*SOLVED* Fanuc OM-C GoProbe Throwing 115 Alarm

I've managed a mostly working legacy Renishaw Probe System on a mid 90's YCM Supermax 3 w/Fanuc OM-C control. I've got Macro B w/Extended Variables.

I don't yet have the extended keyboard so I can do very little in MDI. I've calibrated and run simple Inspection Plus routines successfully. But it's the GoProbe functionality that I really want working.

As a test I've been trying to run a Single Surface Y axis measurement. Command line used is G65 P9901 M1. A2. S55.

It goes through a few nesting cycles eventually throwing an alarm after returning to the main 9901 GoProbe Macro. When it sees the following line it alarms with "115 P/S Alarm". This alarm is early on and before the Probe even turns on. BTW this line does not cause my 18M-C Mori any trouble at all.

M98P9723 (Returning from this short basic time stalling sub to the main 9901 program)
#16=#[#107+#29] (this line)
IF[#120AND3EQ1]GOTO2
#16=#[#106+#29]+#[#107+#29]

Included 2 following lines in case some Look Ahead issues

Fanuc Manual: 115 P/S Alarm
A value not defined as a variable number is designated.
-----------------------------------------
In a subsection of the alarm:

The header contents are improper. This alarm is given in the following cases.
High Speed Machining
1. The header corresponding to the specified call machining cycle number is not found.
Then 4 more about out things of range
5. The storing start data variable number of the executable format data is overlapped with the variable number used in the header.

Yes... a mouthful. Please help. I'm all ears. This is the last thing holding me up. Wasting a lot of time already. Thanks!

Figured it out.

#16=#[#107+#29] (this line) Throws error 115. (Out of range)
IF[#120AND3EQ1]GOTO2
#16=#[#106+#29]+#[#107+#29]

The softwares Setup Macro had previously set a Tool Geometry Offset base number of #2200. The statement above added my probe offset of 64 to that number and that puts the number beyond (out of range) of what the OM uses for System Variables concerning Tool Offsets in Offset Type A. (One column) I changed the #2200 to #2000 and it fixed it. Appears to be a bug in the Renishaw Wizard software when setting up for an OM. Note this info is relevant to OM's with 200 or less offsets. 400 offsets uses numbers over 10000.

One thing for sure, the OM processes waaay slower then my 18M machine. It was tryuly lumbering along.

Can finally get back to work. Yeah!!!

You should see a 6 run it. Glacial.

I wrote a little macro to do parabolic “interpolation”. Ran on a Nakamura TMC20 with Fanuc 0TB. No mater what rpm or feedrate, it could not actually move faster than about 6IPM. The calculations just bogged down the control to the point that’s all the faster it could manage. Would have liked to run that on a 16T for comparison.