Using G-Code for setting offsets

[firedog]

Within the last couple of weeks, there was a post in one of the forums about using a G10 line to set tool length offsets, cutter comp, work co-ordinates and other related values. I have been unable to find that post again and was hoping someone out there could direct me to it.

Thanks in advance,

Firedog

[psychomill]

Are you on a Fanuc type control?

Depending of the offset type you are using and I'll assume this is a mill. Type A ( Single offset only ), Type B (Length and wear offsets), Type C (length, length wear, geometry, geometry wear).

For Type A:
G90 G10 L11 P??? R??? (L11 = offsetting, P = offset number, R = value)

For Type B:
G90 G10 L10 P??? R??? (L10 = length offsetting, P = offset number, R = value)
G90 G10 L11 L??? R??? (L11 = wear offsetting, P = offset number, R = value)

For Type C:
G90 G10 L10 P??? R??? (L10 = length offsetting, P = offset number, R = value)
G90 G10 L11 L??? R??? (L11 = "H" wear offsetting, P = offset number, R = value)
G90 G10 L12 P??? R??? (L12 = "D" geometry offsetting, P = offset number, R = value)
G90 G10 L13 L??? R??? (L13 = "D" wear offsetting, P = offset number, R = value)


HTH

[firedog]

Thanks psychomill!!
It is a Fanuc type control, and it is a mill. The post I remember seeing would put this at the end of the program, after the M30. The operator would start the program the first time at the very end, after the M30, to load the values. After that, all adjustments would be made on the offset pages, not in the program.

I was hoping to find that post again so I could use the same sequence they were using.

Thanks,
Firedog

[MILLMANM]

this is how we do it

O2741 (0040-77741 2ND OP)
/M0 (OPERATOR CHECK STOP)
G10 L2 P1 J1 X-6.8311 Y-12.6290 Z-20.2510 B270.
G10 L2 P2 J1 X-21.9588 Y-12.6290 Z-25.3986 B0
G10 L2 P3 J1 X-1.6843 Y-12.6290 Z-25.3802 B180.

but it has a yasnac control and it writes it to the x,y,z,b, offset every time it runs

[psychomill]

I guess I forgot to add the G10s for work coordinates. Yasnacs use J offsets (G54 J1, G55 J4, G54J3 etc.) On Fanuc it will be like this:

G10 L2 P1 X?? Y?? Z?? B?? (A?? if you have it or even C?? for 5axis)

L2 = G54 ofsetting
P? = offset number (1= G54, 2 = G55, 3 = G56 etc)

Or for extended offsetting (G54.1):

G10 L20 P1 X?? Y?? Z?? B?? etc, etc

L20 = G54.1
P?? = offset number

[chetan]

Hi can anybody tell me,
what is Q in G10 format. My m/c is cnc sliding head turning
Format is something like this.G10 P...... X....... Z........R..... Q....?
I heard that it is tool type from 1 to 9
Does it affects the size of the part.

Thanks in Advance

[dcoupar]

It is the imaginary tip number (0-9) for use with G41/G42. If you don't program G41/G42, it doesn't do anything.

[chetan]

Hi
My machine is tornos bechler enc 162 Fanuc OT. When i use tool for front turning i dont have any problem with diameters. But when i use the same tool for back turning , the first two diameters are coming correctly what i have mentioned in program, but later diameters are coming undersize and some are over sizes. I dont know why is this happening so. The only good news is that every subsequent part is having same variations. I dont know what to do. PLease help me.

[Algirdas]

chetan, Your explanation is very messy, but the problem is clear.
You have several solutions here:
1. Diagnose and remove the problem roots
2. use cure #1
3. use cure #2
4. find better solution
Detailed:
1. You need to investigate, why this happens. Maybe problem is mechanical.
2. You can use separate tool offsets. It doesn't helps much, if You cut the shape with different diameters by one tool.
3. You can use separate zero offsets. This solution can partially compensate mechanical problem.
4. You can combine some and find Yours.
The main obstacle is that it in not clear, why it happens.