need help with a macro

[Bomcc]

I am new to programming macros (bought a book about a week ago) and have decided to take a stab at writing some of my own. I am writing one to tornado mill since we use a ton of it in the shop and chasing all the little subs we use to currently do it is beginning to get a bit overwhelming. The machine is a Toyoda FH450S that is running a FANUC 31i controller. My coding is as follows maybe someone can tell me what im missing???

lead in...

G90 G54.2 P8 X0Y0
G43H20Z1.M3S500
Z.1
M8
G65P8023 H5. D2. Z.05 F100.

========>

O8023
(TORNADO MACRO START AT CENTER OF HOLE)
(H=FINISH HOLE DIAMETER)
(D=TOOL DIAMETER)
(Z=FEED PER REV IN Z AXIS)
(F=FEEDRATE)
(R=REPEAT)

#10=#4003

#33=0(RESET COUNTER)
#25=[#11-#7]/2(H MINUS D/2)
#5=#25
#26=ABS[#26]
#14=ABS[#26*#18]

G91
Y-#25
WHILE[#33 LT #18]DO1
G3 X0 Y0 Z-#26 I0 J#5 F#9
#33=#33+1(ADD 1 TO COUNTER)
END1
Y#25(MOVE UP)
G0
Z#14(RAPID BACK TO START POINT)
GOTO9999

(ALARM)
(ALARM)

N9999G#10
M99
M1
M30
%


Anywho anyhelp would be awesome i feel like im just missing something extremely simple.

[txcncman]

You use the word tornado. I assume this is for spiral milling. For basics, this seems like it will do what you want it to do.

Things to consider:

You are not going to have a smooth lead in and lead out and this will not do a finish pass for a flat bottom hole.

Also, this does not allow you to adjust with cutter compensation using your tool offsets.

[Bomcc]

Excellent. Typically we are only roughing in thru holes in castings with it but yes, I should add a finish pass at the bottom of the hole.

Quick q, I put this in my controller but its giving an alarm, incorrect syntax or something of that nature. Is there anything funny looking with my code??

[txcncman]

What line did it stop on? Look at that line and then up to 3 lines ahead. Usually the control will stop before it actually gets to the bad line.

I do not see anything that jumps out at me as being incorrect. Run every thing high and comment out one line at a time until you find the culprit.

[fordav11]

it could be your G3 line. you are moving in an arc XYZ.
maybe the machine doesn't have helical interpolation option?
or G54.2 P8 ?

[txcncman]

Originally Posted by fordav11 it could be your G3 line. you are moving in an arc XYZ. maybe the machine doesn't have helical interpolation option? or G54.2 P8 ?

ford, good call. I am betting he needs to add K at minus 1/2 of the Z move. The center of the arc is moving down. I ran into this when writing my spiral taper software. Which should be ready for purchase as a stand-alone program by the end of the week.

[Bomcc]

Interesting. I never have to write that k move in normally but maybe within the macro things are different???

[fordav11]

it looks like there's a bug in your program logic.
the loop ends at END1 when #33 => #18
the next line is Y#25(MOVE UP)
but you don 't give it a G00/G01. you have left the program in G03

Since G03 is modal the code would be G03 Y#25 which is not expected behavior?
So maybe the error is the machine is trying to cut in G03 without a proper end point or radius center point?

[Bomcc]

Duh.... excellent. Ill bet that's it. I knew it was something silly. Thanks a ton:-)

[Bomcc]

Maybe someone could tell me..... is there a way to eliminate the "stall" while its looping without programming it longhand??

[beege]

Also, you have "#18" which is R, and no R in the G65 line above. You should have a default #18 of maybe 1 if someone doesn't program the R in that line.

[anand76767]

bomcc,
your are missing the r point (means from where the feed should start) thats denote as #18 as well as pl check z this is not the feed per rev this is the final depth of hole.
hi pl see below in your prg for change

G90 G54.2 P8 X0Y0
G43H20Z1.M3S500
Z.1
M8
G65P8023 H5. D2.R5.0Z-5.0 F100.

========>

O8023
(TORNADO MACRO START AT CENTER OF HOLE)
(H=FINISH HOLE DIAMETER)
(D=TOOL DIAMETER)
(Z=FEED PER REV IN (FINAL DEPTH)
(F=FEEDRATE)
(R=REPEAT)

#10=#4003

#33=0(RESET COUNTER)
#25=[#11-#7]/2(H MINUS D/2)
#5=#25
#26=ABS[#26]
#14=ABS[#26*#18]

G91
Y-#25
WHILE[#33 LT #18]DO1
G3 X0 Y0 Z-#26 I0 J#5 F#9
#33=#33+1(ADD 1 TO COUNTER)
END1
Y#25(MOVE UP)
G0
Z#14(RAPID BACK TO START POINT)
GOTO9999

(ALARM)
(ALARM)

N9999G#10
M99
M1
M30