are in the ballpark. The depth of cut is light, but it depends if your machine can take a bigger cut at that diameter. I know those Haas's aren't known for their rigidity and horsepower. I would slowly up the depth of cut while watching the load meter and listening to the machine to see if it sounds right.

    If 600 rpm is the max that you feel comfortable spinning your chuck, then I would trust that instinct. You don't want to push it and find where that limit is.

  4. #4
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    5,100
    Post Thanks / Like
    Likes (Given)
    1334
    Likes (Received)
    2891

    Default

    I'd go go go until the motor can't push anymore. Then back it off a cunt hair. If you blow the machine up, use it as logic to get an Okuma. By the sounds of your set up, Haas is probably not the right equipment.

    OTOH, you might be more successful doing some major removal by Roughing on a 3A Milling Machine.

    R

  5. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,857
    Post Thanks / Like
    Likes (Given)
    5534
    Likes (Received)
    3738

    Default

    Quote Originally Posted by FleetFarmer View Post
    Hello, 1st post from a self taught CNC Lathe operator...

    I run a Haas SL30 Lathe, I need to turn a bunch of patterns from 18" D2 steel(4" thick) and it is taking me so long it is TORTURE...
    Since I am self taught I never really learned how fast to turn parts or how hard I can run my machine.

    I have my RPM(CSS) set at 415 and a max spindle RPM of 600. This is where im unsure because my chuck is only 12" so I need to use a jig plate to hold large parts and I am afraid if I turn at high RPMs that the part may come loose.

    I currently have my depth of cut at .05 and my feed set at .01 IPR. I use CNMG 432 inserts. I usually have to change my insert every hour or so, is that too long?

    I work in a job shop that does all prototype work, no production.

    Please give me some tips

    Take as large of a cut as the machine will allow, and feed it accordingly.

  6. #6
    Join Date
    Mar 2021
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    3

    Default

    0.05 DOC is an absolute killer. No wonder it's taking forever.
    How much material do you need to remove?
    We machine a lot of this stuff. The typical cutting data we use is
    D.O.C. 0.157
    Feed 0.014
    SS 590 ft/min
    We're gripping in a 12" Hydraulic chuck.
    We use Seco CNMG 433-M5 (120412-M5), Grade TP0501
    We can cut for around 20 mins at that data.
    Some of these things require the removal of 70Kg of material.
    If you could at least double the DOC you've halved the time.
    But maybe you'll run out of torque at 18" dia

  7. Likes Joe Miranda liked this post
  8. #7
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,540
    Post Thanks / Like
    Likes (Given)
    1656
    Likes (Received)
    2107

    Default

    Quote Originally Posted by Mike1974 View Post
    I used to run an SL30. If your setup is rigid enough (and only you are going to know that), I would goto an LNMX style insert. https://www.mscdirect.com/product/details/63920201

    These are in the toolholder tangentially, allowing higher feed and doc. Can't recommend a coating as I have been away from that for a long time now. Hopefully someone can help you out.
    How much torque does an SL30 have?

    LNMX at 18" is going to need a LOT of grunt to break a chip...

  9. #8
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,323
    Post Thanks / Like
    Likes (Given)
    3836
    Likes (Received)
    2865

    Default

    I cut D2 all the time.....
    I want to preface this by saying I have no idea what your machines capabilities are and I do not have a clue how well you are holding your part.
    When I have a good grip on it....I rough at 800 SFM .01"/REV .100"-.125" per side DOC. I leave .02" per side for finishing and .005" in Z. I finish at 1000SFM .006"-.008" /rev.
    Only you will be able to gage if your machine and setup are capable of that ...or possibly more.

  10. #9
    Join Date
    Jun 2016
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    87
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    40

    Default

    Quote Originally Posted by toolsteel View Post
    I cut D2 all the time.....
    I want to preface this by saying I have no idea what your machines capabilities are and I do not have a clue how well you are holding your part.
    When I have a good grip on it....I rough at 800 SFM .01"/REV .100"-.125" per side DOC. I leave .02" per side for finishing and .005" in Z. I finish at 1000SFM .006"-.008" /rev.
    Only you will be able to gage if your machine and setup are capable of that ...or possibly more.
    What inserts are you using for that?

