Probing code help

cncburn

cncburn
I have a new post set up for my Plasma. I am trying to get the code to do an initial Torch Touch and set zero; then at each power cycle (to the plasma), repeat the torch touch cycle. This will allow for any warping or twist of the sheet metal. I am having a bit of trouble. I have tried several variants of the code including adding or removing G0 /G1 commands. The code runs properly for the first touch cycle, but seems to skip over subsequent touch cycles. Can you take a look at the code and suggest what might be wrong?

I am including a simple part with code as an example. Thank you.
 

Attachments

  • 1001.nc
    916 bytes · Views: 15

jolbas

Jolbas
You should remove "G0" from the probing lines.

E.g: Change

N23 G0 G38.2 Z-2.5 F15.

to

N23 G38.2 Z-2.5 F15.
 

cncburn

cncburn
Thank you for the advice Jolbas,

I tried removing the G0 from the probe lines. The result is that the Z axis does the first Touch, sets zero, but then retracts up about half way (up to original 0), and freezes with a Touch Error. Other variations on the G0 on the first Probe line but not on the second, or on the second but not on the first, result in different lockups. The closest that I have to a working program is the 1001withG0.nc file. It runs completely, except that it skips the second probe cycle. I am including the modified post (without the G0's) here. FYI I am running PLASMA V3.39.
 

Attachments

  • 1001withG0.nc
    916 bytes · Views: 14
  • 1001minusg0.nc
    907 bytes · Views: 12

jolbas

Jolbas
You say it works on the first probe cycle:

N18 G38.2 Z-7.5 F15.

And then it doesn't work the other:

N23 G0 G38.2 Z-2.5 F15.

N38 G0 G38.2 Z-2.5 F15.

Maybe Z is to high on the second and third probe instruction. I think it should not refer to the temporary offset Z but machine Z

I think it's not a good idea to have several g-codes on the same line. You have it on N11 and N16 too.
 

jolbas

Jolbas
G91 doesn't take coordinates. This row:

N59 G91 Z2.

Maybe you mean to move up by 2 inches. If so you should change it to two lines:

N59 G91

N60 G0 Z2.
 

cncburn

cncburn
Jolbas,

That sounds like a plausible solution. I will play with it a little. I used -2.5 on the second probe cycle, because the Z is at a very low position already. I did not take into account that the -2.5 may be running up to -2.5 (instead of down an additional 2.5)

I also understand that in some instances, subsequent G0 commands can cancel out previous Modal inputs.

The multiple G codes on the same line are mostly generated by the Fusion 360. They seem to work fine with previous versions of this post. But if nothing else fixes the issue, I can modify the POST to print out the code on individual lines.

Updates soon

Thanks again,
 

cncburn

cncburn
Update: Changing my Z height from -2.5 to 7.5 resolved part of the issue. Good Catch! But, the first probe cycle runs properly, the second now runs down till the torch touch, but gives me a touch error and stops. So we are getting closer :) . I played with variations on the G0 in and out, with no further success.

I just saw your suggestion about the G91 Z2 on the same line. I think you are right there too. I will fix that tomorrow afternoon, and see if that helps. Thank you again for your advice and guidance!
 

jolbas

Jolbas
:)

I also noticed that in the version where you remove the G0 from the probing instruction, G0 is also disappearing on N17. Which may be a problem in combination with the double G-code on N16.

I suggest you add a new line after both G90 and G91, and then use the version without G0
 

cncburn

cncburn
Jolbas,

I tried your last suggestion and it did not seem to work, so I played with several other versions with and without G0. I also played with the number of commands on one line. Ultimately what fixed the issue was adding a G0 after the probe commands. (I don't understand why). I went back again and changed some of the commands back to the original positions as well. After several test with different files, it seems to be solid. Thank you for all of the help. I am attaching the latest version of the G code that works if you are interested.

My next step is to get my Torch Height Controller working properly, and add an Ohmic sensing cap to my torch. This (and code you helped me with), should give me torch touch and Ohmic sense (as a backup). Thank you again.
 

Attachments

  • Final.nc
    947 bytes · Views: 14

masso-support

MASSO Support
Staff member
Hi cncburn

Below is the example touch probe Gcode almost the same as your final Gcode from the Documentation. The only real difference is the G0 and Z height are on the same line and it is Metric. There is an explanation of how the Gcode works. I don't know if you have seen it but I'll post the link to it below

G38.2 Z-20 F200

G92 Z20

G0 Z50





Cheers

Peter
 
Top