Probe in VM-2

[Chris59]

We have a VM-2 2011. We finally upgraded our CAM software from 2011 to 2021. So, they have probing in the CAM now (we used to have to manually add it to the posted G code).
We were adding the code VQC style using P9023 A...

The newer software post uses the many more options shown in the "Inspection Plus software for Haas machining centres" . For example: P9811, P9815 etc..

Well, the probe post output is alarming out. So far, I've narrowed it down to Alarm "503 unsupported macro variable".
The Haas mill alarms at the P9811 line. It actually probes in Z but alarms at the conclusion of the probe motion.

I checked that we have the 9000 programs including P9811 in the machine (we do).

N25 (RENISHAW PROBE)
T25 M06
G00 G90 G58 X0 Y.07
G43 Z1.125 H25
G65 P9832
G65 P9810 Z.3 F100.
( PROBE SURFACE IN Z )
G65 P9811 Z0 Q.1575 S58.
G65 P9833
G00 G53 Z0.0
M01

Do I need to unlock something (yes, we have probing on the mill)?

 

[RenPDL]

I think the issue may be that the S58 input is not valid. The manual I have does not show this format is supported. If you want to update G58 you would need to use S5. Not knowing exactly which version of probe software you have could mean this isn't correct, but it would make sense based on the alarm you are getting. S58 would calculate a variable location that doesn't exist.

 

[Chris59]

I'll try that. Thanks.
I used S58. because that's what is required for the VQC version using P9023.
I'll report back what I find (when I get a chance to break in, I mean)

 

[countryguy]

Just something I found... Might have a clue to hint?
Redirecting to https://www.cnczone.com/forums/haas-mills/107001-probe-alarm.html

 

[jrfiggz]

Not sure if you got this working, but definitely what RenPDL said: S input is invalid.
From the manual,

s = The work offset number which will
be set.
The work offset number will be
updated.
S1 to S6 (G54 to G59)
S0 (external work offset).
S110 to S129 (G110 to G129)
additional offsets option.
S154.01 to S154.99 (G154 P1 to
G154 P99) additional offsets
option.
New work offset = active work
offset + error.
New external offset = external
offset + error.

the link that was provided by country strictly has to deal with vector measurement cycles. All of the standard probing cycles don't require that form of calibration, although it doesn't hurt if you ever want to use the vector cycles.

 

[Chris59]

Thank you guys. I'm afraid it may be a few days (probably next week at the earliest) before I can try out the ideas. We're running a long job that is time critical.
I will absolutely post what I find, when I find it.
Thanks!

 

[Chris59]

Ok, finally had a chance. jrfiggz and RenPDL were right on the money. Thanks all for responding. Changed my S58. to S5. and bingo. Works like a charm!
Thanks!

 

[jrfiggz]

I know it’s been a while, but I’d recommend a process change to make this more intuitive… if you program to your 154 offsets, in your inspection routines you simply specify your P offset with an appended decimal… S154.01 === G154 P1, S154.02 === G154 P2 and so on. It’s a little more clear than S5 is updating G58

 

[rjwalker1973]

I know it’s been a while, but I’d recommend a process change to make this more intuitive… if you program to your 154 offsets, in your inspection routines you simply specify your P offset with an appended decimal… S154.01 === G154 P1, S154.02 === G154 P2 and so on. It’s a little more clear than S5 is updating G58

Thats how I do mine as well. Just translates better.