Fanuc 18i-MB macro question

[YoDoug®]

Working on a Bridgeport XR760 mill with a Fanuc 18i-MB control.

 

I have a o9011 macro in the control. When I input G65 P9011 it calls the program as it should.

 

When I go into the 6051 parameter and assign G202 to call the 9011 program it alarms out after reading a G202 saying 078 program not found. I have never had this not work before and I'm stumped.

[Tim Johnson]

It Looks right to me. Can you post the G202 line? Nevermind, if it says it's says it's not found then the G202 is working.

 

Have you shut down and restarted the control?

[YoDoug®]

Yup we already tried restarting. No luck. These mills have a Renishaw probing package with a conversational style interface that was developed by Renishaw/Hardinge. The control is saying that option is not enable and I think the G macro calls may be tied to that function. For now we are just using the G65 macro calls.

[Tim Johnson]

Have you tried the M calls?

[YoDoug®]

I did not try an M code assign yet. I'll try one later today when i get back to the machine.

[SKIR68]

make sure the 9011 program is in the machine memory, NOT just on the hard drive.

[Guest CNC Apps Guy 1]

I'd try an m-code too. 6081 = 202, mod the program to O9021

[Tim Johnson]

Is there any closure to this thread?

 

It's my turn now on a Fanuc 31i-MB.

 

I'm trying to call M501 using program O9026, assigning 501 to parameter 6086 and also G201 using program O9018, assigning 201 to parameter 6058.

 

Neither call works (error 310, program not found) and Fanuc says it appears to be correct. They did say to try a different M-code just in case I'm stepping on the builder's M-code. I tried M55555 with the same results.

 

I use both calls on 7 Fanuc 18i controls but this is my first 31i.

[Guest CNC Apps Guy 1]

I'd make sure that it's in the "LIBRARY" folder on the 31i. If it's not there, put it there. If it is there, then you'll need to go to the parameter (#3457) that expands the folders where MACRO calls are allowed to search.

 

There's a few bits that dictate which folders are searchable.

[YoDoug®]

I could not get the G macro call to work, but I was able to make similar M macro calls work in the machine in question. We ended up just using G65 Pxxxxx when we needed to pass variable through.

[Tim Johnson]

Ok,

 

Setting parameter #3457.6 (SCC) to 1 did the trick.

 

Thanks James for the heads up.

 

 

[Guest CNC Apps Guy 1]

TIm, my pleasure.