fanuc macro b

[Josh Kinney -Elite Engineering]

Guys,

Is there anyway to write multiple variables on one line?

 

Like:

 

#510=1 #515=0 #516=0 #517=1

 

I can't find a way and my macro b book doesn't say anywhere that I can find.

 

Thanks,

 

Josh-

[crazy^millman]

Josh, not that I am aware of they must be defined on a line by themselves.

[Guest]

Any particular reason you want them all on one line anyway?

[Josh Kinney -Elite Engineering]

Josh, not that I am aware of they must be defined on a line by themselves.

Thanks Ron.

[Josh Kinney -Elite Engineering]

Any particular reason you want them all on one line anyway?

Just to keep things clean. I'm passing through the work offset and toolplane coordinates to a sub program and wanted it on one line if possible. It would lessen the chance someone edited the wrong line.

 

Josh-

[Tim Johnson]

You could write the pass-through code to another subprogram. If someone needs to edit the code it's all in one spot.

[TerryT]

Here's something for you to look at. The operator's  place their offset changes in the top part of this main program. It has a built in safety check to make sure no one fat fingers a number.Example.txt

[Josh Kinney -Elite Engineering]

I'm pretty happy with how I have it now. If I could put them on one line it would be nice. Just thought I would ask the old timers....

 

I'll post up mys code structure Monday.

 

Josh-

[Allan]

Like Tim says

 

How about using a G65 call and using the local variables #1 thru #33 set your values A,B,C,D ect...

then in your macro sub program

#510 EQ #1 (Value of A in the G65 Call)

#511 EQ #2 (Value of B in the G65 Call)

 

Then you get all your variables on one line and error checking like in the TerryT example.

[AlbertZini]

http://www.emastercam.com/board/topic/76926-cool-macros/?p=974228

[Josh Kinney -Elite Engineering]

I'll look into that tomorrow. That sounds doable.

 

Instead of

#510=1.

#515=0.

#516=0.

#517=1.

M98P9999

 

It would be G65P9999W1.X0.Y0.Z1. And then just reference the local variables once inside P9999.

[Guest]

If you're going to pass the values through for something else then you could just create a MACRO G/MCode. For example

 

G154 Xn Yn Zn An Bn Cn In Jn Kn

 

O9011(G154 Macro)

 

(SET PARAMETER #6051=154)

 

#501=#24

#502=#25

#503=#26

 

#504=#1

#505=#2

#506=#3

 

#507=#4

#508=#5

#509=#6

M99

 

HTH

[cncchipmaker]

Guys,

Is there anyway to write multiple variables on one line?

 

Like:

 

#510=1 #515=0 #516=0 #517=1

 

I can't find a way and my macro b book doesn't say anywhere that I can find.

 

Thanks,

 

Josh-

Have you tried using a while/do?

 

Check out this example:

 

#100=532.

WHILE[#100LT899.]DO1

#[#100]=#0

#100=#100+1.

END1

 

Basically what happens here is that #100 is set to your first variable that you want to set and 899. is the last variable to set. All of the variables inbetween the two get set to #0 which is null. Of course this will only work for you if you are setting everything the same.

[Josh Kinney -Elite Engineering]

We have subplates and charts that map out every location with a number. In the past we've typed in the values from the chart. Say X-12, Y-10, Z-21.1319. Now you can just type the vise location number. MasterCam outputs the incremental shifts from top of vise (Top WCS in MCX) to get to your toolplane.

 

Her'es what I got. The G65 calls are W=Work offset (G10 offset, 1=54), XYZ are incremental to toolplane.

 

%

O0123 (T)

(POST REV 1.1)

(DURACENTER 5 - VMC)

(MCX FILE   - T)

(DATE       - MAR-23-2015)

(TIME       - 7:57 AM)

(USER ID    - ***)

(OPERATIONS - 50/60/70)

 

 

#510=1(OPTIONAL N SEQ START)

 

IF[#510EQ1]GOTO3000

M0

(USING OPTIONAL N SEQ START)

M0

(YOU ARE STARTING PART WAY THROUGH)

N3000

 

(***  TOOL LIST  ***)

(T1   - 0.125 CHAMFER MILL   - D0.1250)

 

(***  OVERWRITE MACRO ADJUSTMENTS  ***)

 

G90 G52 X0. Y0. Z0.

