Laser Software for Acorn

[carocad]

I have added a 20W Laser to my CNC router powered by the fantastic Acorn board.
I can run all sample G-code files provided by Centroid, but I have a hard time finding a laser engraving/cutting software.
can you please point me in the right direction. Thank you

[tblough]

Most people seem to use LightBurn.

[Sword]

If you use one of the Vectric products, you can purchase the Laser Module add-on.

LaserGRBL is a free option. The saved G-code might need a little editing to make for optimal use, but that can be done with a macro in NotePad++.

https://lasergrbl.com/

[suntravel]

I use lightburn, works fine with Centroid.

Uwe

[carocad]

Thank you Sword. I have used Ventric before, nice software.
Do you have any experience with the Laser Module add-on? can it be configured to output G-code ready for Acorn?

[carocad]

suntravel, what machine type are you using in LightBurn?
my laser is setup with Acorn PWM on output 2, and using M37 for laser ON with S command for laser intensity.

[suntravel]

I export the g-code with my custom settings in Lightburn, based on GRBL g-code

Uwe

[Sword]

Thank you Sword. I have used Ventric before, nice software.
Do you have any experience with the Laser Module add-on? can it be configured to output G-code ready for Acorn?

I do have the laser add-on and use it some. It's okay and it did recently get an update, but I still prefer to use LightBurn.

You can edit one of the Centroid posts (in or mm) to output as needed for laser control. GRBL posts can be configured to work as well.

For LightBurn, I use it the same as Uwe does, using custom start and end codes with a GRBL post. I also run the posted GRBL file through NotePad++ with a macro that auto edits/saves the file ready for use.

[grossmsj]

https://centroidcncforum.com/viewtopic.php?f=60&t=5431

Sword's process works great with Lightburn.

I find Vectric to be a little more 'stable', but Lightburn is much more powerful. I occasionally see laser misfires with Lightburn where the laser apparently fires during G0. I've added another step that seems to eliminate that problem:
1) in Lightburn -> Device settings -> GCode, tick the box for "Emit S value for every G1 command".
2) Edit the GCode from the post processor output in Notepad++. (You'd be doing this anyway if you follow SWords workflow.) In Notepad ++, do a global search and replace. Search for ^(G0.*), replace with \1S0 (this is a regex expression).
https://cambamcnc.com/forum/index.php?topic=6067.0
This puts "S0" at the end of every line that starts with G0, telling the laser to shut off for that rapid move.

It sounds like a lot of work but it's just part of my workflow now and I don't get pieces ruined by this problem popping up.

[carocad]

thank you all. I am still figuring out the best way to edit the NC file in Notepad++

as grossmsj mentioned I use "Emit S value for every G1 command" and make sure the "use G0 for overscan" is off otherwise the very next G1 after a G0 does not have an S command.

in Notepad++ I recorded a macro to find and replace the following ... (please do your own testing before running any files on your machine)
M4 -> G37 ON \nM37
M8 -> S0
G0 -> G0 S0
M5 -> M38
M9 -> M5
M2 -> ;

this way I did not have to add any custom start or end
I think M8 from LightBurn is for the air assist. I have run out of relays to control the air so I am doing that manually until the expansion board is here.
will keep you posted with any updates.