Hi Bill
No joy.
Distance to go - 250 and ends up machine - 250
Where do I go from here
Dusty
View attachment 396991
Hello Dusty,
Everything on the above page is how it should be, except for the Distance To Go of Z-250.0. This would have been the ALL Position Page just after G90 G43 Z0.0 H01 Block was executed with the Feed Rate Override turned to Zero with the Control in Dry Run Mode.
I suggested using the Number 00 Shift Offset (G52) as a test, for if you got no positive result with that, then you won't get any different result with G54 to G59.
The value in the Absolute display of Z-100.0 indicates that the control is reading the value registered in the G52 (00) Offset registry. The Machine Coordinate System reading of Z0.0 is correct, as the Z Axis will be at the Reference Return Position, but the control seems to have missed doing the Math to apply the Z Work-shift and Tool Length Offset values together.
I had a play with the Argo Vertical Machining Centre I referred to in an earlier Post and in MDI, any axes move command entered via MDI simply disappear off the screen when Cycle Start is pressed, as if execution was successful, but no movement occurs. Accordingly, it could be that your issue is because you're executing the command in MDI and not via a program in memory. If this is the case, its MTB introduced and nothing to do with Fanuc. However, if you get the same result running program in memory, there may be an issue with the control not doing the math to combine the Work-shift and Tool Offset values.
With a +100.0 value in the Z Work-shift registry, and a Zero Value registered in the H01 Offset, its saying that the Z Zero of the Workpiece is at Z+100.0 from the current Z axis slide position, therefore, it must be at Z-100.0 currently. If you were to execute the G90 G43 Z0.0 H01 with a Zero value in Tool Length Offset 01, the control would try and move the Z axis from its current Z-100.0 to Z 0.0 and would Overtravel in the Z+ direction. With a -250.0 value set in the Offset Registry for T01, the control combines the Z Work-shift value of Z+100.0 and the Tool Length offset of Z-250.0 to result in a minus Z direction move of -150.0.
I take it that there is no real job in the machine and you're just seeing that all functions work. That being so, try another method of setting the Work-shift and Tool Length Offsets. For this test, rough values will be close enough.
1. Measure the length from the face of the Spindle to the Tip of the Tool that's in the Spindle. A rule or tape measure, measurement will be close enough. Let's say that it's 100.0mm and register +100.0 in the T01 Tool Length Offset registry.
2. Move the Z Axis down, will the Tool in the Spindle, so that the Tip of the Tool is where Z Zero is on an imaginary Workpiece. Again, a rule, or tape measure measurement up from the table will be close enough.
3. Lets say that with the tip of the Tool at 150.0mm up from the surface of the table the Z value in the Machine Coordinate Display value reads Z-175.0. Add the absolute value of Z-175.0 (+175.0) to the Offset Value of the Tool Offset value of +100.0 and the result is 275.00. Register this value, but as a Minus Value, in the G54 Z Offset Registry. This indicates that the distance and direction from the Spindle Nose Face to Z Zero on the Workpiece is Z-275.0mm.
4. From a program registered in memory, run the following Blocks:
G91 G28 Z0.0
G90 G54 Z0.0 H01
With the control in Dry Run Mode and the Feed Rate Override set to Zero, the ALL Position Page should show a Distance To Go of Z-175.0 when the G90 G54 Z0.0 H01 Block is executed. I really don't expect this to be a resolve though.
Regards,
Bill
