Cross Peck Drilling Code Help
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default Cross Peck Drilling Code Help

    Hey guys! My CAM software spat out a weak G01/G00 peck drilling cycle on my Tsugami B325 w/ Fanuc 32i control. I tried changing it to a G83 peck cycle and (it all happened so fast ) it looked like it just rapid-ed into the part, broke the drill, backed out, and carried on with the next tool path (of course the one time I don't carefully step through the program ) I am sure Morris Midwest will hook me up with the answer but I cannot sleep until I figure this out and won't get back in until Tuesday. I searched both the Fanuc and Tsugami pdf manuals for "G83" and "peck" and found NOTHING! Here's the code and [what I think it means]

    M23 S2203 P2 G00 Z3.718 T0101; [cross live tool on, 2203 RPMS, Motor #2, rapid to Z3.718, tool 1 offset 1]
    X0.7503; [rapid to X.7503 - part is previously turned to .690" diameter]
    M312; [spindle speed arrival confirmation]
    G98 G83 X-.8035 Q5000 R.750 F3.3; [Initial X retract, peck drilling cycle, target depth of X-.8035, .050" peck depth, retract plane of X.750, 3.3ipm]
    G80 [cancel canned cycle]
    M25; [cross live tool stop]
    G00 X5.4331 W0.0 T0: [rapid to X5.4332 in T0 - this will center the cross slide]

    The G98 line is the only thing I ADDED after removing a bunch of G01's and G00's so I imagine the problem is in there. Does anyone know what in tarnation I am doing wrong there? Does G83 maybe default to IPR? There's another G98 a few lines up so even though I think the one on the G83 line is activating initial X point retract we should still be in IPR mode from a few lines before the code I shared.

    Thank you for your help!

  2. #2
    Join Date
    Jan 2011
    Location
    SF Bay
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    209

    Default

    Greetings,

    I'm running a Ganesh, which runs on a Mitsubishi control, so it's slightly different.
    But...
    (This is all in "A" mode G code.)
    Live cross tool peck drilling for *us* is G87. That may be part of it. The other kinky part is that the R plane isn't.
    It's distance from wherever you parked the tool in the last move.
    So for your code, if this was my machine, your tool would park at x0.7503, and then rapid in .750". Not rapid in *to* .750, but actually move in .375". (.750/2) Which nearly blew up a whole bunch of my drills until I figured it out. (The Ganesh (and most swiss-like machines) have a really handy 'handwheel' walk-thru mode, where they only move while you're cranking the handwheel. You stop, they stop. You back up, so do they. *Incredibly* handy, that.)

    Just for testing, try setting your first park location way up in the air, and then set the "R" to about .250. (with nothing in the spindle, and the rapids down to zero.) See what it does. I bet it only moves down just the least little bit from wherever you parked it.

    Hope this helps.
    -Brian

  3. Likes TeachMePlease liked this post
  4. #3
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quote Originally Posted by Nerdlinger View Post
    Hey guys! My CAM software spat out a weak G01/G00 peck drilling cycle on my Tsugami B325 w/ Fanuc 32i control. I tried changing it to a G83 peck cycle and (it all happened so fast ) it looked like it just rapid-ed into the part, broke the drill, backed out, and carried on with the next tool path (of course the one time I don't carefully step through the program ) I am sure Morris Midwest will hook me up with the answer but I cannot sleep until I figure this out and won't get back in until Tuesday. I searched both the Fanuc and Tsugami pdf manuals for "G83" and "peck" and found NOTHING! Here's the code and [what I think it means]

    M23 S2203 P2 G00 Z3.718 T0101; [cross live tool on, 2203 RPMS, Motor #2, rapid to Z3.718, tool 1 offset 1]
    X0.7503; [rapid to X.7503 - part is previously turned to .690" diameter]
    M312; [spindle speed arrival confirmation]
    G98 G83 X-.8035 Q5000 R.750 F3.3; [Initial X retract, peck drilling cycle, target depth of X-.8035, .050" peck depth, retract plane of X.750, 3.3ipm]
    G80 [cancel canned cycle]
    M25; [cross live tool stop]
    G00 X5.4331 W0.0 T0: [rapid to X5.4332 in T0 - this will center the cross slide]

    The G98 line is the only thing I ADDED after removing a bunch of G01's and G00's so I imagine the problem is in there. Does anyone know what in tarnation I am doing wrong there? Does G83 maybe default to IPR? There's another G98 a few lines up so even though I think the one on the G83 line is activating initial X point retract we should still be in IPR mode from a few lines before the code I shared.

