[camtd]

I have two programs that I am using for a reference. One has a G50 and the other has a G92 if use for setting the tool coordinate system and max. rpm would the only difference be if you are programing for a Fanuc A,B or C Gcode system?

Does one Fanuc Gcode system work on all Fanuc controls?

Which sample would be recommended for most Fanuc lathe programs?

Thank You

Here is a reference that I am using http://stankomach.com/catalog/fanucd/B-64304EN-1_01.pdf

Sample - 1

%
O2088
(11/09/99)
N10 G00 G40 G96 G99 M41
N20 G30 U0. W0.
N30 M01

N40 G30 U0. W0. (ROUGH FACE & ID)
N50 T0100 G40
N60 G50 X28. Z15. S50
N70 G00 X33. S100 M03 T0101
N80 Z1.77 M08
N90 G01 X34.5 F.007
N100 G00 Z1.85
N110 X33.3
N120 G01 Z1.445
N130 X32.9
N140 G00 Z2.
N150 X33.7498
N160 Z1.85 G41
N170 G01 Z1.8
N180 X33.5008 Z1.445
N190 X33.25
N200 G00 Z15. G40 M09
N210 G30 U0. W0. T0100
N220 M01

Sample - 2

(03/08/2001)
N10 G00 G40 G96 G95 M42
N20 G30 U0. W0. T0000
N30 G92 X25. Z15. S30
N40 M01

N50 T100 M43 (ROUGH FACE & ID)
N60 G92 S150
N70 G00 X33. S1200 M03 T101
N80 Z1.77 M08
N90 G01 X34.5 F.005
N100 G00 Z2.2
N110 X33.3264
N120 Z2. G41
N130 G01 Z1.8006
N140 X33.0768 Z1.445
N150 X32.6
N160 G00 Z2.3 G40
N170 X33.6338
N180 Z2.1 G41
N190 G01 Z1.9368
N200 X33.2888 Z1.445
N210 X32.8
N220 G00 Z2.4 G40
N230 X33.792
N240 Z2.2 G41
N250 G01 Z1.86
N260 X33.5008 Z1.445
N270 X33.1
N280 G00 Z15. G40 M09
N290 G30 U0. W0. T100
N300 M01

[angelw]

I have two programs that I am using for a reference. One has a G50 and the other has a G92 if use for setting the tool coordinate system and max. rpm would the only difference be if you are programing for a Fanuc A,B or C Gcode system?

Does one Fanuc Gcode system work on all Fanuc controls?

Which sample would be recommended for most Fanuc lathe programs?

Thank You

Yes to the A,B, and C code system question. Most Fanuc controls are set to use system A.

In general terms, Fanuc programs are transportable across controls. There will be some differences with regards to OEM assigned M functions, but the programs will work without too much editing.

Of the two examples listed, sample 1.

If its an Oi control you have then its likely to have geometry offsets, and automatic coordinate system setting was available on these controls if they didn't have work shift offsets. If this is the case, use geometry offsets and work shift or automatic coordinate system setting instead of G50 for coordinate setting; its a lot safer than using G50 coordinate setting.

Regards,

Bill

[MetalZilla]

G92 on a Fanuc control is a threading cycle on a mill it is like a G50 on a lathe. Check this: G92 Example

[angelw]

G92 on a Fanuc control is a threading cycle on a mill it is like a G50 on a lathe. Check this: G92 Example

Besides being an ancient Thread you've dragged up, I'd suggest you read the Thread first as your reference to G92 in the context of the Subject Thread is completely incorrect.

Regards,

Bill

[MetalZilla]

Besides being an ancient Thread you've dragged up, I'd suggest you read the Thread first as your reference to G92 in the context of the Subject Thread is completely incorrect.

Regards,

Bill

Excuse me. Did you even bother to read the post!? You have obviously confused a G92 Threading Cycle with a G90 Code. Duh!

[angelw]

Excuse me. Did you even bother to read the post!? You have obviously confused a G92 Threading Cycle with a G90 Code. Duh!

Yes I did read it, quite thoroughly in fact; but clearly you haven't. Following is most of the OP's original text. You will notice that the G92 in Sample2 and highlighted in Red, is being used for the same purpose as G50 also highlighted in Red in Sample1. G92 is used to set the Coordinate System and to clamp the Maximum Spindle Speed in Constant Surface Speed in Fanuc "G" code System B and C. G50 is used for those purposes in Fanuc "G" Code System A.