  11. Likes BT Fabrication liked this post
  12. #10
    Join Date
    Sep 2009
    Location
    tonawanda new york
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    63
    Likes (Received)
    127

    Default

    I would refer to the load meter when you are cutting to determine your cutting parameters

  13. #11
    Join Date
    Nov 2019
    Country
    CANADA
    State/Province
    Ontario
    Posts
    540
    Post Thanks / Like
    Likes (Given)
    829
    Likes (Received)
    127

    Default

    I was gonna ask what grade is the insert and geometry, that makes the most difference. id be feeding in a little deeper, my smaller lathe can take 0.100" all day long or better, feed it hard until the chip starts turning blue. it does sound pretty light of a cut, and all comes down to rigidity and sound in the cut. also find what the manufacturer of the insert reccomends and start in the middle. if worried, turn the feed rate or speed down and turn it up till it starts bogging the spindle down

  14. #12
    Join Date
    Jul 2003
    Location
    Carson City, Nv. USA
    Posts
    918
    Post Thanks / Like
    Likes (Given)
    728
    Likes (Received)
    491

    Default

    Quote Originally Posted by FleetFarmer View Post
    Hello, 1st post from a self taught CNC Lathe operator...

    I run a Haas SL30 Lathe, I need to turn a bunch of patterns from 18" D2 steel(4" thick) and it is taking me so long it is TORTURE...
    Since I am self taught I never really learned how fast to turn parts or how hard I can run my machine.

    I have my RPM(CSS) set at 415 and a max spindle RPM of 600. This is where im unsure because my chuck is only 12" so I need to use a jig plate to hold large parts and I am afraid if I turn at high RPMs that the part may come loose.

    I currently have my depth of cut at .05 and my feed set at .01 IPR. I use CNMG 432 inserts. I usually have to change my insert every hour or so, is that too long?

    I work in a job shop that does all prototype work, no production.

    Please give me some tips

    As others have said, go deeper on your depth of cut, if your setup will allow.

    However, I think another issue is your max allowable RPM. Not saying it is not justified, but the problem is that you are rubbing the crap out of the insert as you get toward center & your SFM is going through the floor.

  15. #13
    Join Date
    Nov 2012
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,323
    Post Thanks / Like
    Likes (Given)
    3836
    Likes (Received)
    2865

    Default

    Quote Originally Posted by 70olds View Post
    What inserts are you using for that?
    Sandvik WNMG 432-PM 4315

  16. #14
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    9

    Default

    On the sl30 i use, i do .250 doc on diameter at 0.016 ipr with a kennametal roughing insert for od turning. For facing i do a 0.050 doc at 0.018 ipr with same insert.
    To me if you have a good work holding then bump the doc up and do the same for your max rpm as well as the feed rate.

  17. #15
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,204
    Post Thanks / Like
    Likes (Given)
    2461
    Likes (Received)
    3084

    Default

    Quote Originally Posted by gregormarwick View Post
    How much torque does an SL30 have?


    LNMX at 18" is going to need a LOT of grunt to break a chip...
    Don't know, but cut 12" diameter with that insert all the time, .15 ish pet side, .02" rev turning, .05 facing, .03" rev

  18. #16
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    5,945
    Post Thanks / Like
    Likes (Given)
    6435
    Likes (Received)
    3309

    Default

    Quote Originally Posted by FrankieB View Post
    On the sl30 i use, i do .250 doc on diameter at 0.016 ipr with a kennametal roughing insert for od turning. For facing i do a 0.050 doc at 0.018 ipr with same insert.
    To me if you have a good work holding then bump the doc up and do the same for your max rpm as well as the feed rate.
    I'm struggling to see any Haas lathe taking 1/2" off per pass at 18" diameter.

