Laser burn significantly reduced with "Laser mode on"

I’ve bought a cheap Chinese 7watt laser from Amazon to cut printing plates for my pad printer. But I’m new to this so, I’m learning as I do it.

After putting it together and getting it running with lightburn, I noticed that it was cutting the marks between letters and across them as it moved.

I read that I needed to turn on “laser mode” $32=1, and did that in the console. That did stop the laser from cutting between the letters but the power coming out of the diode laser is so weak now that it’s hardly making any noticeable burns, even with the power maxed out at 100%.

When I turn laser mode off, $32=0, it burns like a magnifying glass on a hot day, but cuts the travel marks. And turning it back on makes it go weak again.

How do I get it to burn at full power again with the laser mode one?

1 Like

Somebody more knowledgeable will chime in, but does your $30 value (max spindle speed) match your S-Value Max in your LightBurn settings? They’re typically 255 or 1000, from my experience.

1 Like

I’m having the exact same problem with the same laser!!

Most likely you’re asking the machine to go faster than the firmware is limiting you to.

Read here, particularly the stuff about Laser Mode and speed: Configuring a 3018 CNC for use with LightBurn

Thanks for that information. I read through it and understand about half of it.

What I understand is that, “In laser mode”, the travel speed governs the output power of the laser and that if its going too fast the power is reduced. So, I need to optimize my GRBL setting for the X and Y axis.

Based on my laser, $110 and $111 have some optimal number setting for speed that allows full power but if it is exceeded then the power output get squelched.

I don’t understand how to find that number. I think it has something to do with stepper motor resolution, $100 and $101?

Attached is a picture of my default GRBL configuration from the laser document.

Anybody know what these should be or how to find the limit? I got lost on the explanation of the stepper motor resolution and speeds.

According to the attached picture, your stepper resolution probably is wayy to high! The most common is 80 or 160 (at 16 microsteps, check your driver configuration how many you have). Basically, this value is obtained by your gear size, microsteps and some other things. Start with one of the values above and then tweak them. If it’s printing right with “1600”, don’t change them and just tweak them! Simply design a 300x300mm rectangle or some other size (not to small), laser it and measure it. If it meaures 300 perfectly, the value you set is spot on. If it’s more (or less) than it’s supposed to be, tweak the value. X and Y aren’t the same value, you must tweak them individually.

The “secret” formula to get the right numer on the first try is to measure the printed out rectangle and putting it in following “formula”:

(Designed_Size / Actual_lasered_size) * Current_resolution

For instance, if the resolution is set to X = 80 in GRBL, you design 300mm (in the X axis) and it comes out with 301, the formula would be:

300 / 301 * 80 = 79.7342

Set the value writing just $100=79.7342 and press enter. It should reply with ok (in above case). If you have a program for communicating graphically with GRBL, just type it in and save.

The acceleration with my particular laser is 2500, but the heavier your laser head is, the slower this value must be. This value is there to “ramp” your steppers up to speed, so they don’t loose steps. Too fast, it stalls (makes noise and doesn’t move properly) and you’ll loose steps, to slow and you’re wasting time for no reason and possibly burning edges and steep angles where it slows down and speeds up slowly for no reason.

ProTip: Also, when lasering and setting speeds in LightBurn or any other G-Code program, if you put in acceleration values too fast, but still within your defined GRBL configs, it can occurr that it lases without loosing steps, but jittering at steep angles or edges. If that occurrs, make it slower in your software. Don’t need to change it in GRBL, since fast moves while just going to a position is good :slight_smile:

I personally start a not too low value (for lighter setups to 1000 or above) and start incrementing 100. If the motor starts to stall while it’s moving at it’s maximum speed, go back down quite a bit, maybe 30% under that value. After all, it should be sturdy while moving and not stall if you just “touch” it. The faster it goes, the less torque it has, so it gets more sensitive to loosing steps the faster you go. Don’t worry about the noise when it stalls, this shouldn’t harm your steppers or laser, it’s just the motor which is loosing steps and that’s purely magnetic.

The maximum travel is literally the bed size in mm. Just set them both to 1000 or so and advance the laser slowly until you get to the very far edge of the bed, then you have your values. Overwrite the maximum travel with those and you’re good to go! Do this only after you’ve set the resolution, should be obvious.

1 Like

Depending on what machine you have, you might be stuck with that stepper setting. For example, if you are using a CNC machine with lead screws, you need to spin the screw quite a bit to move the axis, compared to a belt driven system where it’s much more direct.

Your max rate settings are $110 and $111, and they are set to 1000 mm/minute right now. If you tell the controller to go faster, it doesn’t, but it will reduce the power output so you get the amount of burn you asked for. For example, if you requested 2000 mm/minute at 100% power, that would be equivalent to going half that speed, with half that power level. If you ask for 4000 mm/min, you’ll get 1/4 the power output, because that’s the amount of “burn” you asked for.

8-bit GRBL is only capable of outputting about 30,000 motor pulses per second. With your steppers needing 1600 of them to go 1 mm, your absolute maximum speed is going to be 18.75 mm/sec, or 1125 mm/minute.

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.