Cross Peck Drilling Code Help

Nerdlinger · Aug 31, 2019

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 :willy_nilly:

) 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 :wall:

) 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!

Alberic · Sep 1, 2019

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

sinha · Sep 1, 2019

Nerdlinger said:
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.

Nerdlinger · Sep 1, 2019

Alberic said:
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!

Nerdlinger · Sep 1, 2019

sinha said:
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!

DouglasJRizzo · Sep 1, 2019

For cross hole peck drilling try G87.

TeachMePlease · Sep 2, 2019

Alberic said:
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.

sinha · Sep 2, 2019

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.

Nerdlinger · Sep 2, 2019

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!

sinha · Sep 3, 2019

Nerdlinger said:
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.

Rick Finsta · Sep 3, 2019

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.

sinha · Sep 3, 2019

Rick Finsta said:
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.

Nerdlinger · Sep 3, 2019

Rick Finsta said:
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????

Nerdlinger · Sep 3, 2019

sinha said:
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!

angelw · Sep 4, 2019

Nerdlinger said:
Thanks, Sinha! I just may!

Hello Nerdlinger,
Both G83 and G87 are covered in the Fanuc Lathe Operators Manual.

Regards,

Bill

sinha · Sep 4, 2019

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.

Nerdlinger · Sep 4, 2019

I imagine it's in there but I can't find it! :reading:

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... :willy_nilly:

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!

Search

Largest Manufacturing Technology Community on the Web

Search

Cross Peck Drilling Code Help

Nerdlinger

Stainless

Alberic

Cast Iron

sinha

Titanium

Nerdlinger

Stainless

Nerdlinger

Stainless

DouglasJRizzo

Titanium

TeachMePlease

Diamond

sinha

Titanium

Nerdlinger

Stainless

sinha

Titanium

Rick Finsta

Stainless

sinha

Titanium

Nerdlinger

Stainless

Nerdlinger

Stainless

angelw

Diamond

sinha

Titanium

Nerdlinger

Stainless

Similar threads