584,861 active members*
5,092 visitors online*
Register for free
Login
Results 1 to 15 of 15
  1. #1
    Join Date
    Mar 2006
    Posts
    255

    Lightbulb C Axis Turning

    Hello
    Does anyone have a sample bit of code with I can check a C axis on my machine. This is Fanuc 18T controlled and when I purchased it, I was informed it had C axis control. It also came with some live tooling.

    So the kind of thing I want to test is turning the axis to certain degree points and also being able to turn the spindle while lets say using an end mill on the live tooling.

    Any sort of code will do, I'm just having trouble actually turning the spindle with B/C coding, which I have seen done on the machine before I bought it.

    pinguS

  2. #2
    Join Date
    Aug 2006
    Posts
    98
    Man, what's problem do you have using B/C code ??? What's happen ??? You check is the degrees in the parameters are correct ??? PRM 4963 ??? Chech these PRM's !!! If has problems using M codes, i send to you how configure the parameters to make an position from spindle (C axis) !!!

    Daniel

  3. #3
    Join Date
    Jan 2006
    Posts
    4396

    Arrow C Axis Programming

    Quote Originally Posted by pinguS
    Hello
    Does anyone have a sample bit of code with I can check a C axis on my machine. This is Fanuc 18T controlled and when I purchased it, I was informed it had C axis control. It also came with some live tooling.

    So the kind of thing I want to test is turning the axis to certain degree points and also being able to turn the spindle while lets say using an end mill on the live tooling.

    Any sort of code will do, I'm just having trouble actually turning the spindle with B/C coding, which I have seen done on the machine before I bought it.

    pinguS
    Fanuc has a few ways of programming for a "C" axis. More than likely there is a specific "M" code to Lock an Unlock the spindle before and after Indexing. M70 Sets Indexing Mode M71 Resets spindle for regular use, M100000 range in .0001 of a degree indexing (ex. M10900=90 degrees), and M113 Live Tool CW Rotation, M114 CCW Rotation, M115 Stop. These may not be for your machine, but are used on a Tsugami Swiss.

    One question is your "C" Axis in the Main Spindle or a Sub-Spindle?

    Here is an example of the Tsugami Program that has 90 degree Slots

    %
    O4130
    (SEAT BALL SOCKET REV.5)
    M8
    S1000 M3
    G0 G40 G99 Y1.5 T0 M11
    G110 T0
    G100 C6.6>>> C Axis here is the Sub-Spindle like a Z Axis Stroke(Home Position)
    G300 Z1.5
    M10
    G50 Z-.01
    G0 X1.5 Z-.03 T0 M18
    M1

    N1(FACE)
    T505 S6500 M13
    G0 X.4 Z0
    G1 X-.008 F.001
    G0 X.4 Z-.01
    X1.5 T0

    N2(SPOT DRILL 3/8 DIA.HSS)
    T1111 S1500 M13
    G0 Z-.02
    Y0
    G1 W.15 F.0008
    G4 U1.0
    G0 Z-.05
    Y1.5 T0

    N3(DRILL 1/8 DIA. 135SPT COB STUB)
    T1212 S1500 M13
    G0 Z-.02
    Y0
    G1 Z.336 F.0015
    G4 U.05
    G0 Z-.05
    Y1.5 T0

    N4(BORE .11 DIA. TRUE MADE COATED)
    (.004 TNR HONED FOR FINISH SF)
    T1313 S2000 M13
    G0 Y.6 Z-.05
    G1 Y.339 Z-.015 F.005
    Y.127 Z.091 F.00025
    Z.285 F.0005
    Y.125
    G0 Z-.05
    Y1.5 T0

    N5(FACE/TURN)
    T051505 S6500 M13
    G0 X.4 Z0
    G1 X.275 F.0008
    X.3285 F.0015
    X.3385 Z.005 F.0003
    U-.0004 Z.425 F.0005
    X.35 Z.4462 F.0003
    G0 X1.5 T0

    N6(R-GROOVE .058W THINBIT)
    T140614 S2000 M13
    G0 Y.4 Z.3142
    G1 Y.24 F.0005
    Y.349 F.01
    G0 Z.308
    G1 Y.24 F.0005
    Y.349 F.01
    G0 Z.32
    G1 Y.24 F.0005
    Y.35 F.01
    G0 Y1.5 T0

    N7(F-GROOVE .069W ROBINSON)
    T150615 S6000 M14
    G0 Y.349 Z.304
    G4 U.05
    G1Y.329 Z.314 F.0003
    Y.219
    Z.325
    Y.329
    Y.349 Z.335 F.0003
    G0 Y1.5 T0 M5

    /N8(SLOT SAW 1.25 DIA. .02 WIDE 36T)
    /(OFFSET LIVE TOOL POST .25 W/PLATE)
    /T011501 M8
    /G50 A0
    /A.9
    /M70>>>SETS MAIN SPINDLE TO LOCK AFTER AND UNLOCK BEFORE INDEXING
    /M117 (750 RPM)
    /M114 (CCW)
    /M10000 (0 DEGREES)
    /G0 X.75 Z-.05
    /X0
    /G98 G1 Z.26 F15.0
    /G4 U.05
    /G1 A-.4 F3.5
    /Z-.05 F25.0
    /M10900 (90 DEGREES)
    /G0 A.8
    /G1 Z.26 F15.0
    /G4 U.05
    /G1 A-.4 F3.5
    /Z-.05 F25.0
    /G99 X.75 M115
    G0 X1.5 T0 M71>>>>>>RESETS FOR REGULAR SPINDLE USE

