[san]

Could anybody explain FANUC G75 canned grooving cycle with example.
Thanks

[Hursty]

The attached page from my book should help.

[jackson]

depending on the year of the control it could be a two line read of a one, also i think one the new controls you can use either you have to change a pram.

Say your part is 1.5 od and your using a .125 groove and you want to groove 1" past Z0

G0G54T101
G50S2000
G96S600M3
X1.6Z-1.125M8(X.100 over the part Z is groove location)
G75R.025(R is how much tool will retract after each cut)
G75X.875Q200F.006(X is the diam. of groove Q is amount per cut)
G0X1.6
Z3.M9
M1

So it will take .02 per cut till reaching .875 will retract .025 to break chips
hope this helps

[san]

Hursty,
jackson,

Thanks for the solution. I will try and let you guys know about the result.

[joecnc1234]

G00T0900
G96S250M3
G0X5.45Z1.T909M8
Z-.325 (start position for grooving)
G75F.005X4.1Z-1.94I250K1000 (x value is final dia. z value is final z wall. I value is amount of peck. k value is step over amount in z.)
I hope this helps this is for fanuc 11t)

[joecnc1234]

On my machine the retract amount is set by a parmeter.

[san]

Thank you all. MY cnc is Oi Mate-TC.
I tried with above all got error but jackson format works. May be the Jackson fromat is compatible to my cnc.
G75 R0.
G75X43.5Z-37.95Q2600P500R0.5F0.1
G0Z2.
and it works.
thank you all . You all make me try and now i know something about it.

[harshal]

click here CNC PROGRAMMING TUTORIAL
FANUC G75 CANNED CYCLE GROOVING CNC PROGRAM WITH DESCRIPTION
July 19, 2018
In this program we only perform fanuc grooving G75 cycle for cnc lathe operation

01451
N10 G90 G21 G99 F0.15 ;
N20 G50 S1500 ;
N30 M06 T01 01 ;
N40 M03 G96 S300 ;
N50 G00 X52 Z-10 ;
N60 G75 R1 ;
N70 G75 X30 Z-30 P3000 Q20000 ; CNC PROGRAMMING TUTORIAL
N80 G00 X60 ;
N90 G28 U0 W0 ;
N100 M05 M30 ;

DESCRIPTION OF MAIN PROGRAM :-
01451 - Name of main program
N10- Absolute co-ordinate system , metric input in mm , feed rate per revolution , feed is 0.15
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Tool change command , select tool no. 1
N40- Spindle ON clockwise , constant surface speed command , speed is 300 ;
N50- Rapid action command , where X52 and Z-10 CNC PROGRAMMING TUTORIAL
N60- Grooving cycle command , distance of return 1mm.
N70- Grooving cycle command , grooving depth on x-axis is 30 , last groove position in z-axis is 30 , Peck increment in x-axis 3000 micron = 3 mm , stepping in z- axis is 20000 micron = 20 mm .
N80- Rapid action command , where X60 and Z-30
N90- Referance point command , where X0 and Z0
N100- Spindle stop , main prog end .

[sinha_nsit]

Thank you all. MY cnc is Oi Mate-TC.
I tried with above all got error but jackson format works. May be the Jackson fromat is compatible to my cnc.
G75 R0.
G75X43.5Z-37.95Q2600P500R0.5F0.1
G0Z2.
and it works.
thank you all . You all make me try and now i know something about it.

Better to replace R0 by R0.1 in the first line.
Do not use R in the second line unless there is room for lateral retraction.

[harshal]

FANUC G75 CANNED CYCLE GROOVING CNC PROGRAM WITH description
July 19, 2018 - FANUC G75 GROOVING CYCLE [T]

In this program we only perform fanuc grooving G75 cycle for cnc lathe operation

01451
N10 G90 G21 G99 F0.15 ;
N20 G50 S1500 ;
N30 M06 T01 01 ;
N40 M03 G96 S300 ;
N50 G00 X52 Z-10 ;
N60 G75 R1 ;
N70 G75 X30 Z-30 P3000 Q20000 ;
N80 G00 X60 ;
N90 G28 U0 W0 ;
N100 M05 M30 ; More examples..........!!!!

DESCRIPTION OF MAIN PROGRAM :-
01451 - Name of main program
N10- Absolute co-ordinate system , metric input in mm , feed rate per revolution , feed is 0.15
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Tool change command , select tool no. 1
N40- Spindle ON clockwise , constant surface speed command , speed is 300 ;
N50- Rapid action command , where X52 and Z-10
N60- Grooving cycle command , distance of return 1mm.
N70- Grooving cycle command , grooving depth on x-axis is 30 , last groove position in z-axis is 30 , Peck increment in x-axis 3000 micron = 3 mm , stepping in z- axis is 20000 micron = 20 mm .
N80- Rapid action command , where X60 and Z-30
N90- Referance point command , where X0 and Z0
N100- Spindle stop , main prog end .

my link is
FANUC G75 CANNED CYCLE GROOVING CNC PROGRAM WITH description - CNC PROGRAMMING TUTORIAL

[sinha_nsit]

Digging old graves ?

[juanprettell]

excelente amigo , este código también es compatible con el fanuc 6t