Laser noob would like some g code info

[tasdau]

Hi all,
My company hired me earlier this year to run their wire EDM. I have been running EDMs for many years but now they want me to run their old laser machine too which has been sitting dormant for a while. The controller is an old 160i-L Fanuc with a Windows 95 OS (that interface and those old screenshots are a blast from the past!). The program it uses is called CNCScreen (I think- I'm at home now).

There is no one there that really knows how to program for it and, of course, no manual so I am trying to learn it from looking at the old programs that are still in the machine. I recognize the motion and offset commands but there are several ambiguous g codes that I'm not familiar with. With what seemingly limited info I have found online, I think some of them are for the laser beam settings like wattage gas and duty and others are for the shutter. Specifically I would like to know what G13, G14, G32 and G24 are for and what the single letter/number combo after them represent. Most of the old programs call up sub-programs for pierce cycles. It would be great if someone could post a link for a g/m code list. I haven't been able to find much online. I can post an old program and pierce cycle if that helps you guys help me.

The type of stuff they want me to do is pretty simple so I could create the motion part of the program and just copy and paste the rest from and old similar program but I'm the type of guy who likes to know what every letter/number in a program does.

Also, I was told the machine has a "height sensing" nozzle so I assume some of those g codes might have to do with that.

Thanks in advance from a Laser Noob!

 

[Foostrap]

Some G-Codes are common to Fanuc controls. But others are machine tool builder dependent. So knowing what machine brand and model you have might help.

 

[tasdau]

I will post a sample program and the other info tomorrow.

 

[tasdau]

The machine is an iMachines i-L2500 (2KW) with a 3x4 matrix of oxygen tanks.
The laser generator is a GE Fanuc Laser C2000 Model E.

I double checked the rest of the info from my original post and it is correct.

 

[tasdau]

Here is a sample .nc file with the pierce cycle at the end.

The pictures are not of my machine but are almost identical except my controller has a trackball on it.

 

[Foostrap]

I don't know that machine tool builder, but looking at the code, I would assume this is what happens:
N2: Rapid travel to X... and Y...
N3: Z-axis goes to Z0.5
N4: Z-axis goes to 0
N5 M98 P9125. M98 calls sub-program 9125, which is the piercing in your case.

Not sure what D1 is. Maybe to turn on the cutting gas.

N7 G41 S600 P600 Q95 G1 X36.69465 F50. This must be the cut condition. S is the power. P is the frequency. Q is the duty cycle. F must be the speed.
N8 G3 is a circular cut
...
N12 G32 P0 is to turn the gas and beam off (at end of profile)
N13 G14 is to disable the tracing (sensing of the material height)
N14: similar as N3...


In the piercing sub:
G13 P1: enables sensing (head follows the material height)
G32 P1 T12 R10: Turn on assist gas 1 with pressure of 1.2 bar and preflow of 0.1 sec
G24 S300 P300 Q24 R1500: Pierce with Power of 300W, Freq of 300Hz, Duty of 24% and time of 1.5 sec (I assume the unit is milliseconds)

 

[tasdau]

Thanks for the info.

I tried some test cuts and learned a few things:
As you said, G13 P1 is height sensing on but G13 P0 (which is not in any old programs) is sensing off- I still don't know what G14 does.
D1 is the offset.

I'm curious about the power/freq/duty that is listed on N7 of the main pro. It only reads this once at the beginning, but each hole in a multi cavity program recalls the sub which has different power settings. Will the machine go back to the original power settings after the pierce? Does the G24 tell it to only use those settings for the pierce or will it just use whatever settings it read last?

 

[Foostrap]

G14 is most likely the same as G13 P0 (sensing off) in your case.
For the cutting power, freq,... it should use the same values are previously used on the N7 line. To know for sure, go to the STATUS screen where you can see the commanded power, duty, freq. You can then see if it matches the N7 line.
If it doesn't, you'll have to repeat the line "G41 S600 P600 Q95 G1 F50."

 

[tasdau]

I can MDI a G14 while head sensing is on and it does not turn it off but a G13 P0 will.

I will look up the status page while it's cutting to see if the settings go back.

The guy who made the old programs not only deleted all the G40s (except the one at the begining) but deleted the whole line. So if the next rapid move happened to be at a pretty steep angle, the part would not even cut off because the machine would just read it as a very sharp corner with an offset. Strange.

Thanks for your help Foostrap.