    Thank you for your help!
    Are you using g-code system A, B or C ?
    Are you in absolute or incremental mode ?
    G83 is for front drilling and G87 is for side drilling.

  5. #4
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    Quote Originally Posted by Alberic View Post
    Greetings,

    I'm running a Ganesh, which runs on a Mitsubishi control, so it's slightly different.
    But...
    (This is all in "A" mode G code.)
    Live cross tool peck drilling for *us* is G87. That may be part of it. The other kinky part is that the R plane isn't.
    It's distance from wherever you parked the tool in the last move.
    So for your code, if this was my machine, your tool would park at x0.7503, and then rapid in .750". Not rapid in *to* .750, but actually move in .375". (.750/2) Which nearly blew up a whole bunch of my drills until I figured it out. (The Ganesh (and most swiss-like machines) have a really handy 'handwheel' walk-thru mode, where they only move while you're cranking the handwheel. You stop, they stop. You back up, so do they. *Incredibly* handy, that.)

    Just for testing, try setting your first park location way up in the air, and then set the "R" to about .250. (with nothing in the spindle, and the rapids down to zero.) See what it does. I bet it only moves down just the least little bit from wherever you parked it.

    Hope this helps.
    -Brian
    Thanks, Brian. I’ll try changing to G87 and then watch the POS screen carefully to see how each block behaves while clicking through the program. I ALWAYS handwheel through while watching the “distance to go”.....except for this one time haha!

  6. #5
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    Quote Originally Posted by sinha View Post
    Are you using g-code system A, B or C ?
    Are you in absolute or incremental mode ?
    G83 is for front drilling and G87 is for side drilling.
    Hi Sinha,

    I am not familiar with the various G-code systems that both you and Brian referenced. The machine is only a few months old, if newness has anything to do with it....

    Brian mentioned the same thing about G87 so I’ll fool around with that if Tsugami tech doesn’t get back to me first.

    Thank you!

  7. #6
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    489
    Likes (Received)
    318

    Default

    For cross hole peck drilling try G87.

  8. #7
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,685
    Post Thanks / Like
    Likes (Given)
    10297
    Likes (Received)
    3114

    Default

    Quote Originally Posted by Alberic View Post
    Greetings,

    I'm running a Ganesh, which runs on a Mitsubishi control, so it's slightly different.
    But...
    (This is all in "A" mode G code.)
    Live cross tool peck drilling for *us* is G87. That may be part of it. The other kinky part is that the R plane isn't.
    It's distance from wherever you parked the tool in the last move.
    So for your code, if this was my machine, your tool would park at x0.7503, and then rapid in .750". Not rapid in *to* .750, but actually move in .375". (.750/2) Which nearly blew up a whole bunch of my drills until I figured it out. (The Ganesh (and most swiss-like machines) have a really handy 'handwheel' walk-thru mode, where they only move while you're cranking the handwheel. You stop, they stop. You back up, so do they. *Incredibly* handy, that.)

    Just for testing, try setting your first park location way up in the air, and then set the "R" to about .250. (with nothing in the spindle, and the rapids down to zero.) See what it does. I bet it only moves down just the least little bit from wherever you parked it.

    Hope this helps.
    -Brian
    For reference, my Mitsubishi controlled Citizens behave exactly Brian has described with regard to both needing to use G87 for cross peck drilling, and the R argument, it is NOT retract plane, it is the incremental amount (diametral) to rapid FROM the starting position TOWARD the work piece.

  9. #8
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quite a few things are parameter dependent. The following information is for Fanuc ...

