584,817 active members*
5,140 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > Feed stops when commanding new spindle speed
Results 1 to 7 of 7
  1. #1
    Join Date
    Jun 2008
    Posts
    113

    Feed stops when commanding new spindle speed

    Hi,

    I'm trying to eliminate resonance of the workpiece with code such like this:
    G97 S500 M3
    G0 X100 Z2
    G1 W-2 S400
    G1 W-2 S500
    G1 W-2 S400
    G1 W-2 S500
    ...etc

    It works, but on every line the feed stops until the spindle is up to the new speed, ruining the surface finish. How do I make it so that the movement is smooth?
    The machine is a Puma 400 LM with Fanuc 18i-T control.

    THANKS A LOT!!!

  2. #2
    Join Date
    Aug 2011
    Posts
    2517

    Re: Feed stops when commanding new spindle speed

    generally you can't. the machine waits for the spindle speed to be whatever is programmed before continuing. all lathes do that.
    you could try either smaller speed increments/decrements or try G96, again with small increments.
    there might be a parameter you could change to tell it not to wait for the speed signal to complete before continuing.
    look in the parameter manual for the section on parameters relating to the spindle and/or M.S.T functions.

  3. #3
    Join Date
    Aug 2011
    Posts
    2517

    Re: Feed stops when commanding new spindle speed

    update:

    I found only 1 parameter that may help....

    3708 bit 0 SAR
    The spindle speed arrival signal is:
    0 : Not checked
    1 : Checked

    if you make 3708 bit 0 = 0 it may solve your problem.....

  4. #4
    Join Date
    Aug 2011
    Posts
    2517

    Re: Feed stops when commanding new spindle speed

    update update:

    there's another one that may be more suitable....

    3715 bit 0 NSAx
    This parameter specifies an axis for which confirmation of the spindle
    speed reached signal (SAR) is unnecessary when a move command is
    executed for the axis. When a move command is issued only for an axis
    for which 1 is set in this parameter, the spindle speed reached signal
    (SAR) is not checked.
    0 : Confirmation of SAR is necessary.
    1 : Confirmation of SAR is unnecessary.

    this parameter has 8 bits for each axis.
    find the one for Z axis and set it to xxxxxxx1 (x=ignore)
    then you should be able to change the speed randomly and the Z axis movement isn't affected.

  5. #5
    Join Date
    Jun 2008
    Posts
    113

    Re: Feed stops when commanding new spindle speed

    You have been very helpful, I will try your suggestions at work on monday. I'll also post my resonance eliminator macro in case somebody will find it useful...

  6. #6
    Join Date
    Jun 2008
    Posts
    113

    Re: Feed stops when commanding new spindle speed

    Late update: 3708 bit 0 SAR did the trick. The other parameters did not work. Thanks a lot!

  7. #7
    Join Date
    Aug 2011
    Posts
    2517

    Re: Feed stops when commanding new spindle speed

    glad you got it sorted. please post that macro you mentioned above. I'm sure many people here will find it interesting :-)

Similar Threads

  1. Feed rates and speed of spindle etc
    By Raf-1200 in forum SolidCAM for SolidWorks and SolidCAM for Inventor
    Replies: 5
    Last Post: 11-02-2013, 09:29 AM
  2. feed rates and spindle speed
    By alanstclair in forum Chinese Machines
    Replies: 6
    Last Post: 07-15-2012, 03:25 PM
  3. About feed rate and spindle speed
    By yanlo in forum Uncategorised MetalWorking Machines
    Replies: 2
    Last Post: 11-02-2009, 12:34 PM
  4. spindle speed/feed rate
    By lamed in forum MetalWork Discussion
    Replies: 8
    Last Post: 06-03-2009, 12:25 PM
  5. CNC feed rate and spindle speed
    By misc.garfield in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 5
    Last Post: 01-30-2008, 12:20 AM

Tags for this Thread

Posting Permissions

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