    I did a lot of 14 and 16" 1045 on a 30HP (DC) Mazak with 3 headstock gear ranges from 0-2000 RPM. It had the grunts for certain. I got the best life out of CNMG 632 inserts/holders and I was usually around a .150" DOC and .016-.018" IPR for roughing. I kept the SFM pretty low, I liked to see my chips barely tan. Probably only 200ish RPM for the OD stuff at 16".

    I would run my 100-140 lb blanks to 900 rpm max with a 12" chuck and step jaws gripping on .200" of the OD. I think I would keep it under 500 for an 18" x 4" blank. Atleast until I got most of the weight and/or imbalance machined off of it.

  19. Likes Joe Miranda liked this post
  20. #17
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    368
    Post Thanks / Like
    Likes (Given)
    85
    Likes (Received)
    109

    Default

    Quote Originally Posted by Garwood View Post
    I'm struggling to see any Haas lathe taking 1/2" off per pass at 18" diameter.

    I did a lot of 14 and 16" 1045 on a 30HP (DC) Mazak with 3 headstock gear ranges from 0-2000 RPM. It had the grunts for certain. I got the best life out of CNMG 632 inserts/holders and I was usually around a .150" DOC and .016-.018" IPR for roughing. I kept the SFM pretty low, I liked to see my chips barely tan. Probably only 200ish RPM for the OD stuff at 16".

    I would run my 100-140 lb blanks to 900 rpm max with a 12" chuck and step jaws gripping on .200" of the OD. I think I would keep it under 500 for an 18" x 4" blank. Atleast until I got most of the weight and/or imbalance machined off of it.
    I read the statement ".250 doc on diameter" as .125" doc per side.

  21. #18
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    5,945
    Post Thanks / Like
    Likes (Given)
    6435
    Likes (Received)
    3309

    Default

    Quote Originally Posted by wmpy View Post
    I read the statement ".250 doc on diameter" as .125" doc per side.
    That sounds more believable then.

  22. #19
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    4,540
    Post Thanks / Like
    Likes (Given)
    1656
    Likes (Received)
    2107

    Default

    Quote Originally Posted by Mike1974 View Post
    Don't know, but cut 12" diameter with that insert all the time, .15 ish pet side, .02" rev turning, .05 facing, .03" rev
    And that breaks a chip? What material?

    When I was playing with LNMX I was pushing close to 1mm/r before it would break a chip at 4mm DOC in 16" 4340V. Anything less and it was just ribbons and birds nests. Tool failure at that was unpredictable, sudden and catastrophic. Switched back to CNMG, 7mm DOC at .5mm/r, slightly lower MRR than the LNMX but much better process security.

    I did use the LNMX with much more success on a batch of 8" 4145H, but the CNMG is still a better all rounder.

    Quote Originally Posted by Garwood View Post
    I'm struggling to see any Haas lathe taking 1/2" off per pass at 18" diameter.

    I did a lot of 14 and 16" 1045 on a 30HP (DC) Mazak with 3 headstock gear ranges from 0-2000 RPM. It had the grunts for certain. I got the best life out of CNMG 632 inserts/holders and I was usually around a .150" DOC and .016-.018" IPR for roughing. I kept the SFM pretty low, I liked to see my chips barely tan. Probably only 200ish RPM for the OD stuff at 16".
    Why such a huge insert for that DOC? The 7mm that I mention above is because it's the max. DOC of a CNMG 120416, which is think is a 434 (I don't understand the US nomenclature, so maybe I'm mistaken)

  23. #20
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    103

    Default

    Quote Originally Posted by gregormarwick View Post
    How much torque does an SL30 have?

    LNMX at 18" is going to need a LOT of grunt to break a chip...
    I would also avoid LNMX inserts. Quite frankly, I do not like them at all. I think the CNMG is a much better tool for him. I wish he posted a picture.
    He may have better luck turning that chuck with a breaker bar than he will a Haas, lathe spindle. I like the Haas mills, but those lathes are complete shit.


Tags for this Thread

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
  •