In order for the laser to cut (turn on) with the BeagleBoard MoshiDraw replacement three conditions must be met. One the hardware "Laser Switch" must be enabled or pressed down. Also on the software side LinuxCNC must have the laser mill enabled with the mouse selection. And finally the laser to be modulated will occur whenever the .gcode/ngc states a mill < 0 in depth position. Whenever the mill gcode call for a z position that is greater than zero the laser will shut off.
Material | Thickness | Action | Laser power | Speed | Pulses/mm (PPM) | # Passes | Notes |
---|---|---|---|---|---|---|---|
Plywood | 3mm (1/8") | Cut | 7-9mA (20-30%) | 500mm/min | CW | 1 | |
Plywood | 3mm (1/8") | Engrave | 7mA (20%) | 1500mm/min | CW | 1 | |
Acrylic | Any | Engrave | 7-9mA (20-30%) | 1500-2000mm/min | CW | 1 | |
Acrylic | 3mm (1/8") | Cut | 9mA (30%) | 500mm/min | CW | 1 | |
Acrylic | 4.5mm (3/16") | Cut | 7-9mA (20-30%) | 250mm/min | CW | 1 | |
Acrylic | 6mm (1/4") | Cut | 11mA (40%) | 250mm/min | CW | 1 |
Got a chance to test out some setting this morning. May I present, my findings!
It was... terrible. The default pocket follows the edge of the design and does concentric patterns inwards, which is great for CNC but terrible for lasers.
But then I found the magic setting. There is a setting: 'Region Fill Style' . You want to change it to either Horizontal or Vertical Hatch. That'll force it to only cut in one direction, and gives you a much, much higher quality engraving.
Here is an engraving with a horizontal hatch:
I tried a few different tool diameters. I tried 0.1mm, 0.5mm, and 1mm. The 0.5mm diameter was by far the best results. You could see the stepping in 1mm, but 0.1mm took forever and gave crummy results, so stick around the 0.5mm diameter.
Another setting to pay attention to is 'Velocity Mode'. There are two options, "Constant Velocity" or "Exact Step", and deals with how the laser head moves from position to position. Constant velocity performs some decceleration smoothing, while exact step doesn't do that smoothing. In the image below, the top card is with Exact Step, and you notice that both the left and right edges of each letter are burned the same amount.
The bottom card is the default, constant velocity.This smooths the exit, which means that the laser is on longer at the right edge, so it makes that edge darker than the left edge.
Pocket Settings:
So, for index cards, I'd recommend doing pockets with 3500mm/min speed, a 0.5mm diameter, a target depth of -0.02mm, with horizonal hatch and exact step velocity. The power of the laser should just be high enough to leave a mark, reads about 2.5mA on the analog meter. The knob, btw, turns more than the decal suggests, the engraving was far below the first mark on the decal.
Profile Settings:
For Profile cuts, I did a 2000mm/min speed, with a profile cut in cambam. I used the same -0.02 target depth, with a 0.5mm tool diameter. Finally, I had the power at about 4mA on the meter, slightly more than for engraving.
1. Modify speed. slow down for darker etch areas speed up for lighter. Figuring out acceleration settings might be a pain.
2. Multiple passes, make "darker deeper" and then set your pass depth less than target depth (this is how cambam-> 3d profile would do it) figuring out how many passes would be needed at what speed could be a pain. Also might need to tweak how deep the lithopane STL is.
No fancy scripts should be needed. Go ahead and drag any image into cura, then accept the defaults. It makes a lithopane (height map) STL (see attached pic). Then , (if I can figure out how to get cambam to use a STL properly) have cambam carve that shape like it is a pocket.
As it goes deeper, there is less and less to do in the light areas and because only the darker values have anything to be done at that depth.
That is the plan anyway. I've never stuck with attempting getting a CNC machine to carve a STL file long enough to figure it out. It is just as confusing as trying to get MeshCAM to do it and I've given up a couple times.
Laser etched picture seems like it would make some of my art'see type stuff (like the owl face, and those cutting boards) go a lot faster. Going from SVG->DXF then hours cleaning up the DXF in draftsigjht removing excess lines and making the shapes manifold in cambam. It would be nice to skip all that and just drag in a picture. Try the heightmap generator out in cambam->plugins. maybe you will have better luck riddling out the proper settings there or in 3d profile. If it works for the laser, it will work for the fireball, and for dremelflexbot.
Acrylic:
Acrylic engraves and cuts wonderfully. I picked up some 1/8th inch acrylic from lowes for 10 bucks, and used the mini bandsaw to cut off a couple index card sized pieces. Probably a little too small for the designs, but I could fit two of my logos onto a single piece if I was careful with alignment. I then sat the acrylic onto a piece of wood to support it in the cutter. If you had a larger sheet, you could just put the acrylic in by itself, but mine were too small.
The settings I used were similar to the index cards. Horizontal hatch, 3500 mm/min speeds. I tried both 0.5mm and 0.3mm tool diameters, but since the acrylic was raised closer to the laser by the wood support, that 0.5mm turned out much better. While engraving, I had the power at about 3mA, manually adjusting it to get the depth I want.
To cut, I created a Profile cut from a rectangle I drew in CamBam, had it go at 500 mm/min, and adjusted test power until I could see the laser start to burn the wood underneath. Normally you can't see the laser when engraving the acrylic, so by looking for a small dot on the wood, you know the lasers cutting all the way through. 1 pass was enough to cut through, with the power at about 6-7mA.
Once you are finished cutting, leave the acrylic to off gas for a few minutes inside the enclosure, so that the fan can remove most of the unpleasant smells. (Mark and I figured that out the hard way last night).
Wood:
I grabbed a piece of 1/4 inch birch plywood from Lowes, one of the 6 dollar small sheets. The actual thickness is 0.19 inches. I also cut that into a few 5"x3" pieces using the bandsaw (although it was a little smaller, as you'll see from the results).
I used no support here, just the pieces of wood themselves. Engraving used the same gcode as above, with about the same power levels. The more power, the darker the areas. Turn it up too high and you'll get flames along with the cut, which you should avoid as it'll leave soot on your pieces.
Cutting is another matter. Because we do not have an "Air assist", which blows air at the spot where the laser hits, we have to be conservative with the power so that we don't produce flames. Flames are bad, they mark your piece, obscure the laser, and is overall no good. Because of that, I had to do about 10 passes to cut completely though the wood, adjusting the laser to a point just before it created large flames. As you go deeper, you can pump up the power, and flames are less bad at this point (theres less oxygen getting to the wood in the groove). Eventually it cut all the way though. Once one of the little holes in the pulleys fell out, I stopped and was able to push the rest out with my fingers.
I also was able to create a living hinge, through carefully designing a series of lines to cut all the way though. This took a few iterations, as the kerf of the laser is actually pretty significant when cutting all the way through (There is a lot of burning of the wood on the sides of the groove). The 3rd attempt was the charm, and I now have a nice, flexible piece of wood. Its fun to play with. Again, this also took about 10 passes of increasing laser power to cut through, and I think it could have used a few more, as it did not quite cut all the way through some of the grooves.
Also, doing a quick pass with 120 grit sandpaper makes a huge difference in surface finish with the wood. If you cut all the way through, you'll have a lot of dark burn marks around the cut, but those are easily removed with sandpaper. For example, compare the living hinges above (which are after sandpaper finishing), to the raw cut below.
Careful with the sandpaper though, if you have also engraved in that wood, then you could be sanding away some of that engraving.
That is it for todays lessons with the laser cutter! I'll probably show off my results at the demo on Tuesday, and can show people how I set up and used the machine!