 

(***  USER DEFINED WORK COORDINATES START  ***)

 

M01 (MAKE SURE YOU SET YOUR VISE LOCATIONS FROM THE CHART)

 

( G54 VISE LOCATION NUMBER )

#550=0. (NUMBER FROM CHART - THIS IS ALL YOU NEED)

 

#517=0. (X AXIS INCREMENTAL SHIFT)

#518=0. (Y AXIS INCREMENTAL SHIFT)

#519=0. (Z AXIS INCREMENTAL SHIFT)

 

( DONT TOUCH )

G65P9999W1.X2.Y-1.5Z1.

 

( G55 VISE LOCATION NUMBER )

#550=0. (NUMBER FROM CHART - THIS IS ALL YOU NEED)

 

#517=0. (X AXIS INCREMENTAL SHIFT)

#518=0. (Y AXIS INCREMENTAL SHIFT)

#519=0. (Z AXIS INCREMENTAL SHIFT)

 

( DONT TOUCH )

G65P9999W2.X2.Y-1.5Z1.

 

(***  WORK COORDINATES END  ***)

 

GOTO #510 (JUMP TO SEQ)

 

 

M01

N1(Sequence #1.)

(TOOL# 1 - 0.125 Chamfer Mill)

(OP  1 )

(MAX - Z0.)

T1 M06

G0 G17 G90 G54 X-2. Y1.5 S6000 M03

G43 H1 Z1. M8

 

 

Here's the Sub:

 

% 

O9999(MACHINE ZERO SHIFT)

 

(N40 - DURACENTER 5 - VMC) 

 

#551=-21.3139(MACHINE Z-ZERO - SUBPLATE) 

#552=-9.9995(MACHINE Y-ZERO - SUBPLATE)

#554=-1. 

IF[#550EQ1.]THEN#553=1.

IF[#550GT1.]THEN#553=[#550*2]+#554 

IF[#550LT1.]GOTO1000 

IF[#550GT16.]GOTO1000

 

G90G10L2P#23X-#553Y#552Z#551

G91G10L2P#23X#24Y#25Z#26

G91G10L2P#23X#517Y#518Z#519 

 

 

M99

N1000#3000=10(INCORRECT VISE LOCATION NUMBER)

M30

%

[Josh Kinney -Elite Engineering]

Operator loads the vise in one of the pinned locations, types in the number and hits cycle start.

[soymilk]

nice, I really like the creativity.  Here's my take on it.  About the same thing but written different just for kicks.  I normally use 8000 program numbers for in house macros, and leave 9000 for system/builder macros.  Unless I make my own G/M code like foghorn mentioned.  Used more local variables.  I also rolled in the #550 macro as variable V.  

 

O8050

#5=-9.9995 (MACHINE Y-ZERO - SUBPLATE)

#6=-21.3139(MACHINE Z-ZERO - SUBPLATE) 

IF[#23LT1]THEN#3000=1 (ERROR WORKOFFSET SET LOWER THAN 1 -G54)

IF[#23GT6]THEN#3000=2 (ERROR WORKOFFSET SET HIGHER THAN 6 -G59)

IF[#22LT1.]THEN#3000=3 ( ERROR PIN LOCATION LESS THAN 1 )

IF[#22GT16.]THEN#3000=4 ( ERROR PIN LOCATION MORE THAN 16 )

 

(SETS X WORK OFFSET)

#1= [#23*20]+5201 

#[1]=[[#22*2]-1]

#[1]=#[1]+#24

 

(SETS Y WORK OFFSET)

#2= [#23*20]+5202

#[2]=#5+#25   

 

(SETS Z WORK OFFSET)

#3= [#23*20]+5203 

#[3]=#6+#26   

M99

 

Another idea would be to have all the code you want the operator to edit in one spot.  That way they don't have to hunt around. 

 

O0123 (T)

(POST REV 1.1)

(DURACENTER 5 - VMC)

(MCX FILE   - T)

(DATE       - MAR-23-2015)

(TIME       - 7:57 AM)

(USER ID    - ***)

(OPERATIONS - 50/60/70)

 

(*******EDIT ONLY HERE ********)

(V = VISE POSTION)

(W = WORK OFFSET G54=1, G55=2, etc)

 

G65 P8050 V1 W1. X2 .Y-1.5 Z1. (G54)

G65 P8050 V2 W2. X2. Y-1.5 Z1. (G55)

(*******EDIT ONLY HERE ********)