Fanuc 18m Macro Parameter

[fahque99]

We have a fanuc 18m and used to have a macro for circular bolt holes, but all the parameters were lost and now the macro does not work. Does anyone know the option parameters for getting marcos to work? Or if anyone has a option parameter list for the 18m could they please send it to fahque99@hotmail.com ?

Thanks.

[stevo1]

So you lost your options/parameters and you have no backups? What is the alarm you have when trying to run a macro or will it not carry over values in the macro call or do the IF,GT, GOTO statements? Or can it be the fact it was a custom G or M code that called the program and now it will not? Need a bit more info.

9933.7 Macro B programming.

Stevo

[fahque99]

as soon as you try to write a value to a variable you get a error code.

error 009 ILLEGAL ADDRESS INPUT

[fahque99]

That option setting allows me to use variables now, but now I get DIVIDE BY ZERO errors whenever I try to use a divide command. Are there options to be able to use math commands? I dont have a backup of the machine because when I started this job the machine was already wiped of all the settings and I have been slowly getting everything working on it.

Thanks.

[stevo1]

There is no options to turn on to use these math functions this is part of the macroB option. Some functions can not be used depending if it is macroA or macroB that is turned on. Can you post the code you are trying to run and getting the error? I am not sure about the 009 alarm on the 18 control but the divided by zero alarm is typical when you do exactly that, try to divide by 0. If you are trying a macro call with G65 make sure that the variables that you are passing through are actually being set. Ex. G65P()A5B10. Look at variables #1 and #2 to see if they are set to #1=5 #2=10. Remember not to hit the reset button before going to look at these variables as they will clear when the reset button is hit. Easy try for dividing. Program in MDI.
#1=5
#2=10
#3=#2/#1
If you get no alarm look at the variables they should be equal to
#1=5
#2=10
#3=2

I thought that you were having trouble changing the parameter. I was digging through my stuff to find the procedure for changing the parameters on the 18m control but I could not find it. Must have lost it with the move. If you have it could I PM you my email to get it from you?

Stevo

[fahque99]

Here is the code I am trying

 
=%
O9010 (BOLT CIRCLE)
#1= 8 (NUMBER OF HOLES)
#2= 15 (DIAMETER OF CIRCLE)
#11=0 (ANGLE OF FIRST HOLE )
(DO SOME SETUP CALCULATIONS)
#2=#2/2 (BOLT CIRCLE RADIUS)
#20=[360/#10] ( ANGLE BETWEEN HOLES)
#1=#1-1
G91 G28 Z0.
G54 G90
M05
M00 
S2000 M03
(FIRST LOCATION)
G81 X[[COS[#11]*#2]] Y[[SIN[#11]*#2]] R1.0 Z-0.25 F4.5 (DRILL CYCLE)
WHILE[#1GT0]DO1 (LOOP)
#11=#11+#20 (POSITION HOLE TO DRILL)
#1=#1-1 (NUMBER OF HOLE DECRIMENT)
#21=[[COS[#11]*#2]]
#22=[[SIN[#11]*#2]]
X #21 Y#22
END1
G80
M05
G91 G28 Z0.
M00
M30
%

I dont know if I have the macroA enabled or not, should I have both on?
Is it the fanuc 18m manuals that you are looking for? PM me your email.

[stevo1]

You don’t need macroA and B active. Check #9933.7 if this is set to 1 you’re fine for macro programming. If it is set to 0 check #9922.6 for macroA. If you are able to use variables then one of these 2 should be set.

I don’t need the 18m manuals those I have. I thought you had to change #9933.7 which is an option and takes a procedure that is not in the manuals.

I have not looked over your entire program but I see why you are getting the alarm. Look at the calculation for “angle between holes”. #20=[360/#10]. You don’t have #10 set before that. So as the program reads #10 is set to null. If you try to divide by a null variable you will get the divided by zero alarm. This is probably supposed to be #1 instead of #10. This will make #20 equal to 45 the angle between your holes. I will read the rest a bit later to see if I can see any other errors.

Stevo

[fahque99]

Yep, it was the #10 problem. Everything seems to work good now. Thanks for all the help.