G90 doesn't enter into the argument whatsoever, except that it's used to set Absolute Mode when the Fanuc Control is set to use either "G" Code System B or C; there is no confusing it with G92. Obviously you're totally confused. You dragged up an old Thread in your Post #3 to advertize your software, but the main thing that's on display in your Post #3 and #5 is your lack of programming knowledge.

Duh!

I have two programs that I am using for a reference. One has a G50 and the other has a G92 if use for setting the tool coordinate system and max. rpm would the only difference be if you are programing for a Fanuc A,B or C Gcode system?

Does one Fanuc Gcode system work on all Fanuc controls?

Which sample would be recommended for most Fanuc lathe programs?

Thank You

Here is a reference that I am using http://stankomach.com/catalog/fanucd/B-64304EN-1_01.pdf

Sample - 1

%
O2088
(11/09/99)
N10 G00 G40 G96 G99 M41
N20 G30 U0. W0.
N30 M01

N40 G30 U0. W0. (ROUGH FACE & ID)
N50 T0100 G40
N60 G50 X28. Z15. S50
N70 G00 X33. S100 M03 T0101
N80 Z1.77 M08
N90 G01 X34.5 F.007
N100 G00 Z1.85
N110 X33.3
N120 G01 Z1.445
N130 X32.9
N140 G00 Z2.
N150 X33.7498
N160 Z1.85 G41
N170 G01 Z1.8
N180 X33.5008 Z1.445
N190 X33.25
N200 G00 Z15. G40 M09
N210 G30 U0. W0. T0100
N220 M01

Sample - 2

(03/08/2001)
N10 G00 G40 G96 G95 M42
N20 G30 U0. W0. T0000
N30 G92 X25. Z15. S30
N40 M01

N50 T100 M43 (ROUGH FACE & ID)
N60 G92 S150
N70 G00 X33. S1200 M03 T101
N80 Z1.77 M08
N90 G01 X34.5 F.005
N100 G00 Z2.2
N110 X33.3264
N120 Z2. G41
N130 G01 Z1.8006
N140 X33.0768 Z1.445

[angelw]

Double Post for some reason.

[harshal]

CNC G92 threading cycle for fanuc program (metric threading)
July 29, 2018 - FANUC G92 THREADING CYCLE [T]

G92 threading code is used in "G-code system A"




O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X50 Z2 ;
N60 G92 X49.07 Z-20 F1.5 ;
N70 X48.77
N80 X48.47
N90 X48.17
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF MAIN PROGRAM :-
Calculation :- Depth of thread = 0.6134 X Pitch
= 0.9201
Crest = major dia - 0.9201
= 49.07
Root = Major dia - 2 x Depth of thread
= 50 - 2 x 0.9201
= 48.16 (root)
Each cut is 150 microns =0.15mm , it means total reduce 0.30 mm and cutting upto root 48.16 mm
First cut is 49.07 mm (Crest)
Second cut is 49.07-0.3 = 48.77
Third cut is 48.77-0.3 = 48.47
Final cut is 48.47 -0.3 = 48.17 (~ 48.16)(root)
*************************all dimension in mm ***********************************
01571 - Name of main program
N10- Tool change command , select tool no 2
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Spindle ON clockwise , constant spindle speed , speed is 200 rpm
N40- Coolant ON
N50- Rapid action command , where X50 and Z2 .
N60- Threading cycle command , where X49.07( crest )(First cut) and Z-20 , feed rate is 1.5 ( it is always is equal to pitch )
N70- Second cut is 48.77 in X axis
N80- Third cut is 48.47 in X axis
N90 - Final cut is 48.17 in X axis (root)
N100 - Reference position command , where X0 and Z0 ;
N110 - Spindle OFF , coolant OFF , main prog. end

my link is
CNC G92 threading cycle for fanuc program (metric threading) - CNC PROGRAMMING TUTORIAL

[angelw]

CNC G92 threading cycle for fanuc program (metric threading)
July 29, 2018 - FANUC G92 THREADING CYCLE [T]

G92 threading code is used in "G-code system A"

O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X50 Z2 ;
N60 G92 X49.07 Z-20 F1.5 ;
N70 X48.77
N80 X48.47
N90 X48.17
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;

Just like that other Spambot MetalZilla, you've dredged up an ancient Thread to promote your own web site. The OP's Thread is specifically about the use of G92 being used to set the Coordinate System of a Lathe control; it has Zero to do with the G92 Threading. Clearly, one of the machines referred to by Poster camtd, must be set to use "G" code System B or C.

Just like Spambot MetalZilla, you should read the Thread.