I want to know the version too! any answer??

Hello I think I found the GRBL version

on their latest post about the new released version (https://www.laseraxe-customize.com/forum/cncc-software/cncc2019-v1-09-software-released), laseraxe posted a picture on which you can see V 0.8

Also I've read another post (https://www.laseraxe-customize.com/forum/laser-engraving-machine/update-grbl-1-1f) on which people talking about the firmware and they say it's based on version 0.8

regards

Thanks a mil, jonat_26 ... it's the best we have so far. I've been using trial and error to see which commands work, at least for the ones I use. I'm using Fusion360 and exporting GRBL/g-codes using a PostProcessor script I found on the internet. Of course the GRBL format exported is too new for the 0.8 firmware, but I wrote a small C# program to strip away most of the non-compatible coding and add a few M-codes which control the laser on/off. At the moment I'm looking into controlling the laser power from GRBL, I know there are $ codes which set those, but I haven't tested if CNC2019 will allow them to control the power from within the g-codes. I will probably buy a separate controller board that I can flash to 1.1f without compromising the one I have, but for now it's easier (and cheaper) to fiddle around with the GRBL g-code files. I appreciate your feedback and effort!

Thanks for your encouraging answer jacobekker777,

I'm a CADCAM engineer at a woodworking software company based into SOLIDWORKS environment.

The software is called SWOOD.

For my own laseraxe (1mx1m 15W) I developped a specific PostProcessor with SWOOD (based on gcode test files given by laseraxe) but in these test file I found no trace of power driving command (like S or M) so this is why I posted on this forum a subject https://www.laseraxe-customize.com/forum/cncc-software/controlling-laser-power-with-gcode but with no answer.

I can't share my PostProcessor because SWOOD is a licenced software (sorry)

I'm also thinking about buying another arduino nano3 controller to have the latest GRBL 1.1f

Before, I'll make some tests with laseraxe soft try to drive power with S or $,

I'll give you my feedbacks on this forum.

If you find things (even with another controler) don't hesitate to share

Hello again,

I watched a bunch of stuff about GRBL and so on,

I watched my official laseraxe firmware based on CNCC2019 v1.09.01

it looks like this

then I compared it to the different GRBL settings directly on the official Github page

https://github.com/grbl/grbl/wiki/Configuring-Grbl-v0.8 (from $0 to $22)

https://github.com/grbl/grbl/wiki/Configuring-Grbl-v0.9 (from $0 to $132 like our setting)

And I was really surprised to realize that all the parameters were the exact copy of the V0.9 version

So sorry if I put you in the wrong direction in my previous post

Great minds think alike ... I were just busy prepping the exact same screenshot from my other computer ... see screenshot below...

I first realized I could maybe use the $ codes when I saw an export from Fusion360 containing one of them ($133) ... see screenshot below ...

So, you're correct ... GRBL definitely supports the $ codes in the .nc files. I still need to test it though, proof of the pudding and all that.

Sure, no problem, I'd be more than happy to post my findings here. I'm definitely a newby to laser cutting and this is my first machine. I'm a programmer by trade (in South Africa), so I'm just tinkering with the laser cutting in my spare time.

In the mean time, I've also managed to get a SVG viewer working in my C# g-code conversion program. So I'm hoping to use the similarity between the SVG vector drawing commands and the g-code drawing commands, to enable my program to draw a preview of the g-code file before conversion. From there it should be easy to make it zoom and pan, so I can fit and view complete 1m x 1m drawings on there. Maybe even select individual shapes and set the laser power and repeat count for each shape. That should be a very handy combination.

I'm very happy to hear you have the same laser cutter than I do (1m x 1m @ 15W), so I'd very much like to post my findings and tap into your expertise a bit.

