584,842 active members*
4,098 visitors online*
Register for free
Login
Results 1 to 13 of 13
  1. #1

    G76 Thread help

    Attempting to turn 5/16-18 Threads on 4140 Material. L20 Citizen Mitsubishi Controls
    Turn down .312(.030 chamfer 45 degree), and Grooving clearance (Groove to .242) past the threads. I am using an Iscar 16ER18 turning insert, with a right hand holder that is at a 10 degree

    Using the code below, I consistently get threads that fit in the go gage for pitch, not in the no go for pitch, but the back side appears to have what looks like nicks, and the first thread appears damaged.
    Unsure how to control retract as wondering if machine is not retracting far enough to clear the part.

    G96S700

    G0X.355 Z-.225

    G76 P020030 Q0005 R0005

    G76 X.2405 Z.16 P0350 Q0010 R0 F.055


    Any advice would be greatly appreciated.

  2. #2
    Join Date
    Jun 2015
    Posts
    4131

    Re: G76 Thread help

    hy osub i have worked with citizen cincom l12 with mithusbishi cnc, mass-production, setups > 2 months

    i like to program the depth of each pass, like this :
    Code:
    T0505 G99
    M3 S1=3000
    G0  X13                    Z-1
    G92 X5-0.28                Z3.5 F0.5
        X5-0.28-0.24
        X5-0.28-0.24-0.16
        X5-0.28-0.24-0.16-0.08
        X5-0.28-0.24-0.16-0.08
        X5-0.28-0.24-0.16-0.08
    G0  X13
    T00
    M5
    last 2 passes are spring passes, thus they don't cut material, but only make the thread look better

    Unsure how to control retract as wondering if machine is not retracting far enough to clear the part
    in previous code, retraction occurs at X13

    also, is good to be able to detect the retracting diameter, without looking inside the code

    please take a look over attached image : i have never used that code, by i only shared it, so to show you that i could find informations pretty fast, like in 60 seconds

    if you wish for cnc manuals, please share an e-mail in private message; archive is about 32mb

    Using the code below, I consistently get threads that fit in the go gage for pitch, not in the no go for pitch, but the back side appears to have what looks like nicks, and the first thread appears damaged.
    this is a classical problem thus you have ok from the go&no-go calibers, but the thread does not look ok

    there are methods to improve the aspect, for frontal chamfer, back chamfer, and in-between

    [ frontal-chamfer, back-chamfer ] : after the threading operation, re-cut only the chamfer, by going down, towards X-; if you wish to improve the aestetich even more, try using a double chamfer, like merging a 45degrees with a 30degrees
    [in-between] : also the entire thread aspect can be improved, and the method involves spring-passes, and sometimes also re-cutting the od; what do to depends, if there is used a full-profile-insert, or a partial-type

    also, if needed, i program custom infeed patterns

    i hope you find this useful / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  3. #3

    Re: G76 Thread help

    I appreciate the info, but I'm still trying to figure out why my G76 isn't working. It should work in theory. By cosmetic, I mean that it appears I am not retracting enough, as a section of the beginning thread is missing, and the back side on everycthread is gouged (not at same position but multiple positions), making me believe the tool is dragging into it during the retract pass.

    Quote Originally Posted by deadlykitten View Post
    hy osub i have worked with citizen cincom l12 with mithusbishi cnc, mass-production, setups > 2 months

    i like to program the depth of each pass, like this :
    Code:
    T0505 G99
    M3 S1=3000
    G0  X13                    Z-1
    G92 X5-0.28                Z3.5 F0.5
        X5-0.28-0.24
        X5-0.28-0.24-0.16
        X5-0.28-0.24-0.16-0.08
        X5-0.28-0.24-0.16-0.08
        X5-0.28-0.24-0.16-0.08
    G0  X13
    T00
    M5
    last 2 passes are spring passes, thus they don't cut material, but only make the thread look better



    in previous code, retraction occurs at X13

    also, is good to be able to detect the retracting diameter, without looking inside the code

    please take a look over attached image : i have never used that code, by i only shared it, so to show you that i could find informations pretty fast, like in 60 seconds

    if you wish for cnc manuals, please share an e-mail in private message; archive is about 32mb



    this is a classical problem thus you have ok from the go&no-go calibers, but the thread does not look ok

    there are methods to improve the aspect, for frontal chamfer, back chamfer, and in-between

