Charmiles robofil 440 Zero point problem!!

Hello to everyone,
We have charmiles robofil 440 machine, and when we set the zero point on the part and start the program everything works just fine, but when we cancel the program and start it again the zero point of the part changes.

Here is my program code maybe there is any M or G code that cancels it when i load the program?


%
O0001
N100 G0 G21 G90
N110 G92 X0. Y0. Z250.
N120 G0 X-18.4142 Y-.588
N130 M60
N140 M35
N150 M81
N160 S501 N170 G41 G1 X-7.5 Y-7.5 Z0.
N162
N164
N166
N180 X27.5
N190 G40 X-18.4142 Y-.588
N200 G41 G1 X-7.5 Y-22.5
N210 X27.5
N220 G40 X-18.4142 Y-.588
N230 G41 G1 X-7.5 Y-37.5
N240 X27.5
N250 G40 X-18.4142 Y-.588
N260 G41 G1 X-7.5 Y-52.5
N270 X27.5
N280 G40 X-18.4142 Y-.588
N290 G41 G1 X-7.5 Y-67.5
N300 X27.5
N310 G40 X-18.4142 Y-.588
N320 G41 G1 X-7.5 Y-82.5
N330 X27.5
N340 G40 X-18.4142 Y-.588
N350 G41 G1 X-7.5 Y-97.5
N360 X27.5
N370 G40 X-18.4142 Y-.588
N380 G41 G1 X-7.5 Y-112.5
N390 X27.5
N400 G40 X-18.4142 Y-.588
N410 G41 G1 X-7.5 Y-127.5
N420 X27.5
N430 G40 X-18.4142 Y-.588
N440 G41 G1 X-7.5 Y-142.5
N450 X27.5
N460 G40 X-18.4142 Y-.588
N470 G41 G1 X-7.5 Y-157.5
N480 X27.5
N490 G40 X-18.4142 Y-.588
N500 G41 G1 X-7.5 Y-172.5
N510 X27.5
N520 G40 X-18.4142 Y-.588
N530 G41 G1 X-7.5 Y-187.5
N540 X27.5
N550 G40 X-18.4142 Y-.588
N560 G41 G1 X-7.5 Y-202.5
N570 X27.5
N580 G40 X-18.4142 Y-.588
N590 M50
N600 M30
%

The program you have shown has a G92 resetting position at the beginning. Its doing what its supposed to.

iirc
I believe you need to set "Points sep,cp1" on the Charmilles and have a "GOP,1" in the command file?

Unless you are just running the iso file then all that should be in the iso file. Someone please correct me if I'm wrong.

The program ends with the machine at location "N580 G40 X-18.4142 Y-.588", then that locate is set to X0 Y0 when the program is ran again with "N110 G92 X0. Y0. Z250"
To avoid this always send the machine to a known location before running G92, i.e. G00 X1. Y1., then G92 X1.Y1. where I used locations other than 0,0 for demonstration purposes.

Red James said:

The program ends with the machine at location "N580 G40 X-18.4142 Y-.588", then that locate is set to X0 Y0 when the program is ran again with "N110 G92 X0. Y0. Z250"
To avoid this always send the machine to a known location before running G92, i.e. G00 X1. Y1., then G92 X1.Y1. where I used locations other than 0,0 for demonstration purposes.

Click to expand...

I find out what to do i am doing like you said before, i change the g92 to g0 in the program begining, but the other problem is that the graphic now is not same as the program

this is what i change in the program begining :
%
O0001
N100 G0 G21 G90
N110 G92 X0. Y0. Z250.
N120 G0 X-18.4142 Y-.588

i change to this

%
O0001
N100 G0 G21 G90
N110 G0 X0. Y0. Z250.
N120 G92 X-18.4142 Y-.588

xal3r said:

I find out what to do i am doing like you said before, i change the g92 to g0 in the program begining, but the other problem is that the graphic now is not same as the program

this is what i change in the program begining :
%
O0001
N100 G0 G21 G90
N110 G92 X0. Y0. Z250.
N120 G0 X-18.4142 Y-.588

i change to this

%
O0001
N100 G0 G21 G90
N110 G0 X0. Y0. Z250.
N120 G92 X-18.4142 Y-.588

Click to expand...

You need to realize that G92 sets the current machine location to whatever the numbers are in the X,Y of the G92. Your line N120 changes the X0 Y0 location to X-18.41472 Y-0.588

The G92 location is the RE-THREAD location, as well as useful for setting coordinates. THE G92 SETS THE COORDINATES TO THE CURRENT MACHINE POSITION TO BE WHATEVER THE ARGUMENTS IN G92 LINE ARE. So your correction still changes location. If this is what you intended, fine, but I suspect it is not.

You need to be at the program start point before the G92 line.

You can return there just before the M30, before the G92, or manually between cuts.

If you are stopping the program before completion you will need to return to X0. Y0. manually or:

%
O0001
N100 G0 G21 G90
N105 G0 X0. Y0. Z250.
N110 G92 X0. Y0. Z250.
N120 G0 X-18.4142 Y-.588


Why are you cancelling the program and restarting?

Does your 440 have "resumption of cutting"?

KilrB said:

You need to be at the program start point before the G92 line.

You can return there just before the M30, before the G92, or manually between cuts.

If you are stopping the program before completion you will need to return to X0. Y0. manually or:

%
O0001
N100 G0 G21 G90
N105 G0 X0. Y0. Z250.
N110 G92 X0. Y0. Z250.
N120 G0 X-18.4142 Y-.588


Why are you cancelling the program and restarting?

Does your 440 have "resumption of cutting"?

Click to expand...

We just bought the machine couple days ago thats why i was canceling the problem, but right now the problem i solved with going to the starting problem in the program begining, but now my big problem is that program graphic is showing the wrong position i mean that the program runs corectly but the program graphic shows wrong direction.