hi,
I have Fanuc Om Kontrol Machine by supermax,

that machine;
I was send rs232
:9016
G66P9017
G#100
G67
G91G30X0
G65H04P#101Q2R#1000
G65H03P#102Q30R#101
..
..
machine accept and record but

not accept this kind of macro
:9020
#3003=1
IF[#20EQ#0]GOTO100
M70T#20
G4X0.1
IF[#1008EQ1]GOTO300
IF[#20EQ0]GOTO100
IF[#20GE100]GOTO90
IF[#20GE21]GOTO100
N90IF[#1012EQ1]GOTO101
#140=0
#149=#4003
#148=#4001
#147=#4006
G0G91G80G49M19
..
..
and give me alarm
004 adress not found
I was changed TV kontrol nothing,

I try write "IF" impossible
I try write "#" impossible

What shell am I do?

Osmanselim you are on a bunch of forums. All the same ones as me. I never know which one to answer. I have answered this at 2 other forums. I know that this site can be picky about what kind of data is posted when it comes to options. So check the other forums for more information. This however is probably your problem.

Address not find means that it read some of your statments but when it tries to GOTO it is not finding the N address that you are telling it to GOTO.

At the beginning of your program take out the #3003=1 this is a single block suppression. Now you can single block through the program. You will then be able to see which GOTO line and it is alarming out on. For example if it reads the IF[#1008EQ1]GOTO300 line and alarms out it means that #1008 was equal to 1 and it is trying to jump to N300 line but could not find it in the program.

Check that you have MacroB and not MacroA. This could also be your problem.

Stevo

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

This is tool changed macro İs this correct,

:9020
#3003=1
IF[#20EQ#0]GOTO100
M70T#20
G4X0.1
IF[#1008EQ1]GOTO300
IF[#20EQ0]GOTO100
IF[#20GE100]GOTO90
IF[#20GE21]GOTO100
N90IF[#1012EQ1]GOTO101
#140=0
#149=#4003
#148=#4001
#147=#4006
G0G91G80G49M19
M6
IF[#1009EQ1]GOTO10
WHILE[#1009EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
#140=0
N10M71
M72
WHILE[#1010EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO98
G30P3Z0
END1
#140=0
M73T#20
WHILE[#1009EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
M74
G#148G#149G#147
M75
GOTO300
N98#3000=20
N99#3000=21
N100#3000=22
N101#3000=28
N300
#3003=0
M99

Your #20 is not being set to the tool that you want to call. I assume that you are doing a M6T5 to call this program. The best way is at the beginning of the program Set #20 equal to your modal T call which would be 5 or whatever tool you want to call.
#20=#4120
Once you hit any of your WHILE statements they will loop until #140 is GE to 4 then they will alarm out. I am not sure what you are trying to do in those statements. What are all of your WHILE statements suppose to be doing with the system variables that you are using #1009, #1010????

I think that you are way over complicating the tool change process. It is a rather short process. There is only a few lines of checks that you should need and a few special setting that you want to set. Really just skip the M6 command if your calling a tool that is already in the spindle that’s an easy command. Move to your tool change position, change tools and set the variables that you want and end the program. I also see that you have your M6 programmed before you move to your tool change position. You can’t change the tool with an M6 if your out of position.

Below are some changes if you need to use all of this data. After this program I wrote one that you can prove out and try that is much cleaner.

:9020
#3003=1
#20=#4120
IF[#20EQ#0]GOTO100 I would make this equal to null so if a T is not specified the machine will alarm out change to this
IF[#20EQ[#[0]]]GOTO100
M70T#20
G4X0.1
IF[#1008EQ1]GOTO300 not sure what your doing here. Don’t know what system variable #1008 is in your machine. I see you are just sending it to the end of the program and turning of your single block supression
IF[#20EQ0]GOTO100 –most machines can take M6T0 so this can probably be removed.
IF[#20GE100]GOTO90
IF[#20GE21]GOTO100 is this alarming because you have a 20 tool magazine max??
N90IF[#1012EQ1]GOTO101 put this in place of IF[#20GE100]GOTO90. I don’t see why you are skipping the line above when your always going go read this line anyway if the program does not alarm
#140=0
#149=#4003
#148=#4001
#147=#4006
G0G91G80G49M19
M6
IF[#1009EQ1]GOTO10
WHILE[#1009EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
#140=0
N10M71
M72
WHILE[#1010EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO98
G30P3Z0
END1
#140=0
M73T#20
WHILE[#1009EQ0]DO1
#140=#140+1
IF[#140GE4.]GOTO99
G30Z0
END1
M74
G#148G#149G#147
M75
GOTO300
N98#3000=20
N99#3000=21
N100#3000=22
N101#3000=28
N300
#3003=0
M99
-----------------------------------------------------------------------------------------
I like to set a variable equal to the tool in the spindle and track it that way. You could use the system variable that tracks the tool in the spindle. You have to find out which one it is. If you want to use the system variable replace it with #535. If you use a variable set it to the current tool in the spindle.


Program a M6T5

:9020
#3003=1
#20=#4120—sets #20 equal to modal T which is 5.
IF[#20EQ[#[0]]]GOTO100
IF[#1012EQ1]GOTO101
IF[#20GT20]GOTO102
IF[#20EQ#535]GOTO200—skips the M6 tool change if the tool call is the same as the spindle tool
G40G80M19
G90G49Z#5043—cancel offset and the tool will not move because of #5043
G91G28Z0M9—tool change Z
G28Y0M5---tool change Y
G30P3Z0---UNLESS THIS IS YOUR TOOL CHANGE POSITION IN THE REFERENCE POSITION 3
M6
N200
#537=#[2000+#20]+#[2200+#20]—tool geometry and wear(not need but I like to set my length here)
G43Z[#5043-#537]H#20—sets tool H value with no tool movement(not needed same as above.
#535=#20
#3003=0
M99
N100#3000=22(NO T COMMAND)
N101#3000=28(I DON’T KNOW THIS SYSTEM VARIABLE)
N102#3000=10(20 TOOL MAGAZINE MAX)---probably don’t need this because machine should alarm out if you call a tool number lager then the machine can hold.

(The opinions in this post are my own and not those of machinetoolhelp.com and its management)

HI,
nice to see that you help with your experiances ,
I am having a 20 fa fanuc contoller , and makino machine ,
my machine dont have macro varibles of lost during format , now when we use machine on dnc , it gives buffer flow erroor
, what is the programm which is used for nesting for a external devices and where to specify , provide me the process along with the programm i will be really thankfull sir.