Hi. I have the Opt Lasers PLH3d-6w-xf laser connected to the BlackBox Motion Control System. After updating the software, the laser lost power and does not cut. More on the video. Is it a matter of compatibility and something does not match, or settings on the BlackBox?
Your backup file is empty. Make sure to be connected first, then Backup. Open the text file and review before posting Your screenshots 1,2,3 are all of the same screen ($0-$11), so I can't see what you have $30-32 set to. Screenshot 4 starts at $101. In essence, I wanted to see if you have $30 set to 1000 or 255 (and wanted to confirm laser mode, etc) , and then we'd have followed up to make sure you did set the same range in Lightburn If you have $30=1000 but you are telling Lightburn to use 255 - then its max power would be M3S255 instead of M3S1000 - giving 255 to a controller expecting 1000 would be about 25.5% power
I checked the settings "briefly" and the laser worked at full power so it is operational. I am sending the backup. If you can, see what and how.
Ok cool,so you do have $30=1000 ; Maximum spindle speed, RPM $31=0 ; Minimum spindle speed, RPM $32=1 ; Laser-mode enable, boolean Laser mode is an important one. $31=0 is good, otherwise scaling is off. And we do have $32=1000 So next up, if you create a job with 100% power and export the GCODE. Is the S-word 1000? M3/M4 S1000 in the gcode somewhere. Post the gcode for review please You did setup docs:software:lightburn [OpenBuilds Documentation] as per the docs?
; GCODE Generated by cam.openbuilds.com on 2023-07-11 G21 ; mm-mode G54; Work Coordinates G21; mm-mode G90; Absolute Positioning M3 S1; Spindle On M3; Constant Power Laser On M4; Dynamic Power Laser On ; Pass 0 ; Operation 0: Laser: Vector (no path offset) ; Laser Spot Diameter: 0.1 G0 Z10; move to z-safe height G0 F1000 X0.0000 Y0.0000 G0 Z0 G1 F300 Z-0.1000 G1 F150 X0.0000 Y50.0000 Z-0.1000 S1 G1 F150 X100.0000 Y50.0000 Z-0.1000 S1 G1 F150 X100.0000 Y0.0000 Z-0.1000 S1 G1 F150 X0.0000 Y0.0000 Z-0.1000 S1 G1 F150 X0.0000 Y0.0000 Z-0.1000 S1 ; retracting back to z-safe G0 Z10 M5 S0; Spindle Off M5; Laser Off M5; Laser Off
You have only got S1 = 1/1000 = 0.01%? Should be S1000 - Check toolpath settings. Both M3 and M4 is bad too: one or the other, not Both... The Optlaser likes M4 Dynamic power You added Both. Only add the M4/M5 option. Delete the other one (or delete both and only add back the correct one)
"You have only got S1 = 1/1000 = 0.01%? Should be S1000 - Check toolpath settings." Will you guide me where in the settings I can change this? I generally use openbuilds cam.
Yes, See Reply #7 above But its a paired combo. What you set in the controller settings, you also have to make sure your CAM knows about it, $30=1000 is pretty stock, so you changed something along the way I don't really know what you changed but check Settings Tab > Settings Button > Make sure you only have the one tool init in (4) as shown above and also lower down in (5) that Power/Speed Scale is 0-1000 Then the Power percentage is set when you setup a toolpath 100% with power to speed scale of 0-1000 means 100% outputs S1000 Grbl has $30 Max RPM(Power) set to 1000 as well, so S1000 tells to to output 100%