On the g-codes, looking at the screenshot above, you can see the G0 codes used to quickly move the laser head to a new position. So my conversion approach in essence is to remove the version 0.8 unnecessary commands, and then use the G0 commands to split all the drawing/cutting commands into "islands" ... meaning continues cutting regions. That allows me to just put M05 (laser off) in front and M03 (laser on) after each G0 command. Works pretty well (so far).

Nice found with $ codes within the GCODE!

I found a lot of forums about laser machine in GRBL based controller and they often say that controling laser power was only possible if PWM is enabled and cabled on the card, so I really hope it could work with our hardware.

I'm going tu run bunch of tests this week-end so I hope I will go further than my theorical thoughts (I'll keep you update).

Awesome, thanks!

I'm swamped in work at the moment, so I doubt I'll make much more progress on my side within the next few days, but I'll keep you posted on any progress too.

Hi jonat_26, just thought I'd post a quick update on the above laser level tests ... did a bit of late night tinkering. I took a g-code file I had, which consists of ten bars, and modified the G-codes by adding the spindle speed command (Sn) to each bar, varying from S100 to S1000 in steps of 100 ... and it worked perfectly ... it controlled the laser intensity for each bar it engraved, directly from the G-codes file.

See photo below ... you can clearly see how the cut deepend as the laser intensity increased from left to right. All bars were done at the same feed rate of F500.

So, success, no I can add that feature along with the repeats to my C# program.

One more thing I noticed, is the laser head wobling after moving the laser head quite fast using G0 code. It is visible in the photo as the extra black dots at the top left of every bar. But, that should be easy to fix, by putting in 'n delay of 250ms or so after the G0 move, but before turning on the laser. I should be able to have my C# program add the delay automatically.

Cheers

Waooo, nice!!

hopefully it's working!

thank you sharing this so quickly.

could you just copy the text of the GCode you tried for me to check it?

cheers

Sure, no problem ... see below the g-codes that did the cuts/engraving in the previous photo. You can see the G1 S100 F500 that sets the spindle speed to 10% and feed-rate to 500 (mm/min).

G90

G21

M05

G0 X105.483 Y6.75

M03

G1 S100 F500

G1 X105.05 Y6.5

G1 Y5.05

G1 X109.95

G1 Y48.5

G3 X105.05 I-2.45

G1 Y6.5

G1 X105.483 Y6.25

M05

G0 X94.372 Y6.75

M03

G1 S200 F500

G1 X93.939 Y6.5

G1 Y5.05

G1 X98.839

G1 Y48.5

G3 X93.939 I-2.45

G1 Y6.5

G1 X94.372 Y6.25

M05

G0 X83.261 Y6.75

M03

G1 S300 F500

G1 X82.828 Y6.5

G1 Y5.05

G1 X87.728

G1 Y48.5

G3 X82.828 I-2.45

G1 Y6.5

G1 X83.261 Y6.25

M05

G0 X72.15 Y6.75

M03

G1 S400 F500

G1 X71.717 Y6.5

G1 Y5.05

G1 X76.617

G1 Y48.5

G3 X71.717 I-2.45

G1 Y6.5

G1 X72.15 Y6.25

M05

G0 X61.039 Y6.75

M03

G1 S500 F500

G1 X60.606 Y6.5

G1 Y5.05

G1 X65.506

G1 Y48.5

G3 X60.606 I-2.45

G1 Y6.5

G1 X61.039 Y6.25

M05

G0 X49.927 Y6.75

M03

G1 S600 F500

G1 X49.494 Y6.5

G1 Y5.05

G1 X54.394

G1 Y48.5

G3 X49.494 I-2.45

G1 Y6.5

G1 X49.927 Y6.25

M05

G0 X38.816 Y6.75

M03

G1 S700 F500

G1 X38.383 Y6.5

G1 Y5.05

G1 X43.283

G1 Y48.5

G3 X38.383 I-2.45

G1 Y6.5

G1 X38.816 Y6.25

M05

G0 X27.705 Y6.75

M03

G1 S800 F500