[Master Miller]

Hello,

Can someone explain me how the aditional zero point works with Fanuc?

Example: G54.1 to G54.48 (I believe there are 48 points??)

I wanna know: How I program this en how I call them.

(sorry for my bad english)

Thnx for helping!

Grtz from the Netherlands

[beege]

G54.1 works just like G54, G55....G59. It's only G54.1 though, and P1 though P49

If you have it turned on, you have a table added to you work coordinate systems for P1, P2, P3 etc.

G54.1 P1 X0 Y0
(stuff happens)

G54.1 P2 X0 Y0
(more stuff happens, different place)

Hope it helps!

Beege

[Master Miller]

thnx for your reply!

But how does my program look?

En how I define it?

En are the coordinates data from the ref. point? Like a normal G54?

Hope you will help me

Thnx

[angelw]

thnx for your reply!

But how does my program look?

En how I define it?

En are the coordinates data from the ref. point? Like a normal G54?

Hope you will help me

Thnx

Offset values for G54.1 P1 through P48, or alternatively up to 300, are set in the same way as G54 to G59. A P value should be specified after a G54.1, if its omitted P1 is assumed. G54.1 is called in your program in the same way G54 to G59 are. For example:

G90 G00 G54.1 P1 X0.0 Y0.0

Regards,

Bill

[Master Miller]

Offset values for G54.1 P1 through P48, or alternatively up to 300, are set in the same way as G54 to G59. A P value should be specified after a G54.1, if its omitted P1 is assumed. G54.1 is called in your program in the same way G54 to G59 are. For example:

G90 G00 G54.1 P1 X0.0 Y0.0

Regards,

Bill

Thnx, I think i understand,

except one thing:

How and where i define for example P1???????


Thnx!

[angelw]

Thnx, I think i understand,

except one thing:

How and where i define for example P1???????


Thnx!

If your control has the additional Offset System, the registry can be accessed via the OFFSET function keys, or input via program using G10; the syntax for this is:
G10L20 Pn IP
Where n is the offset number and IP is the axis address and value. These values can be applied in absolute or incrementally by specifying G90 or G91 respectively.

Regards,

Bill


the latter is

[Master Miller]

If your control has the additional Offset System, the registry can be accessed via the OFFSET function keys, or input via program using G10; the syntax for this is:
G10L20 Pn IP
Where n is the offset number and IP is the axis address and value. These values can be applied in absolute or incrementally by specifying G90 or G91 respectively.

Regards,

Bill


the latter is

Oke, for example, is this correct?

G10 L20 P1 x.. y.. z..
G54.1 P1
G90 G0 x.. y..

En what does L20 mean?

Grtzz

[angelw]

Oke, for example, is this correct?

G10 L20 P1 x.. y.. z..
G54.1 P1
G90 G0 x.. y..

En what does L20 mean?

Grtzz

Yes, that's correct. L20 specifies that its the additional offset system that's being accessed. When specifying the additional offset system, it can be programmed as just G54 Pn. It has the same meaning as G54.1 Pn.

Regards,

Bill

[Master Miller]

Yes, that's correct. L20 specifies that its the additional offset system that's being accessed. When specifying the additional offset system, it can be programmed as just G54 Pn. It has the same meaning as G54.1 Pn.

Regards,

Bill

Oke I gonna try it.

But is it also possible to write G54 via the program?
Like:

G10 G54 x.. y.. z..
G54
G90 G0 x.. y..

Hope you understand what i mean.

Grt

[angelw]

Oke I gonna try it.

But is it also possible to write G54 via the program?
Like:

G10 G54 x.. y.. z..
G54
G90 G0 x.. y..

Hope you understand what i mean.

Grt

Just to differentiate between the two systems I would use G54.1, but G54 can be used as long as the Pn is specified.

With regards to your question relating to G10 G54 X...Y...Z..., the answer is no. You have to specify L20 for the additional offset system.

To set the standard offset system G54 through G59 via G10 the syntax is as follows:

G10 L2 P1 X... etc (G54)
G10 L2 P2 (G55)
G10 L2 P3 (G56)
G10 L2 P4 (G57)
G10 L2 P5 (G58)
G10 L2 P6 (G59)

Regards,

Bill

[Master Miller]

Thank you very much for your answers!

I gonna try it

Grtz !

[sinha_nsit]

Everything is nicely explained. I can add just one thing:
G10 L2 P0 X_ Y_ Z_ refers to External WCS.
And, as a matter of personal choice, I recommend the use of system variables (if available) instead of G10 for such purposes.

[sjh]

Hi,
First U must define Zero points coordinates by G10 L20 for ex. :
N100 G10 L20 P1 x100. Y200. Z300.
then call by G54.1 P1 to G54.1 P48

N105 G54.1 P1
I hope I could help u
sjh
:violin:

[Master Miller]

Thanks for any help

it must succeed!

[birdi52]

Hello,

Can someone explain me how the aditional zero point works with Fanuc?

Example: G54.1 to G54.48 (I believe there are 48 points??)

I wanna know: How I program this en how I call them.

(sorry for my bad english)

Thnx for helping!

Grtz from the Netherlands

hlo

we have hearding vmc in which shown coordinates only G54 To G 59


how can i extend offsets like G54.1 P1 G54.1 P2 etc .?

[zavateandu]

What model of Fanuc controller you have?
The extended offsets for coordinate system si an option from Fanuc and must be activated

[memoryman]

What model of Fanuc controller you have? I may be able to answer in Dutch...