[CANDC]

Can anyone help explain why this program doesn't work?
It is a simple grid pattern program G79 for fanuc 0p.
the problem seems to be number #103 and #104. when I substitute other numbers, say 20. for I and 2 for K it works. I think part of the problem is #104 has a decimal which is not allowed for hit count. I was hoping the absolute function might drop the decimal point and the FIX would round down to a real number.
Any help would be greatly appreciated!

O0560(HEAD JAMB)
(T3 = .265X.500 OBROUND)
#101=7(WALL THICKNESS)
#102=42(OPENING WIDTH)
#103=[#102+2]
#104=[ABS[FIX[#101/2.75]]]
G20
G90
G65P9700A38.5B10.0
M75X65.Y51.
G31T3X1.25Y2.375
G79I#103P1J2.75K#104
X1.25Y[[#101+7.0625]-4.688]
X[#102+2.25]
G28
G92X65.Y51.
M99

this is for a Strippit turret with fanuc op controls

[G0G90]

Try seperating it out;

#104=FIX[#101/2.75]
#104=ROUND[#104]
#104=ABS[#104]

[CANDC]

Thanks.
So this program does work on other machines. The program is not the problem, my machine is not storing my macro variable values. after I run my program and I check they are stored as null (zero). So now I think I need to figure out why my machine is not storing them? is it a parameter....

[txcncman]

Thanks.
So this program does work on other machines. The program is not the problem, my machine is not storing my macro variable values. after I run my program and I check they are stored as null (zero). So now I think I need to figure out why my machine is not storing them? is it a parameter....

Does your machine even have macro capabilities enabled? Yeah, best start checking parameters.

[CANDC]

Does your machine even have macro capabilities enabled? Yeah, best start checking parameters.

If I understand your question correctly, yes the Fanuc op controller is capable of running macro programs. All the 9000 programs are essentially macros. as far as my parameter settings being correct as to allow this I'm not sure. I have to crack open the manual, unless someone is familiar with these controllers.
For some reason not to many people seem to program turrets like this.

[fordav11]

do you really need to use 2.75?
If you use another number that divides into 7 more evenly you can do this kind of calc and it'll be a 4 digit number without decimal....

7/4=1.75*1000=1750
in a calculation the number is really 1750.0 but without a decimal the Fanuc control interprets it as 1750 which should work with words where a decimal point is not allowed like your K

alternatively 7/2.8=2.5*1000=2500

however if storing numbers into macro variables is forcing the decimal point regardless of the calculation you are out of luck and nothing will work.

I have not tried it on a Fanuc control but I wonder whether direct maths would work......

G79 etc etc K[7/2.8*1000]

this type of direct calc is accepted on Okuma User Task 2.... e.g. G00 X[10.0 + 0.001]
yes I know its a different beast and yes I know Okuma is not adhering to other more widespread 'standard' control systems

[txcncman]

If I understand your question correctly, yes the Fanuc op controller is capable of running macro programs. All the 9000 programs are essentially macros. as far as my parameter settings being correct as to allow this I'm not sure. I have to crack open the manual, unless someone is familiar with these controllers.
For some reason not to many people seem to program turrets like this.

Just my opinion, but many people incorrectly refer to sub-programs as macros. Macro B (or A or C) is a specific programming language. While a sub-program, such as a O9*** can contain the Macro B (or A or C) language, it would not have to. Main programs can contain one of the Macro language statements. That does not make it a sub-program.

[CANDC]

do you really need to use 2.75?
If you use another number that divides into 7 more evenly you can do this kind of calc and it'll be a 4 digit number without decimal....

7/4=1.75*1000=1750
in a calculation the number is really 1750.0 but without a decimal the Fanuc control interprets it as 1750 which should work with words where a decimal point is not allowed like your K

alternatively 7/2.8=2.5*1000=2500

however if storing numbers into macro variables is forcing the decimal point regardless of the calculation you are out of luck and nothing will work.

I have not tried it on a Fanuc control but I wonder whether direct maths would work......

