Newbie- Macro problem with Haas VF-1 and HS-1

[colton_m]

Hello everyone,

I'm having some problems and am hoping someone could shed some light. I will start off with what I am trying to accomplish:

I am trying to write a program such that the machine will execute a courtesy line (returning the table to in front of the machine doors) ONLY when optional stop is activated. This would be for set-up purposes only so I can inspect/measure the part after each operation during the first setup WITHOUT manually jogging the table back to the doors after the M01 commands are read.

Below is the program I have come up with so far, I have excluded the actual machining for simplicity but it demonstrates my idea pritty well:

%
O0001 (MACRO TEST)

N1 (MACHINING OPERATION 1)
T1 M06
S1000 M03
<MACHINING CODE HERE>
G91 G28 Z0.
IF [ #3033 EQ 1.0 ] GOTO100
N10 M01

N2 (MACHINING OPERATION 2)
T2 M06
S500 M03
<MACHINING CODE HERE>
G91 G28 Z0.
M30

N100 (TABLE RETURN)
G91 G28 Y0.
G91 G28 X12.
GOTO10
%

But now the headache haha,

I have run this program on a HAAS simulator and it works flawlessly which is great! However, the shop floor is a different story. The Newer VF-1 I have access to does not have the Macro option enabled so that machine wont work. But I do have access to an older VF-1 and HS-1 Horizontal with the Macros enabled . But in the older machines the system variable #3033 (op stop) does not work. I get an "Illegal Macro Variable ALARM".

I am wondering if anyone knows what the variable for optional stop would be on these older machines? Or how I could find out? I'd really like to give this a try!

Or when push comes to shove if anyone could suggest a better way of having the table center itself ONLY when op stop is pressed it would be greatly appreciated.

Thanks,
Colton M.

[Donkey Hotey]

Why not just do block delete with the machine coordinates you want?

/G53 X-10.0 Y0.0 Z0.0
/M00
(Flip part over, then push the green button, dummy)

[colton_m]

Originally Posted by Donkey Hotey Why not just do block delete with the machine coordinates you want? /G53 X-10.0 Y0.0 Z0.0 /M00 (Flip part over, then push the green button, dummy)

Three reasons:

1. I am using a block delete on all the M08 coolant commands to avoid soakage while the door is open when proving the program. But when I actually let the part run for the first time I wouldn't want the coolant to be skipped.

2. I am trying to link this table courtesy motion directly to the op stop button being pressed or not. Just for ultimate set-up efficiency.

3. I'm learning all this in school right now and it would be much more satisfying to make it work than to find a way around it I'm paying them, they aren't paying me... Yet

Thanks for the suggestion though.

- C

[chucker]

You could right a 9000 program and call it from a M code and in the 9000 program have your move to the doors them a M00 or M01 then it would return back to your main program

[dcoupar]

According to the manual there is no system variable for the optional stop switch on the older controls. The system variables stop at #3006.

[MKproto]

Run a sub program with a macro call out via m97 or g65 and the sub program sends it home then you just need a #xx=1do 1, elsedo2

[Dane Lindon]

IF [ #3033 EQ 1.0 ] GOTO100

This syntax doesn't look right.
try
IF[#3033EQ1]GOTO100

Here is something else to think about, it is a macro used for a automatic door, maybe it will help.

%
O0001 (MACRO TEST)

N1 (MACHINING OPERATION 1)
T1 M06
S1000 M03
<MACHINING CODE HERE>
G91 G28 Z0.
M98P8998(DOOR OPEN)
M01

N2 (MACHINING OPERATION 2)
T2 M06
S500 M03
<MACHINING CODE HERE>
G91 G28 Z0.
M30
%

%
O8998(DOOR OPEN)
(DOOR OPEN MACRO.NC)

N1(CONFIRM STATUS)
IF[#109EQ1]GOTO3
IF[#109EQ2]GOTO2
#109=#108(SET 1=OPEN 0=RUN)
M99

N2(DOOR OPEN #109=1)
M5
M85
#108=1(OPEN DOOR UNTIL #109=1)
#109=#108(SET 1=OPEN 0=RUN)
M99

N3(DOOR OPEN #109=0)
M5
M85
#108=0(OPEN DOOR ONCE)
#109=#108(SET 1=OPEN 0=RUN)
M99
%

Good luck.