    N12(CUT-OFF .06 WIDE)
    T061506 S3500 M13
    G0 Z.4
    X.4
    G1 X.2 F.0005
    X.349 F.003
    Z.39
    X.329 Z.4 F.0003
    X-.035 M17
    M18
    M95
    /M98 P9800
    M96
    M97
    M30
    %
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  4. #4
    Join Date
    Mar 2006
    Posts
    167
    The M codes used to activate C-axis control will vary depending on the machine manufacturer. The machines we sell use M67 (C On) and M66 (C Off), and Position is controlled using a simple C angle (eg. C135 = 135deg. ).

    regards, Oz

  5. #5
    Join Date
    Jan 2006
    Posts
    4396
    I've seen that configuration as well as "A" used for programming index points on a Lathe
    Fanuc Controls are all built around the Machine Tool Builder so it makes it very difficult to pinpoint which way to program for his. Maybe he could ask for a program from the previous owner? This would tell a lot about how it should be programmed.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  6. #6
    Join Date
    Mar 2006
    Posts
    255
    Ok
    But say you want to lets say write a letter around a bar. From what I understand the C axis is full C axis, so that is can rotate while machining, would this be done using the code above?

    pinguS

  7. #7
    Join Date
    Mar 2006
    Posts
    255
    Also the C axis is the main spindle, there is no sub spindle.

  8. #8
    Join Date
    Jan 2006
    Posts
    4396
    Quote Originally Posted by pinguS
    Ok
    But say you want to lets say write a letter around a bar. From what I understand the C axis is full C axis, so that is can rotate while machining, would this be done using the code above?

    pinguS
    No, what I have written above is a slot through a part Perpindicular to the Diameter. For what you want I invision a Z and a C axis movement with a live tool (Engraving Tool or End Mill) with an X Axis depth of cut.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  9. #9
    Join Date
    Jan 2006
    Posts
    4396
    This is the part for the program above.
    Attached Thumbnails Attached Thumbnails seatball 1.JPG   seatball 2.JPG   seatball 3.JPG  
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  10. #10
    Join Date
    May 2006
    Posts
    265
    Quote Originally Posted by pinguS
    Ok
    But say you want to lets say write a letter around a bar. From what I understand the C axis is full C axis, so that is can rotate while machining, would this be done using the code above?

    pinguS

    You can use the G107 cycle or just output all the c and z coordinates to make the letters... I can check the manual how the g107 cycle works at work tomorrow.
    Attached Thumbnails Attached Thumbnails SUC50178.JPG  

  11. #11
    Join Date
    Mar 2006
    Posts
    255
    Some good information there, I will try all this stuff once I get a chance to go back onto the machine. Probably in 2 weeks.

    Although I have got manual, I will look for G107 in there, can't say I have ever seen it, or probably was looking in the wrong manual!!

  12. #12
    Join Date
    Jan 2006
    Posts
    4396
    Quote Originally Posted by pinguS
    Some good information there, I will try all this stuff once I get a chance to go back onto the machine. Probably in 2 weeks.

    Although I have got manual, I will look for G107 in there, can't say I have ever seen it, or probably was looking in the wrong manual!!
    It could be any number of G-Codes

    G121
    G120
    G300
    G301
    G201
    G202

    There is a long list. Honestly it all depends on the machine tool builder, as they all want different options and configurations.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  13. #13
    Join Date
    Dec 2004
    Posts
    524
    Quote Originally Posted by tobyaxis View Post
    Fanuc has a few ways of programming for a "C" axis. More than likely there is a specific "M" code to Lock an Unlock the spindle before and after Indexing. M70 Sets Indexing Mode M71 Resets spindle for regular use, M100000 range in .0001 of a degree indexing (ex. M10900=90 degrees), and M113 Live Tool CW Rotation, M114 CCW Rotation, M115 Stop. These may not be for your machine, but are used on a Tsugami Swiss.

    One question is your "C" Axis in the Main Spindle or a Sub-Spindle?

    Here is an example of the Tsugami Program that has 90 degree Slots

    ...much has been deleted...
    %
    Toby,

    I'm in the thinking stages now of doing a lathe CNC conversion. Do you happen to know how the C axis spindle control is implemented on a lathe? How do they get .0001 degree resolution? Is the spindle motor actually a servo with some type of very high resolution encoder? Any info you can provide would be appreciated.

    Ken
    Kenneth Lerman
    55 Main Street
    Newtown, CT 06470

  14. #14
    Join Date
    Jan 2006
    Posts
    4396
    Quote Originally Posted by lerman View Post
    Toby,

    I'm in the thinking stages now of doing a lathe CNC conversion. Do you happen to know how the C axis spindle control is implemented on a lathe? How do they get .0001 degree resolution? Is the spindle motor actually a servo with some type of very high resolution encoder? Any info you can provide would be appreciated.

    Ken
    I really don't know but AL the Man might. Start a new Thread calling for AL_the_Man. If anyone can help you he can. You can also send him a PM.

    Sorry I couldn't help
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com

  15. #15
    Join Date
    Dec 2003
    Posts
    24216
    Ken, There are two typical ways that it is done, for an all featured spindle, i.e. CSF, Threading and Caxis,
    All Require an encoder on the final spindle shaft.
    Many systems use a regular spindle controller, that is fairly closely controlled by means of either an encoder also on the motor or a pulse generator of some kind.
    This allows close control of spindle rpm when CSF and when threading, the encoder on the final shaft uses the marker pulse to synchronize the Z axis to enable the correct point for the tool to enter the thread. The Z axis then follows according to spindle rpm.
    For C axis control, often this spindle is not precise enough, unless it is an actual servo construction, but for large spindles 5~10hp and up, this is often impracticle, so what is done is that a smaller servo motor is used to position the spindle shaft (C axis) when live tooling is used etc.
    If the servo is lower Hp/Torque, then it can often be achieved with one Servo type spindle motor.
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

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

Posting Permissions

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