fanuc 9000 series programs

[axis overtravel]

hi all

i have a question regarding 9000 series programs.

i run a daewoo puma 350m 3 axis lathe, with a fanuc 18t controller. the machine's build date is 2000

my question is, do the 9000 series program numbers have to refer to a specific function?

or to put it another way, if there is in memory, a program numbered o9001, which is say, a dwell routine, could i overwrite this with another program o9001, which records the position of the tailstock?

the reason i aks, is that i have a training course reference book, which shows programs for different functions, but having the same numbers.

now i realize that there can only be one program in memory with the number o9001 at any time, but i am wondering if the numbers are function specific

thanks in advance for any replies

best regards, axis

Similar Threads:

• Unlock 9000 programs on Fanuc 6m (Parameter 168 set, but machine builder has no idea)
• Fanuc omb 9000 series macros needed bad
• Need Help!- need to unlock 9000 series programs
• Need Help!- 9000 series programs deleted.
• Need Help!- deleted 9000 series sub-programs

[dcoupar]

You should check parameters to see if those program number are being called by M-codes (6071-6079, 6080-6089) or G-codes (6050-6059). If these parameters have values in them, then that program may need to remain unchanged.

6071 M code that calls the subprogram of program number 9001
6072 M code that calls the subprogram of program number 9002
6073 M code that calls the subprogram of program number 9003
6074 M code that calls the subprogram of program number 9004
6075 M code that calls the subprogram of program number 9005
6076 M code that calls the subprogram of program number 9006
6077 M code that calls the subprogram of program number 9007
6078 M code that calls the subprogram of program number 9008
6079 M code that calls the subprogram of program number 9009

6080 M code that calls the custom macro of program number 9020
6081 M code that calls the custom macro of program number 9021
6082 M code that calls the custom macro of program number 9022
6083 M code that calls the custom macro of program number 9023
6084 M code that calls the custom macro of program number 9024
6085 M code that calls the custom macro of program number 9025
6086 M code that calls the custom macro of program number 9026
6087 M code that calls the custom macro of program number 9027
6088 M code that calls the custom macro of program number 9028
6089 M code that calls the custom macro of program number 9029

6050 G code that calls the custom macro of program number 9010
6051 G code that calls the custom macro of program number 9011
6052 G code that calls the custom macro of program number 9012
6053 G code that calls the custom macro of program number 9013
6054 G code that calls the custom macro of program number 9014
6055 G code that calls the custom macro of program number 9015
6056 G code that calls the custom macro of program number 9016
6057 G code that calls the custom macro of program number 9017
6058 G code that calls the custom macro of program number 9018
6059 G code that calls the custom macro of program number 9019

[axis overtravel]

many thanx, dcoupar, for that information.

i think i am beginning to see the light

regards

axis

[g-codeguy]

It has been my limited experience that machine builders do not use the 9001 through 9029 for any subroutine they incorporate. They will use a different 9000 number, and leave those numbers alone. There is a good chance that the 9001 program in your control was put there by a previous user. There is no function assigned to any of the 9000 numbers.

To me the idea for using 9000 numbers is to have a subroutine that can be used by any program. Thus they are always loaded in the control. Protection is always turned on.

An example is the O1 through O4 Safe Index Subprograms that Hardinge suggests you use. I put them in O9001 through O9004 and set the M-codes (6071 to 6074) to call them to 91 through 94 so M91 calls O9001, M92 calls O9002 etc.

[dcoupar]

It has been my limited experience that machine builders do not use the 9001 through 9029 for any subroutine they incorporate. They will use a different 9000 number, and leave those numbers alone. There is a good chance that the 9001 program in your control was put there by a previous user. There is no function assigned to any of the 9000 numbers.

To me the idea for using 9000 numbers is to have a subroutine that can be used by any program. Thus they are always loaded in the control. Protection is always turned on.

An example is the O1 through O4 Safe Index Subprograms that Hardinge suggests you use. I put them in O9001 through O9004 and set the M-codes (6071 to 6074) to call them to 91 through 94 so M91 calls O9001, M92 calls O9002 etc.

Many of the builders I'm familiar with DO use O9001, O9029, etc. for ATC, APC, etc. macros on new machines from the factory. I thought it was best to check before overwriting important macros and subs.

[g-codeguy]

That's why I qualified my statement. Plus it makes more sense to me for the builders to leave those programs for the buyer to use. Not that I've ever come close to using them all! But I guess that would depend on what subroutine the builder supplied. If it got used a lot, then being able to call it up with something like M91 (or whatever number you choose) saves typing and a few characters of memory.

I've stated before that I have zero experience with mills. I would think that a mill could make use of more subroutines than a lathe.

I stand corrected, and you are absolutely right. Best not to overwrite a needed program. Of course, if you're going to be doing something like that, then you should first have an understanding of what is needed for your machine. No sense in reinventing the wheel. I've never overwritten a supplied 9000 program even when I never used the program even once. Might someday want to.

[axis overtravel]

hi g-codeguy

the 9000 series are also used by renishaw probe macros for part measuring/setting etc.

initially, i was wondering if there was/is a specific function assigned to each 9000 number, but after studying the manual, and the information supplied here, i have concluded that there is a relationship between 9000 number, certain parameters and additional G and M codes.

specifically, i have now entered 9000 series programs that will allow me to record the home position and forward position of the tailstock, and then call it forward and send it home again, just by issuing 2 M codes and 2 G codes.

the position record is numbered 9001, which was being used as a macro to reference the c axis.

i have another 9000 program that allows me to use the G30 2nd reference position as a time saver

many thanks for your replies


regards

axis

[gibran23]

algien que tenga los macros 9000 de republic lagun s8 studio