G79 etc etc K[7/2.8*1000]

this type of direct calc is accepted on Okuma User Task 2.... e.g. G00 X[10.0 + 0.001]
yes I know its a different beast and yes I know Okuma is not adhering to other more widespread 'standard' control systems

Thanks, but yes I have to use 2.75 to get the pattern I need.

[CANDC]

Just my opinion, but many people incorrectly refer to sub-programs as macros. Macro B (or A or C) is a specific programming language. While a sub-program, such as a O9*** can contain the Macro B (or A or C) language, it would not have to. Main programs can contain one of the Macro language statements. That does not make it a sub-program.

Yes, I probably mixed up my terminology. My machine uses Macro B language. But my problem is not the program as I originally thought it was. It seems to be the fact that my machine is not storing any values for the variables I am using. I read that #100 to #149 are the common variables that I should use. The P9700 program that I call in my program is to move the auto clamps into their locations. I noticed that that program uses #104 as well, I thought this might be changing my value. But there is still nothing stored for #101 or #102 or #103. I have not located any parameter that effects this yet.

[fordav11]

did you try using #500 onwards? you can use any variable that is unused even global variables.
but what you are doing is incredibly simple. macro is usually used to simply programming of a complex task.
what you are doing is overkill. if there's no easily found solution just program it normally and move on.

[fordav11]

btw, just tested today, a direct calc like 'G00 X[10.0 + 0.001]' works on Fanuc controls

[CANDC]

Thanks for the ideas everyone, It seems to be the G31 and T3 commands. Either one of these commands clears out the stored variables.
G31 and T3 before the variables works, but if located after the variables it does not.
The program below works perfectly.

O0560(HEAD JAMB)
(T3 = .265X.500 OBROUND)
G20
G90
G31T3
G65P9700A38.5B10.0
M75X65.Y51.
#101=7(WALL THICKNESS)
#102=42(OPENING WIDTH)
#103=[#102+2]
#104=[FIX[#101/2.75]]
X1.25Y2.375
G79I#103P1J2.75K#104
X1.25Y[[#101+7.0625]-4.688]
X[#102+2.25]
G28
G92X65.Y51.
M99

[cogsman1]

The 100 series variables are usually cleared at end of program and by reset. Do you see them DURING the running of the program? Use "Single block" and check while program is active. You should use the 500 series to stay after the program is completed, or change the parameters.

[xjdubber]

Hi all,

sorry to bring this post back to life, but since you all know something about strippits I'd thought I'd ask!

Working on a 1000xp/20 retrofit and would really like to know what G31 is actually good for...

[sinha_nsit]

G31 is the skip signal on Fanuc which is used for probing.

[Al_The_Man]

G31 is the skip signal on Fanuc which is used for probing.

On some Fanuc P(unch) systems, G33 is skip.
Not sure what G31 is on a punch?
Al.

[xjdubber]

G31 is the skip signal on Fanuc which is used for probing.

A Strippit cnc Punch that does probing, i'd like to see it.... nope sorry thats is definitely not it, the strippit book that i have with the machine says it calls p9010 for simultaneous x,y and t movement...

[xjdubber]

On some Fanuc P(unch) systems, G33 is skip.
Not sure what G31 is on a punch?
Al.

Hi Al,

I think i've seen you post some things here and there about camsoft, i might need some advice in the future. I'm using camsoft to replace a mac control on strippit 1000xp20

[Al_The_Man]

A Strippit cnc Punch that does probing, i'd like to see it.... nope sorry thats is definitely not it, the strippit book that i have with the machine says it calls p9010 for simultaneous x,y and t movement...

I have no idea why you would need a probe on a punch either, but some of the Fanuc P punch operator manuals show G33 as skip??
Al.

[xjdubber]

I have no idea why you would need a probe on a punch either, but some of the Fanuc P punch operator manuals show G33 as skip??
Al.

I`m probably making a mistake thinking that strippit would have had the gcodes the same for fanuc operated and macintosh operated machines..... could be that on fanuc operated machines g31 is used as m35 is on macintosh machines. which is a work clamp search routine very similiar to probing.