[Deco-Doctor]

Hi

I am trying to program the G78 threading cycle on a Fanuc 0i-TD without the proper Fanuc manual. I have the standard 0i-D manual which does not cover the G78.

Please can someone who knows this control jot down a quick example for me, say an M8 x 1.25 external thread 20mm long, 5 rough passes, one finish pass and one spring cut.

Thanks for your help

[dcoupar]

If I'm not mistaken, the G78 cycle is programmed exactly like G76. The G76 is used in G-Code systems A and B, the G78 is used in G-Code system C. Have you tried the G76?

In my experience, most Japanese/Taiwanese/Korean, etc. machines are set up to use G-Code system A. Some American-made machines were set up to use system C.

[Deco-Doctor]

If I'm not mistaken, the G78 cycle is programmed exactly like G76. The G76 is used in G-Code systems A and B, the G78 is used in G-Code system C. Have you tried the G76?

Hi - Yes it seems you are correct. The parameters for G76 seem the same. I have not tried G76, but I will now.

Any idea what the difference is between G76 and G78?

Many thanks

[dcoupar]

No difference other than the G-Code system.

[harshal]

G78 FANUC THREADING CYCLE PROGRAM FOR LATHE CNC EXAMPLE - CNC PROGRAMMING TUTORIAL
Friends , G76 and G78 are similar threading cycle in fanuc contol cnc . Sometimes some fanuc control cnc model working with G78 Cycle . Mostly used for threading cycle is G76 , behaves same as G78 threading cycle. Manin program will be same , change is only is place of G76 .

G78 FANUC THREADING CYCLE PROGRAM FOR LATHE CNC EXAMPLE - CNC PROGRAMMING TUTORIAL

N10 M06 T01 01 ;
N20 M04 G97 S1000 ;
N30 G00 X45 Z5 ;
N40 G78 P020060 Q100 R50 ;
N50 G78 X38.7 Z-50 P1227 Q100 F2 ;
N60 G00 X45 Z5 ;
N70 M05 M09 M30 ;

DESCRIPTION OF MAIN PROGRAM :-

N10- Tool change command , select tool no. 1
N20- Spindle ON anti clockwise , constant spindle speed command , speed is 1000 rpm
N30- Rapid action command where X45 and Z5 .
N40- Threading cycle command , P020060
( P02 = No. of finished path
00 = Chamfer amount at end
60 = Angle of tool tip ) ,
Q100 = Each cut is 0.1 mm ,
R20 = finishing allowance 0.02mm
N50- Threading cycle command , Minor dia X axis , threading along Z- axis up to -50 , Threading depth , Depth of finish cut 0.1 mm , pitch is 2 .

: M40X2

Major diameter is 40
Pitch is 2
Thread depth calculation = Pitch x 0.61363
= 2 x 0.61363
= 1.227 mm in micron is 1227

Minor diameter = 40-1.23 = 38.7 mm

N60- Rapid action command where X45 and Z5 .
N70- Spindle off , coolant off , main program end .

FOR MORE DETAILS VISIT WWW.HDKNOWLEDGE,COM

[angelw]

Friends , G76 and G78 are similar threading cycle in fanuc contol cnc . Sometimes some fanuc control cnc model working with G78 Cycle . Mostly used for threading cycle is G76 , behaves same as G78 threading cycle. Manin program will be same , change is only is place of G76 .

An ancient Thread that was answered succinctly by dcoupar with "No difference other than the G-Code system."

The G76 and G78 cycles are not only similar, but exact same with an alternate address. There are three different G Code Systems available with a Fanuc ontrol, A, B and C. A and B use G76 to execute the Multi-repetitive Threading Cycle, whilst the G Code C System uses G78.

Regards,

Bill