547,434 active members*
2,017 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > No motion with G01 when spindle not running.
Results 1 to 14 of 14
  1. #1
    Registered
    Join Date
    Sep 2008
    Posts
    28

    No motion with G01 when spindle not running.

    Hello

    I have here a FANUC 16iM running a Daewoo 630 horizontal.
    I need to make a back-face with a tool that requires the spindle to be oriented and fed through the pilot hole.... but it wont.
    Of course i could dry-run it or use G00 and be super carefull on the potentios but that is fairly dangerous for some operators.

    Can anyone direct me to the parameter that would allow G01 movement with the spindle in M05 mode ?

    Any help is appreciated !

  2. #2
    Gold Member
    Join Date
    May 2004
    Posts
    4519
    Done.

  3. #3
    Community Moderator Al_The_Man's Avatar
    Join Date
    Dec 2003
    Posts
    23776
    It appears to be a Horizontal mill?
    In some cases the OEM will write the ladder as such that if the spindle does not show a spindle up-to-speed signal in G01 then it does not move.
    Also in some cases it is also written in the ladder if the up-to-speed signal fails a feed hold it implemented.
    Just a guess?
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  4. #4
    Gold Member
    Join Date
    Mar 2003
    Posts
    2932
    You might try M84. This is either "G01 possible with spindle stopped" or "4th axis mirror image." depending on which manual you look at.

    If it's mirror image, M80 cancels all mirror image.

  5. #5
    Registered
    Join Date
    Sep 2008
    Posts
    28
    Thanks all for your help !

    The program is in inch/min.
    The program runs smooth on a Matsuura with Fanuc 30i.

    Al is thinking right up my alley.
    I have to find the parameter(s) that ignores the 'spindle rpm reached' check signal when automatic feed motion.
    I am close but still...


    Anybody done that lately and remembers the para# ? LOL
    Al ?

  6. #6
    Registered
    Join Date
    Sep 2008
    Posts
    28
    Quote Originally Posted by dcoupar View Post
    You might try M84. This is either "G01 possible with spindle stopped" or "4th axis mirror image." depending on which manual you look at.

    If it's mirror image, M80 cancels all mirror image.

    I really want the machine to act 'normal' by correcting the parameter.
    It is a second-hand unit and the previous owner must of ordered it that way or disabled the function for operator safety.

    M84 hmm... i dont even know at this moment what that does on the Daewoo! Isn't that the spindle syncronisation command ?
    Will check that out too!

  7. #7
    Registered
    Join Date
    Jun 2007
    Posts
    119
    This causes to start machining before the spindle has reached it's programmed speed.

    3708#0
    the spindle speed arrival signal (SAR) is:
    0 not cheked
    1 cheked

    3715#0
    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.

  8. #8
    Registered
    Join Date
    Sep 2008
    Posts
    28
    Quote Originally Posted by dcoupar View Post
    You might try M84. This is either "G01 possible with spindle stopped" or "4th axis mirror image." depending on which manual you look at.

    If it's mirror image, M80 cancels all mirror image.

    Quote Originally Posted by viorel26 View Post
    This causes to start machining before the spindle has reached it's programmed speed.

    3708#0
    the spindle speed arrival signal (SAR) is:
    0 not cheked
    1 cheked

    3715#0
    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.

    Very much so !
    Thanks for reconfirming this viorel !
    ...but still no feed after the changes to those parameters.

    The M84 works great !!!
    Thank you dcouper !
    M85 or 'Reset' cancels M84

    Now if i would want to remove the necessety to enter M84 for a program that requires feed with spindle. Lets say, (without having researched that corner yet) the M84 triggers a relay to close a loop that allows G1 with M5 and i simply bridge the corresponding contacts, practically activating M84 when power to machine is turned on.
    The relay i chose as example, it could also be a parameter.
    ... anybody has experiance in what could cause problems with 'normal' machining operations?

    I have 4 machines on divers fanucs that run the same program without problem but not that Daewoo. Because she is the oldest and slackiest of the bunch the managment gave me freedom to do what i (and you!) see fit.
    With the parameters savely backed up of course

  9. #9
    Gold Member
    Join Date
    Mar 2003
    Posts
    2932
    There should be a blue(?) book in the electrical cabinet that has a list of the parameters and keep relays. I don't know for sure but there may be a keep relay that controls this.

  10. #10
    Registered
    Join Date
    Feb 2007
    Posts
    312
    another way could be to write a custom macro called by M05 that enable M84
    it is very simple :

    09021
    M05
    M84
    M99

    Don't worry, M05 will act like a normal M05 within the macro even if it is called by M05.

  11. #11
    Registered
    Join Date
    Sep 2008
    Posts
    28
    Uhhhh , I like the macro !
    A very elegant solution. Thank you samu !

    I still want to fiddle with what M84 actually triggers on that Daewoo...physically and/or digital.
    I will keep everyone posted on my findings...

    I cant express how helpfull all of your info has been so far on my quest to break down the relationship between spindle and automatic feed.

    Keep 'em coming !

    Cheers

  12. #12
    Member
    Join Date
    Aug 2019
    Posts
    18
    Quote Originally Posted by weibelmarco View Post
    Hello

    I have here a FANUC 16iM running a Daewoo 630 horizontal.
    I need to make a back-face with a tool that requires the spindle to be oriented and fed through the pilot hole.... but it wont.
    Of course i could dry-run it or use G00 and be super carefull on the potentios but that is fairly dangerous for some operators.

    Can anyone direct me to the parameter that would allow G01 movement with the spindle in M05 mode ?

    Any help is appreciated !
    I has same problem today, and i got figure it out by change the parameter 1402#0 (NPC) to 1.
    Hope it helps.

    Bagas

  13. #13
    Member
    Join Date
    Aug 2019
    Posts
    18
    Quote Originally Posted by weibelmarco View Post
    Hello

    I have here a FANUC 16iM running a Daewoo 630 horizontal.
    I need to make a back-face with a tool that requires the spindle to be oriented and fed through the pilot hole.... but it wont.
    Of course i could dry-run it or use G00 and be super carefull on the potentios but that is fairly dangerous for some operators.

    Can anyone direct me to the parameter that would allow G01 movement with the spindle in M05 mode ?

    Any help is appreciated !
    Maybe you should add G95 at first of the program, for change type of feeding into feed per minute. Feed per revolution requires spindle to rotate.

  14. #14
    Flies Fast
    Join Date
    Dec 2008
    Posts
    2840
    Quote Originally Posted by bagasajie55 View Post
    Maybe you should add G95 at first of the program, for change type of feeding into feed per minute. Feed per revolution requires spindle to rotate.
    Post is nearly 10 yrs old.... machine is probably replaced by now.

Similar Threads

  1. Replies: 0
    Last Post: 12-24-2013, 04:28 PM
  2. Spindle Stopping, Still have Motion
    By allennella in forum Tormach Personal CNC Mill
    Replies: 0
    Last Post: 04-16-2012, 11:00 PM
  3. mach3 spindle dro not working, spindle speed changing while jogging and running code
    By jasminder in forum Mach Software (ArtSoft software)
    Replies: 0
    Last Post: 02-23-2011, 07:12 AM
  4. spindle keeps running
    By Runner4404spd in forum Mach Mill
    Replies: 0
    Last Post: 05-01-2008, 04:25 AM
  5. Spindle not Running
    By Simon Lee in forum DIY CNC Router Table Machines
    Replies: 1
    Last Post: 02-09-2007, 06:56 PM

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
  •