okuma hem/hsm not keeping up with called feed
Close
Login to Your Account
Likes Likes:  0
Results 1 to 11 of 11
  1. #1
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,649
    Post Thanks / Like
    Likes (Given)
    2624
    Likes (Received)
    628

    Default okuma hem/hsm not keeping up with called feed

    I program for six different Okuma mills with osp200 and osp300 controls. When running high efficient milling paths the machines cannot keep up with a constant say 100 ipm feed. It will achieve those speeds in the field but slows when converting from reposition feed to cut feed. Also when the circles get tight say .5" - .25" rad it slows here also to say 40 ipm. It was worse until I learned about g131 j2 hi pro or nurbs. That did help but still not what a modern machine should do in my opinion. I understand acceleration from stop to go but this seems different to me. I saw this vid on youtube of similar machine keeping high feeds even in tight rads so there must be something I am not doing correctly. I program with Mastercam 2020 and post g01 g02/g03 code. Would only g01 improve?

    YouTube

    Thanks

    Steve Austin

  2. #2
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    192
    Post Thanks / Like
    Likes (Given)
    34
    Likes (Received)
    93

    Default

    Are you dealing with hi-cut or supernurbs? Are you setting it appropriately, or just turning it on? Which machine platforms are you dealing with?

    I suspect you aren't using the look ahead / shape comp correctly, because my M560V with just the hi-cut does a pretty impressive job until you crank the tolerance way down, or start asking it to move in 3 axis simultaneously.

    Once you are certain look ahead is set right, then you can move on to other "tricks" like making sure sharp corners are posted with a fillet, etc... In your demo video, I can pretty much guarantee everything is running with huge tolerance settings. Ever try bumping the E value up to .010 inch? It helps a bunch.

  3. #3
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    954
    Post Thanks / Like
    Likes (Given)
    210
    Likes (Received)
    590

    Default

    Make sure in mastercam you are converting lines to arcs in your tolerance page. When it’s running and studdering do you see any I or j codes or lots of tiny line moves?
    Don


    Sent from my iPhone using Tapatalk Pro

  4. #4
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,649
    Post Thanks / Like
    Likes (Given)
    2624
    Likes (Received)
    628

    Default

    I think the tolerance could be set too tight. One machine has the supernurbs option and the others have hicutpro. One machine is a mu6300 ac trunnion. 3 are mu4000 bc trunnions. The other 2 are ma600H HMC. I am converting lines to arcs. Mastercam has micro lift of .01" in z when repositioning. So that would be 3 axis interpolation. Could that cause the slow down? I could change that if needed. Thanks for your help.

  5. #5
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    The first time this happened to me it was the arc tolerance set too tight. I bet that’s your scum bag. Good luck!

  6. #6
    Join Date
    Mar 2011
    Location
    NY USA
    Posts
    828
    Post Thanks / Like
    Likes (Given)
    172
    Likes (Received)
    546

    Default

    OSP300 is one of the faster controls out there...it's not a volume of code problem, the control is slowing things down on purpose. I suspect tolerance is too tight in the high cut settings.

  7. #7
    Join Date
    Apr 2006
    Location
    Ga.
    Posts
    130
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    12

    Default

    Try using G131, it goes like this.

    G20
    G90 G80 G40 G0
    M6 T1
    (T1 - 1/4 FLAT ENDMILL - TOOL DIA. - .25)
    G15 H1
    M11
    G131 E.01 F750. (E IS THE PRECSION SETTING, F IS THE MAX FEED RATE)
    (THE SMALLER THE E VALUE IS THE TIGHTER THE TOLERANCE BUT SLOW FEED)
    G0 G90 X-1.3125 Y.0375 A0.
    S6500 M3
    G56 H1 Z1. M8
    Z.05
    G1 Z-1. F50.
    G41 D1 X-1.3375 F30.
    G3 X-1.375 Y0. I0. J-.0375
    X0. Y-1.375 I1.375 J0.
    X1.375 Y0. I0. J1.375
    X0. Y1.375 I-1.375 J0.
    X-1.375 Y0. I0. J-1.375
    G1 Y-.01
    G3 X-1.3375 Y-.0472 I.0375 J.0003
    G1 X-1.3372
    G40 X-1.3122 Y-.047
    G0 Z1. M9
    G130 (CANCELL'S THE HSM MODE)
    (MAKE SURE TO CANCELL IT AFTER EACH MILLING OP)
    M5
    Z30
    M30

    Hope this helps.

  8. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,569
    Post Thanks / Like
    Likes (Given)
    4170
    Likes (Received)
    2724

    Default

    What control?
    The older Okuma mills have the old school Hi Cut, and it's AWFUL.
    The Hi-Cut Pro is insane how good it is.

  9. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,569
    Post Thanks / Like
    Likes (Given)
    4170
    Likes (Received)
    2724

    Default

    Quote Originally Posted by rickyt View Post
    G130 (CANCELL'S THE HSM MODE)
    (MAKE SURE TO CANCELL IT AFTER EACH MILLING OP)
    M5
    Z30
    M30

    Hope this helps.
    No need to cancel Hi Cut. Ours is on constantly.

  10. #10
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    192
    Post Thanks / Like
    Likes (Given)
    34
    Likes (Received)
    93

    Default

    I think you still need to confirm what the "E" setting is on your code. It's not one-size-fits-all. A value that will give good accuracy while finishing is going to slow it to a crawl when you are roughing.

    The microlift probably isn't hurting much. I also run volumill roughing, and don't notice significant slowdown on the lift during repositioning.

  11. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,421
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1616

    Default

    Quote Originally Posted by lowCountryCamo View Post
    I think the tolerance could be set too tight. One machine has the supernurbs option and the others have hicutpro. One machine is a mu6300 ac trunnion. 3 are mu4000 bc trunnions. The other 2 are ma600H HMC. I am converting lines to arcs. Mastercam has micro lift of .01" in z when repositioning. So that would be 3 axis interpolation. Could that cause the slow down? I could change that if needed. Thanks for your help.
    Not sure about the newer version on MCX, but in the same place as the microlift is a back feedrate. Make sure that is not defaulted to something slow. I usually set mine to 200-300 IPM, doesn't get near that in the little space I am programming, but it is noticeably faster than the 60-100ipm it is programmed at for cutting. Sorry not Okuma specific, but worth checking your settings in MCX.


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
  •