    Position of R-point
    In G-code system B and C, depending on certain parameter settings, R would either always be
    incremental distance from the initial level (irrespective of G90/G91), or it can be either absolute
    coordinate or incremental distance from the initial level (depending on G90 and G91, respectively). In
    system A, which we are following, this is again parameter dependent; it can be either absolute
    coordinate or incremental distance from the initial level. Since parameter settings are going to vary on
    different machines, the best way would be to execute a program on the machine, in a safe working
    zone, to find out whether R is absolute or incremental. Another way would be to set the parameter
    5102#6 to 0, which would force R to always be the incremental distance from initial level, in all the
    three G-code systems. The incremental distance would always be negative in this case.

    Another issue regarding its value, in side drilling (in front drilling, it is always the actual distance),
    is that whether it would be a diameter value (in diameter programming) or a radius value (even in
    diameter programming), depending on parameters. Therefore, either conduct an experiment on the
    machine to find out what it is, or set parameter 5102#7 to 0 which would always force it to be a radius
    value.

  10. Likes TeachMePlease liked this post
  11. #9
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    You guys are all totally right! I haven’t been able to get back to the machine yet (I will tomorrow) but the Tsugami tech got back to me over the weekend (impressive!) and said exactly what you all did : G87 for side drilling, R is distance from initial point to the retract plane....so watch out for that one! :^)

    I still wish that would have been in one of the manuals! Maybe I missed it...

    Thanks again!

  12. #10
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quote Originally Posted by Nerdlinger View Post
    I still wish that would have been in one of the manuals! Maybe I missed it...
    You may like to have a look at this.
    The information I gave was copied from this only. There is a lot more to read.

  13. #11
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    546
    Post Thanks / Like
    Likes (Given)
    57
    Likes (Received)
    272

    Default

    If it makes you feel better, I learned that only because the Abile software spit out G87s LOL. Otherwise I definitely would have crash a drill or two learning.

  14. Likes Nerdlinger liked this post
  15. #12
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quote Originally Posted by Rick Finsta View Post
    If it makes you feel better, I learned that only because the Abile software spit out G87s LOL. Otherwise I definitely would have crash a drill or two learning.
    Depending too much on a CAM software can be dangerous. All machines are slightly different because of parameter settings. A perfect post-processor is a myth. Sufficient knowledge of manual part programming is desirable.
    Generally, CAM is not needed on a 2-axis lathe.

  16. #13
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    Quote Originally Posted by Rick Finsta View Post
    If it makes you feel better, I learned that only because the Abile software spit out G87s LOL. Otherwise I definitely would have crash a drill or two learning.
    Hmmmm, for me Abile spat out a bunch of G01’s...some at the feed rate and some at a near-rapid feed rate as a pseudo peck drill tool path. How do you get it to actually use the G87????

  17. #14
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    Quote Originally Posted by sinha View Post
    You may like to have a look at this.
    The information I gave was copied from this only. There is a lot more to read.
    Thanks, Sinha! I just may!

  18. #15
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by Nerdlinger View Post
    Thanks, Sinha! I just may!
    Hello Nerdlinger,
    Both G83 and G87 are covered in the Fanuc Lathe Operators Manual.

    Regards,

    Bill

  19. #16
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    The Operator's Manual does cover G83 and G87, but it will have to be read in association with the parameter manual for complete information. For example, the manual says that R is always incremental and a radius value. But, this is parameter dependent.

  20. #17
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    I imagine it's in there but I can't find it! I looked in the table of contents, the index, and even searching (it's a pdf) "G87", "G83", and "peck" with no results. (G01 was found on 195 pages). The G-Code list on page 25 goes G76, G77, G84, G85, G90, G91... This is the Fanuc 32i Operators Manual...

    UPDATE - for some reason the manual they gave me has a file name of "32i" but the title page when I actually open it says "30i + 31i" so I found the 32i manual on-line and I see the G87 listed in the G-Code list page but can't find where it actually describes how to use it, what the different variables are, programming examples, etc. I must be missing something. Oh well...it's working now!


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
  •