Macro A or B ?

[tonper]

Hello,

so I have been doing some macro programming or whatever it's called
Have only worked with CNC Machine for 3 months now so im kinda new.
Anyway I made this macro, and i was woundering if this is a Macro A or a Macro B.
I have tried understanding the difference by reading the manual but can't exactly get it.

%
:311
G00 Z2.
N13 #1=0
N15 #15=#4-#18/2
N16 G91
N17 G00 X-#15
N18 G90
N19 WHILE [#26GE#1] DO 1
N20 #5=#1
N21 G02 Z-#1 I#15
N22 #1=#1+#3
N23 END 1
N24 IF [#5EQ#26] GOTO 31
N25 #12=#26-#5
N26 #7=#12/2
N27 WHILE [#5LT#26] DO 2
N28 #5=#5+#7
N29 G02 Z-#5 I#15
N30 END 2
N31 G02 I#15
N32 G91
N33 G02 X#15 R#15/2
N34 G90
N35 G00 Z5.
N38 M99
%

So, could anyone please tell me if my macro is a A or B macro. And what makes it A or B? Or maybe just explain the difference in simple english

Thanks in advance!

[beege]

Looks to me like Macro B. Macro A uses G65H### to describe an if or conditional branch line. Harder to decipher without memorizing H P and Q word meanings

[tonper]

Originally Posted by beege Macro A uses G65H###

Thanks.

But this sounds a bit like my macro

I use "G65 P311 I9. C0.5 Z32. R12." in main program to call this macro.
The macro itself makes a "well" with a mill. Not so good with english milling terms. But a "well" for a screw head etc.

I = Radius of Well
C = mm to go down in Z-axis per orbit
Z = Depth of well
R = Diameter of mill tool

[beege]

Yes G65 is "macro call", but you can't use words like "IF" and "#1=#1+3" using Macro A. Those are replaced with G65 statements.
With both MacroA and MacroB, you call the macro up from the G65 P#### where P#### is the program number for your macro, and the rest of the words in the line transfer numbers to you macro. It's the "H" in the other G65 lines that tell the program what to do with the number in P or Q using Macro A. Confusing? That's why MacroB was developed, and you have MacroB used in your example.

[stevo1]

Beege is correct you are using macroB no question. As he has stated you can’t use IF,WHILE,LT,GOTO statements in macroA. MacroA is a whole different breed and wisely macroB was developed.

If you are already programming this way and using macroB don’t even look back at “A” keep trucking forward....it’s not even worth the time.

Stevo

[tonper]

Originally Posted by beege Yes G65 is "macro call", but you can't use words like "IF" and "#1=#1+3" using Macro A. Those are replaced with G65 statements. With both MacroA and MacroB, you call the macro up from the G65 P#### where P#### is the program number for your macro, and the rest of the words in the line transfer numbers to you macro. It's the "H" in the other G65 lines that tell the program what to do with the number in P or Q using Macro A. Confusing? That's why MacroB was developed, and you have MacroB used in your example.

Aha!
No, now it's not confusing at all. Thats was the best answer possible I think
Understand it crystal clear now. Thanks alot

[charger19690]

Thanks for this thread, I have been wondering the absolute difference between A & B and being a programmer at work, we just use variable programming from time to time, so that's what I call it. I have seen an "A" program from time to time and it looks foreign to me.

So now when I get asked, I will have the right answer between the 2. Macros can be very powerful stuff, I actually love when I get to use them.

cncmike
http://www.cncbasics.com
http://www.cncbasicsforum.com