[MarkT]

I have never used this feature before on a lathe. I am trying in MDI with no success.
Machines = Daewoo Puma 2 & 3 axis lathes / mill turns
Control = Fanuc 16T circa mid 1990's

I would like to bring preset tooling offsets to the control via the program using the G10 command.
I have tried in MDI using the following syntax

G10 P1000016 X0. Z6.475;
(Insert Drill Geometry offset)

When I go to the geometry screen, nothing has been changed, I am thinking there is a parameter that needs to be changed to enable me to write to the geometry register.

Also, is the following accurate

G10 P16 U-.03 W.01;

The assumtion here is to write in offset backoffs for first piece runs.
That example would not be for the drill example, but for an I.D. Boring bar.

Any help would help, thanks!

Mark T.

[sinha_nsit]

Try G10 P10016 ...

The other G10 block would incrementally change wear offset values. It is ok.

[MarkT]

Tried - same result

Mark T.

[CNCRim]

I'm sure about your machine same the same way/not, you are miss L parameter, on the Fanuc G10 Lxx Pxx .

[Bluesman]

I have never used this feature before on a lathe. I am trying in MDI with no success.
Machines = Daewoo Puma 2 & 3 axis lathes / mill turns
Control = Fanuc 16T circa mid 1990's

I would like to bring preset tooling offsets to the control via the program using the G10 command.
I have tried in MDI using the following syntax

G10 P1000016 X0. Z6.475;
(Insert Drill Geometry offset)

When I go to the geometry screen, nothing has been changed, I am thinking there is a parameter that needs to be changed to enable me to write to the geometry register.

Also, is the following accurate

G10 P16 U-.03 W.01;

The assumtion here is to write in offset backoffs for first piece runs.
That example would not be for the drill example, but for an I.D. Boring bar.

Any help would help, thanks!

Mark T.

Do you have Custom Macro B availible ? if so you can load it directly to the system varible and bypass the G10 function. i use this for loading fixture offsets and the like and it save a tone of cycle time not having to wait for the G10. I can send you the list of system varibles for the 16T and a short manual on how to use them. This is how I load stuff from nest to nest

(PREP NEXT TOOL)
#10191=146.786
T#20
#549=#542
G91G0G43H191Z-[#10191](CALL OFFSET)
#1=[[#14421*.707]+[#14422*.707]]+#14741
#2=[[#14422*.707]-[#14421*.707]]+#14742
#3=#14423+#14743
#5221=[-796.267-#3](G54 X)
#5222=[-506.+#2](G54 Y)
#5223=[-832.225+#1](G54 Z)
#5224=0(G54 B)
G90G0G54X38.74Y0.Z500.B225.
M10
G4P#574
Z88.5
#760=16.
M54S#5
G84Z68.0(Z70.5)R88.5F#6
#760=0.
G80
G0Z400.

This saves tons of cycle time and can also help to lock in offsets you dnt want anyone to mess with

Bluesman

[sinha_nsit]

G10 is an option on some controls. Does it ever work on your machine?

No L-word is needed for geometry/wear offset values on a lathe.

[stevo1]

If the G10 function is not turned on in the control then it would alarm out with "Improper G-Code" alarm.

My guess is that if this alarm did not occur then you probably have the function active. Another way to try is to program G10L2P1X1. Then go look at G54 and see if it change X=1. If so then your G10 is working. Make sure you write down the current value of G54 before you run this that way you can put the proper number back into G54.

Mark....what is the P1000016 for??

Sinha...are you sure the L() is not needed? My notes show L10.

Try G10L10P16X0Z6.475

Stevo

Edit** G10 says geometry and G11 is wear.

[MarkT]

Custom macro b is installed and used on the machine. This is a 16T on a lathe. This is not to change the G54 work offset, but to load the distinct tool geometry & wear offsets on a lathe.
Peter Smid's Custom macro B book states that this is the way this can be accomplished on a lathe - It states the L address is not needed on a T series Fanuc, only needed on an M Series Fanuc.
I have tried various methods, no alarms are generated. I run parametric programs all the time, loop commands, and local variables.
The other method described was to write to the system variable for each offset ( Geometry "X" Geometry "Z" Geometry "Raduis" and Tip Type for one tool would be 4 system variables and they are all independant system varibales assigned to each field so I wanted to try to avoid that if possible.
Hopefully someone has successfully done this on a turning control, I use this on work offsets for milling controls all the time...works great.

Mark T.

[sinha_nsit]

If system variables are available, there is no need to use G10.

Yes, no L-word is needed on a lathe.
P16 refers to wear offset number 16, and P10016 refers to geometry offset number 16.

[MarkT]

The intent is to bring preset tooling geometry offsets into the control, via the program, to eliminate touching off for every job. Very high mix , low quantity operation. The advantage is 2 of the machines do have a good compliment of preset tooling.
We ahve discussed punching the offsets out with each job then loading them with each job, but if I can get the control to read the G10 command, it would embed the offsets within each program. Thats seams like a "cleaner" approach.
I will keep plugging at it!

Mark T.

[stevo1]

Just because you have macroB installed on the machine does not mean that G10 is. G10 is a separate option from Fanuc. Although I believe that you should have it because I have not seen a Fanuc not alarm out with Improper G-code when trying to use one that is not active.

I believe you that you may not need the L(). I was simply stating this because my T-series manual states the L10 and L11. Have you tired this at all?

As Sinha was stating you can use system variables to accomplish the same thing. G10 may seem cleaner but both ways will get the job done. You will just have to write it like so.

#2216=6.475(tool length)
#2016=0(set your wear)

Stevo

[Tom Ryan]

My shop also runs Daewoo Puma's (Fanuc 18T) and I do basically the same thing for drilling and tapping on a bolt circle, except I want to clear out any geometry that may have accidentally been left in. I do it with the following code:

G10P10003X0R0
Breakdown:
G10 = Data setting code
P100 = Parameter address
03 = 2-digit turret position (Tool #) that you want to write the geo. to
X0 = Inputs a value of 0 into the X geometry for the turret position specified
R0 = Inputs a value of 0 into the R geometry for the turret position specified
You would need to add a Z value since in my example I do not want to overwrite anything for Z.

If this doesn't work for you, than it is something with your control.Hope it helps (a year + later)

Tom