    [ frontal-chamfer, back-chamfer ] : after the threading operation, re-cut only the chamfer, by going down, towards X-; if you wish to improve the aestetich even more, try using a double chamfer, like merging a 45degrees with a 30degrees
    [in-between] : also the entire thread aspect can be improved, and the method involves spring-passes, and sometimes also re-cutting the od; what do to depends, if there is used a full-profile-insert, or a partial-type

    also, if needed, i program custom infeed patterns

    i hope you find this useful / kindly

  4. #4
    Join Date
    Jun 2015
    Posts
    4131

    Re: G76 Thread help

    hy, when i started to write programs for the citizen, i was not used with the g76-syntax, thus i was only somehow aware that fanuc has a threading syntax that requires 2 lines of code

    i was used with using a single line syntax, or with controlling the depth of each cut

    now, back to you :
    ... replace "G0X.355 Z-.225" with a bigger X value, thus increase radial clearance
    ... test lower rpms, because at high rpms, the cnc motion is not as stable as when using low rpms, especially when threading
    ... run 1 pass, stop and inspect, run 2nd pass, stop and inspect, and so on; it may be possible to observe that the tool is dragging after 3rd pass

    i have tested many threads, especially when threading with very low clearances, like between shoulders(?!), or inside tight holes

    sometimes, i reduce the rapid speed, so to avoid the dragging effect

    i hope this helps / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  5. #5
    Join Date
    Aug 2009
    Posts
    1567

    Re: G76 Thread help

    ...would G08 or G09 ramping mode affect threading?

  6. #6
    Join Date
    Feb 2011
    Posts
    353

    Re: G76 Thread help

    G96S700

    G0X.355 Z-.225

    G76 P020030 Q0005 R0005

    G76 X.2405 Z.16 P0350 Q0010 R0 F.055


    first thing i would do is remove the g96 s700 as this is csfm and will cause the machine to ramp up and down as it is machining causing different starts as it picks up the point on the spindle to start
    is this machine a sub micron machine or non sub micro machine ?
    if it is a sub micron machine you would need an extra 0 either before or after the number IE 00050 would equal .0005 on a sub micron
    the mitsubishi control i work on you can use the decimal point for the Q,R,P values
    and last thing is if it still isn't working try doing P020060 some times the 60 degrees works good and F.0556

  7. #7
    Join Date
    Dec 2008
    Posts
    3110

    Re: G76 Thread help

    I agree... G97 instead of G96
    M3/M4 missing
    Z-.225 going to Z.16 ( so starting in groove cutting away from chuck.... not allowing any chance to get to correct feed before actually cutting ... P & Q addresses cant have decimal point
    Pxxyyzz
    xx= number of finish passes
    yy= thread ending 00=instant retract
    zz= infeed angle (varies between manufaturers, usually only fixed #s can be used.... I use 29 on 60° vee, so tip flank cleans up a little on each instep, zero is a straight infeed pattern) (60 may not work, so check manual)
    Q0005 is amount to leave for finishing passes
    R0005 is clearance (G76Xvalue plus 2 depths plus this value)... check this out.)
    G76Q0010 is depth of 1st pass.... can be larger

  8. #8
    Join Date
    Jun 2015
    Posts
    4131

    Re: G76 Thread help

    hy guys you are right, g96 should not be there

    i did not looked carefull over the code, i suposed that code syntax is correct, and even if the code is simple, i did not exactly remembered if 96 is ccs also on citizen; there are a few differences between g-codes, at least when compared to okuma ( for example 94 95 vs 98 99 )

    but the control itself should have generated an alarm, because 96 and 76 should not be compatible

    ...would G08 or G09 ramping mode affect threading?
    please, what do you mean by those ? i did not find them inside the citizen manuals / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  9. #9
    Join Date
    Aug 2004
    Posts
    780

    Re: G76 Thread help

    #5 and #6 are great ideas.

    Yet, it seems You are tearing threads on 1 side, only.
    Ramp mode per #5 might affect this, depending on your control.

    The clearance value might affect this.
    R parameter I think.
    Try R at 30x higher.

