[James3BT]

Hello,

Any help much appreciated i have been on this for days and can't figure it out.
A simple program made in Cambam software.
Startup machine - reference, load program, cycle start - runs fine.
Press start a second time (or load a different program and press start) and ALARM - INVALID I,J OR K IN G02 OR G03 (error 304).

The program just completed the cycle fine - there are clearly no issues with the numbers being invalid.
If I power cycle the machine it will run the program (or other similar program) fine again.
Try to run it again and error 304 comes up.

If anyone knows of a solution it would be greatly appreciated.
thank you.

[djm77]

Is there an issue with absolute and incremental programming in your program. G90/G91. The program may run the first time, but if you still have G91 programmed it may not be able to run the program a second time from the machines position.

When you try to run it the second time, does it actually start the program, then get to a point before it alarms out or will it fail to even start?


Sent from my iPad using Tapatalk

[extanker59]

Are the cutter comps cancelled after every tool?

[LeWhite]

Your program just stops. You need to add shut down lines like G01 G90 G28 Z0.0 M30 ect. On the current commands screen there is a section where it lists codes in use. Copy these codes from your first run attempt and then from your second attempt. The difference is where your problem is.

[mactec54]

Hello,

Any help much appreciated i have been on this for days and can't figure it out.
A simple program made in Cambam software.
Startup machine - reference, load program, cycle start - runs fine.
Press start a second time (or load a different program and press start) and ALARM - INVALID I,J OR K IN G02 OR G03 (error 304).

The program just completed the cycle fine - there are clearly no issues with the numbers being invalid.
If I power cycle the machine it will run the program (or other similar program) fine again.
Try to run it again and error 304 comes up.

If anyone knows of a solution it would be greatly appreciated.
thank you.

Best to post your program anyone with a Haas can then see what it may be that is causing the problem

[dertsap]

the g2 might be staying modal . put a g0 in the top line along with the g90g21g17 etc . The code from cambam looks pretty bad , and theres no g43 h call

[mactec54]

James3BT

Yes not really suitable for a Hass Control

This is what it should look like to run, I did not check or run it but the start and end was messed up as it was and no Tool offset call which is needed to run a part ( G43 and H 18 tool number ) a simple program below as well clean and reliable

%
O11115
( CAMBAM )
( T0 = 18 )
G21 G90 G40 G17G80
T18M6
M8
G54
S1000 M3
G90G00 X4 Y0
G43 Z1.4H18 ( Check that you have set your tool length for tool 18 )
G01 F300 Z0
G02 F800 X-2 Y-3.464 I-4 J0
G02 Y3.464 I2 J3.464
G02 X4 Y0 I2 J-3.464
G01 F300 X22
G02 F800 X-11 Y-19.053 I-22 J0
G02 Y19.053 I11 J19.053
G02 X22 Y0 I11 J-19.053
G01 F300 X40
G02 F800 X-20 Y-34.641 I-40 J0
G02 Y34.641 I20 J34.641
G02 X40 Y0 I20 J-34.641
G01 F300 X58
G02 F800 X-29 Y-50.229 I-58 J0
G02 Y50.229 I29 J50.229
G02 X58 Y0 I29 J-50.229
G0 Z3
M9
M5
M30
%


%
O4066
N1G17G40G80
T4M6
M8
G54
S2850M3
G90G0X-.0962Y-.1178
G43Z.1H4
G1Z-.55F20.
G3I.0962J-.0457F8.
G0Z3.
M9
M5
G53Y0.
M30
%

[djm77]

Just edit your post processor to create the program exactly as you want it. We changed ours to look like as if we had written it long hand, that way it's easy to understand, and you know exactly what it should be doing and when.


Sent from my iPad using Tapatalk

[chineshop_guy]

i see this problem from time to time usually has to do with a g18 or g19 being posted and then you try to do a radius in the x,y plane (g17), and g18 or g19 is active.
check your current commands to see what is active when te machine alarms out

[mactec54]

i see this problem from time to time usually has to do with a g18 or g19 being posted and then you try to do a radius in the x,y plane (g17), and g18 or g19 is active.
check your current commands to see what is active when te machine alarms out

He has a G17 in his program so is nothing to do with what plane is active, his program is not formatted correct, most controls would have a hard time trying to run a program formatted like this

[James3BT]

Thanks for your help all.
Mactec54, yes - that code is much better thank you.
After a lot of chopping and changing it appears to be the "G53 Z0" command on line 6 which is the problem.
This has stopped the problem in the initial code.
I will see if I can update the post processor to be more like the suggested code.
Thanks,
James

[beege]

The G53Z0 is NOT the problem. The problem is the G2 at the end of the program. G2 is modal (clockwise arc). Any movement command (like G53Z0 or X10.Y10.) while G2 is active, requires a valid arc or circle center in order to complete the command. What is needed is a G00 or G01 to eliminate the requirement for a circle definition in the next move command, either at the end of the program, or at the beginning of the program or before any next move (like a tool change)

[mactec54]

The G53Z0 is NOT the problem. The problem is the G2 at the end of the program. G2 is modal (clockwise arc). Any movement command (like G53Z0 or X10.Y10.) while G2 is active, requires a valid arc or circle center in order to complete the command. What is needed is a G00 or G01 to eliminate the requirement for a circle definition in the next move command, either at the end of the program, or at the beginning of the program or before any next move (like a tool change)

As it was Programed the G53Z0 would not work in a Haas Control, it has to have a G0 before it is executed, or a G0 in the same line, you also would not want to do this before a Tool Change at the start of a Program, the Tool Change was also messed up, which is all that is needed for a Haas to be at Z0 is a simple T1M6, or the Tool number you want