Macro alarm "009 ILLEGAL ADDRESS INPUT"

[theemudracer]

First I want to thank everyone who helped me get this far but apparently I am missing something. I am trying to engrave on the O.D. of a piece of 2." round stock on my Lathe.

Have a look at the macro prg. below and that part prg. and tell me if you guys see whats wrong.

It gives me a "009 ILLEGAL ADDRESS INPUT" ALARM.

I am trying to take the Y values in my prg and convert them to C-Axis moves in degress with the macro.


Macro prg below....
%
O9100(2.00 DIA MACRO CALL)

G01C[#25*.0174]

M99
%





Part prg below.....


%
O1569(OVAL)
N2#501=2.00
N3#502=[501+.1]
N4G10L2P01X0.Z-23.4684
N5G10L2P02X0.Z-3.0123
N6G10L2P03X0.Z-20.4684
N7G10L2P04X0.Z-12.1784
N8G10L2P05X0.Z-5.3333
N9G11
N10/2M98P9998
N12M118
N13G28U0
N14G28B0
N16G99
N17G54M54
N18
N19(CHAMFER)
N20G50G99
N21S3000
N22T1010G54
N23G0G96S1000M3
N24Z0M8
N25X2.1
N26G1X-.07F.006
N27G0W.05X1.7069
N28G42G1Z0.F.006
N29G3X1.7634Z-.0117R.04
N30G1X1.9766Z-.1183
N31G3X2.0Z-.1466R.04
N32G1G40X2.1
N33G28U0M9
N34G97
M05
M01



T1213
G98
G54
G0X0.Z.1
M69
G04P0500
G01Z4.0F500.
M68
G4P0500
G0W.1
G28U0.




G98
N39T0505(BALL END MILL)
N40M43
N41G56G0C0.
N42G97S4000M13
N43G0Z0.
G0X2.1
G01X2.F20.


G66P9100Z.0002Y.0117 This is where it alarms out....


N56Z.0007Y.0233
N57Z.0017Y.0349
N58Z.003Y.0466
N59Z.0046Y.0582
N60Z.0067Y.0698
N61Z.0091Y.0814
N62Z.0118Y.0929
N63Z.015Y.1044
N64Z.0185Y.1159
N65Z.0223Y.1274
N66Z.0266Y.1388
N67Z.0312Y.1502
N68Z.0361Y.1615
N69Z.0414Y.1728
N70Z.0471Y.184
N71Z.0531Y.1952
N72Z.0595Y.2063

The prg goes on for another 1600 lines....

thanks Jon Thee

[CNCRim]

Originally Posted by theemudracer G66P9100Z.0002Y.0117 This is where it alarms out....

I don't think you can use the letters that use as machine command address like G O Z Y X H few others.

[CBNDude]

Have you tried it this way?

%
O9100(2.00 DIA MACRO CALL)
#503=[#25*.0174]
G01C#503
M99
%

[CBNDude]

Missed read program to start so skip me first post..


Question- Are wanting the Z and Y to feed at same time as C?
If so The Z and Y move needs to be on same line as C.

G01C[#25*.0174]Z.0002Y.0117

[theemudracer]

Originally Posted by CBNDude Missed read program to start so skip me first post.. Question- Are wanting the Z and Y to feed at same time as C? If so The Z and Y move needs to be on same line as C. G01C[#25*.0174]Z.0002Y.0117

My lathe only has Z, X and C with a sub spindle B.

I am wanting to take the Y axis moves in the prg and feed C axis in degress in its place.

thanks Jon

[Dan Fritz]

The Y address may not be permitted on a lathe. For the purpose of calling a macro, you can use any other address that permits decimal points, like "A".

Also, CBNDude is right. If you want the Z axis to move also, you've got to make it move in the macro. The G66 macro call will just pass the numbers to the macro, and it won't move the axes at all. Try this to call the macro:

G66P9100Z.0002A.0117

Then, inside macro 9100, move both the Z and the C axes with a single G01 command, like so:

G01C[#1*.0174]Z#26

There should be a chart in the front of your operator's manual that will tell you the legal addresses, and it will also tell you which addresses can use decimal point formatted numbers and which ones are simple integers. For example, an address X, Y, Z, U, V, U, or A, B, or C should accept decimals. The addresses M, T, S, etc. are integers. Your lathe may not permit the addresses Y, B, or V because this axis doesn't exist on your machine.

Just a guess ...

[theemudracer]

ok that makes sense now.

I will report back after christmas.

thanks again
Jon

[M-man]

I dont think it is possible to do this on a fanuc 18IT.. Mabe it is possible to scale one axis (c-axis) (mabe scale it in the text producing prg).and change the Y to C in a simple text editor..