    Also, run a cycle at S1, aka spindle 1 rpm.
    See what happens.
    Put sharpie on a blank, and see where the error actually occurs after just 1 pass.

    Also, call your local mtb / reseller.
    They are usually extremely good at these types of things, and will tell you exactly what to do, why, and how, free.

    This is what I / we did when I was the commercial manager at Haas Spain.
    (long post deleted)

  10. #10
    Join Date
    Jun 2015
    Posts
    4131

    Re: G76 Thread help

    is possible that the cnc won't be able to handle s1; there may be a minimal rpm required, otherwise the cnc will stop, because it won't receive the confirmation signal

    ... on okuma lathes, the minimum accepted rpm is arround 20
    ... on citizen equiped with bar feeders, there is a parametet for this value, so to keep the spindle turning, when bar feeding occurs, in order to avoid scratching the guide bushing; if this parameter is lowered, then the machine will stop
    * i like to refer to this minimal rpm as dead-slow

    to speed up in machine checks, i use to open the door during cutting, stop the cutting fluid, and run in single block

    single block may be tricky if a 2nd spindle is used, so i use a custom test programs, that executes only the faulty operation / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  11. #11

    Re: G76 Thread help

    Quote Originally Posted by Superman View Post
    I agree... G97 instead of G96
    M3/M4 missing
    Z-.225 going to Z.16 ( so starting in groove cutting away from chuck.... not allowing any chance to get to correct feed before actually cutting ... P & Q addresses cant have decimal point
    Pxxyyzz
    xx= number of finish passes
    yy= thread ending 00=instant retract
    zz= infeed angle (varies between manufaturers, usually only fixed #s can be used.... I use 29 on 60° vee, so tip flank cleans up a little on each instep, zero is a straight infeed pattern) (60 may not work, so check manual)
    Q0005 is amount to leave for finishing passes
    R0005 is clearance (G76Xvalue plus 2 depths plus this value)... check this out.)
    G76Q0010 is depth of 1st pass.... can be larger
    Z 0 is faced off, so by starting at -.225 I am starting in space, then feeding stock into the cut for .160 distance.
    Confused when you say not having chance to correct feed, when should be making at least four complete thread revs before reaching part

  12. #12
    Join Date
    Jun 2015
    Posts
    4131

    Re: G76 Thread help

    Confused when you say
    hy osub, i believe that superman was reffering to the fact that your clearance may be too low ?!

    0.225inch = 5.715mm
    0.055inch = 1.397mm

    when should be making at least four complete thread revs before reaching part
    5.715/1.397=4.09 theoretical revs before reaching the part

    well, math is math, but this does not mean that you reach the required feed before begining to cut

    those 4.09 are theoretical revs, and you should take into consideration the distance required for the linear axis to get up to speed

    it is possible to have a thread that is ok at the go & no-go gauges, even if the machine reached the desired feed after z0

    inside okuma manuals are shared examples how to calculate the distance required to accelerate an axis

    in most cases this does not matter, unless you are threading with high specs, and low clearances / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  13. #13
    Join Date
    Dec 2008
    Posts
    3110
    Quote Originally Posted by deadlykitten View Post
    hy osub, i believe that superman was reffering to the fact that your clearance may be too low ?!
    Bugger off kitty.... that is not what I meant
    .. I pictured part in spindle on left with origin at R/H face
    moving tool further left is Z- dir

    I have always followed the rule that you program the tool to move..... even if it is the part that does the actual movement.

Similar Threads

  1. Help : Wrong Thread is cutting for Internal Metric Thread
    By dolarpond in forum G-Code Programing
    Replies: 0
    Last Post: 06-02-2017, 04:51 PM
  2. Help : Wrong Thread is cutting for Internal Metric Thread
    By dolarpond in forum Chinese Machines
    Replies: 0
    Last Post: 06-02-2017, 08:01 AM
  3. Thread spec for camera lens filter thread
    By cmays in forum MetalWork Discussion
    Replies: 6
    Last Post: 07-20-2016, 10:43 AM
  4. Thread Mill Wizard - Slanted thread produced
    By ngr1 in forum Mach Wizards, Macros, & Addons
    Replies: 5
    Last Post: 07-22-2012, 07:23 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
  •