[723]

I am currently running a VMC with a Fanuc controller. Every time home position needs to be set, we have to jog the machine to the spot and read the machine cordinates, transfer them over to the G54-G59 by writting the position on a paper and entering them manually. Is there a shortcut to this like setting your height offsets ( EOB + Z ).

Thanks

[Al_The_Man]

Do you mean how do you set work co-ordinate zero or that you cannot home using the normal home routine?
Al

[723]

On the Fanuc O controller, it is very time cunsoming right now
for us to set the home position. On a fadal if I am not mistaken, all you have to do is jog to position that you want to set your home and type in SET X & SET Y. On a haas it is even easier by pressing a button and your cordinate offsets are taken. On our machine we have to jog to position, writte down the machine cordinates on paper, transfer them to G54-G59 offsets, double check to see if there was no errors in transfering the numbers.
It get old real fast so I would like to know if there is a short cut to this? I would like to know how you set your home position cordinates on fanuc controllers?
I wish fanuc could make there controllers more user freindly

[bob1371]

Not sure I understand what your looking for here but maybe a G92 X0 Y0 Z0; ?

[Boris_Fly]

Hi there

As a rather experienced user of Fanuc powered VMC's I have never heard of a shortcut way of entering the G54- G59 offset data.
The only thing I have done is put the offset data in the programs with a G10 command and used dowel holes in the table to quickly line up the jigs for each program,

[Scott_bob]

The current machine coordinate position can be writen to your offset register this way:

Make a CNC program for setting offsets.

01111(OFFSETTER)
G0
G91G28Z0M1
M0(X0 Y0 OFFSETS)

N54G0G90G54X0Y0
M0(MOVE TO G54 POSITION)
N541#5401=#5901
M0(SET X)
N542#5402=#5902
M0(SET Y)
G90G54X0Y0
M0(G54 X0 Y0 IS SET)

N55G0G90G55X0Y0
M0(MOVE TO G55 POSITION)
N551#5501=#5901
M0(SET X)
N542#5502=#5902
M0(SET Y)
G90G55X0Y0
M0(G55 X0 Y0 IS SET)

ETC...
The Variable numbers may be wrong above, SO CHECK YOUR MANUAL.
I am at home away from my Fanuc OM manual...

But you can see the logic.
#5501 will be the variable that contains G54 X offset from machine coordinate zero.
Current coordinate position is variable #5901
N541 (sets the G54 X offset value, from the current position variable)
M0 (is for moving the machine to your Y position, say if you're edgefinding, if no move then cycle start sets the offset)
N542 (sets the G54 Y offset value by cycle start...)

This makes it very easy to set all your offsets...
You can use this same program technique to set Z offsets, and length offsets...
Just check out the manual in the custom macro B section.

[Scott_bob]

Correction:

For setting G54 offset from the "Current" machine Coordinate position:

N54G0G90G54X0Y0
M0(MOVE-TO-G54-X0)
N541#2501=#5021(SET-G54-X0)
M0(MOVE-TO-G54-Y0)
N542#2601=#5022(SET-G54-Y0)
G54
G91G28Z0
M30
N55G0G90G55X0Y0
M0(MOVE-TO-G55-X0)
N551#2502=#5021(SET-G55-X0)
M0(MOVE-TO-G55-Y0)
N552#2602=#5022(SET-G55-Y0)
G55
G91G28Z0
M30

**Notice the M30 afterwards, this resets the machine and program**

Here is the Length offset example:

O1111(OFFSETER)
G0G17G40G80
G91G28Z0
G90G53X-17.23Y-.25
M0
N100G91G28Z0T1
M6
M0(SET-Z)
N1#2001=#5023(SET-H1)
G91G28Z0M0
N200G91G28Z0T2
M6
M0(SET-Z)
N2#2002=#5023(SET-H2)
G91G28Z0M0

[Shop Rag]

If you have an old Omate control it is a bit difficult to set the work offset. My question to you is how old is your machine/control. The fanuc manuals that come with the machine will have the model number of the control. The model number is also on the control by the CRT. If you get me this information I might be able to give you some ideas on how to speed up set-up time.

[723]

Thanks Scott_Bob for your info. I will try your way ASAP.
Shop Rag, the controler is from a 1997 VMC. It is a FANUC 0-M C.
I think it was the last of the Fanuc controler before they moved on
Thanks.