Lathe offsett help

Programing an old Whacheon with a Fanuc OT control.
From the programs that were in the machine it goes home with G28 U0 W0 after each tool, then it reads a G50 that is the center of the part. Example G50 X17.135 Z6.13. My experience is with Hardinge with Work shift and a geometry page for offsets. Never used G50 before. If I don't send it home it seems to read the G50 from where it's at I think.
Program looks like this
O5555
G28U0WO
T0101
G50 X17.436 Z6.563
G97S1000M3
GOO X0Z.1
G1G99Z-.25 F.004
G0Z.1
G28U0W0
T0202
and so on.

How do I not send it home and how do I use the G50? There is just one offset page not a geometry and wear page I am familiar with and their is a soft key that says W. SHFT but nothing happens when I push it.
Thanks for any kind of help.

G50 specifies max spindle RPM, used in conjunction with G96 to specify constant surface speed (in lieu of G97).

I'm guessing it's a typo.

Orange Vise said:

G50 specifies max spindle RPM, used in conjunction with G96 to specify constant surface speed (in lieu of G97).

I'm guessing it's a typo.

Click to expand...

Don't think it is. On the 0itc that I run G50 is used for both for max spindle speed and for workpiece coordinate setting depending on what is in the block with G50. I use it most often with live tooling when I have to orient features according to one another.

Looks like the G50 is used to set the tool offset and the G28 U0 W0 insures that the offset is set from the same location every time. If you wanted to comp T1 -.001 in Z then you would change the Z6.563 to Z6.564.

bukwerm said:

Don't think it is. On the 0itc that I run G50 is used for both for max spindle speed and for workpiece coordinate setting depending on what is in the block with G50. I use it most often with live tooling when I have to orient features according to one another.

Looks like the G50 is used to set the tool offset and the G28 U0 W0 insures that the offset is set from the same location every time. If you wanted to comp T1 -.001 in Z then you would change the Z6.563 to Z6.564.

Click to expand...

Correct, it uses G50 for both.

The following is from the 0itc manual so it may not be applicable to your control. If angelw, ox, or someone else who knows fanuc sees this thread maybe they can confirm whether or not it would work. Also, I'm going off of what I've read, not what I've done, so take that into consideration. (I could be incorrect, mistaken, in error, erroneous, inaccurate, inexact, imprecise....)

It appears that G30 P2 U0 W0; (or P3 or P4) can be used to position to 2nd, 3rd, and 4th reference positions respectively. The reference positions are set via parameters No. 1240-1243. (1240 would seem to be the first, or G28, position) That might be a way to set a couple different reference points if you are trying to shave cycle time by indexing closer to your work.

Might cause issues when reloading a program if you had a program that returned to, say, position 2, and then later you changed where position 2 was via the parameter. I'm not experienced enough to say how... I just know I'd do some experimenting with what would happen in various situations before I went ahead and used the method.

bukwerm said:

Don't think it is. On the 0itc that I run G50 is used for both for max spindle speed and for workpiece coordinate setting depending on what is in the block with G50. I use it most often with live tooling when I have to orient features according to one another.

Looks like the G50 is used to set the tool offset and the G28 U0 W0 insures that the offset is set from the same location every time. If you wanted to comp T1 -.001 in Z then you would change the Z6.563 to Z6.564.

Click to expand...

Hi bukwem,
There is around 30 years difference between your control and the OP's. Many FS 0 controls didn't support Workshift Offset programming and only had G50 to set the Coordinate System. Controls that do have Workshift Offset programming still support G50 to set the coordinate system. Workshift Offset Programming is a very basic function; accordingly, I'd be a bit surprised if the machine you spoke of didn't have Workshift Offset programming.

To FIREFOX
When using G50 to set the Coordinate System, the tool must be the actual distance from the X/Z Zero of the workpiece that is specified by the coordinates specified in the G50 block, when the G50 Block is executed. Basically, the G50 Block is setting the Coordinate System as the distance from the current position of the current tool to the Workpiece X/Z Zero. Correspondingly, your comment "If I don't send it home it seems to read the G50 from where it's at I think." is absolutely correct.

Machines that use G50 to set the Coordinate System are easy to crash. Your Block G50 X17.436 Z6.563 is stating that the tool is in a plus direction 17.436 from the Workpiece X Zero and a plus direction 6.563 from the Workpiece Z Zero, when both axes are at the Reference Return position. If the G50 is executed when the Tool is NOT at the X/Z Reference position, say -2.0 inches in X and Z from the Reference position, then the Coordinate System will be wrong by X-2.0 Z-2.0 and a crash is highly likely.

If you can't access the Workshift page then its probable that the control doesn't have that function. Your model control was often supplied with with a single Workshift (No G54 to G59) and a Measure Function was used to set the Workshift. When Workshift is not available, you can set parameter bit 0010.7 to invoke Automatic Coordinate System Setting. When this is set the Coordinate System is set when a Manual Reference Return is performed, using values set in parameters 0708 and 0709 for X and Z respectively. Using this feature is the same as executing the following block:

G50 X_ _ Z* *

Where:
_ _ = the value set in parameter 0708

and

* * = the value set in parameter 0709

When using this system, the offsets for each tool is made in relationship with either one master tool, or static component such as the X/Z face of the turret. The values of parameters 0708 and 0709 are then set using this master tool, or static component.

Regards,

Bill