Laser Cutter: Information, usage details, and useful links!

[Christopher Hoffman]

Hey Everyone.

Got my first taste of the laser cutter in operation yesterday. I've been doing research, figured this would be a good place to put all the stuff I found.

Basics:

The cutter is a K40 Laser Cutter, with an 40W CO2 laser. The main board has been replaced with a BeagleBoard, with documentation that you can normally find here (www.miles-milling.com/LaserK40BeagleBoard.htm), but seems to be down for me.

General Tips:

There is a nice Reddit Wiki about the K40, with basic guidelines, and some speeds/power recommendations for different materials. Read that link, it has a lot of good information. I have not had a chance to validate the information on there yet, I want to do some testing with it to dial in the settings for our particular machine.

Connecting to the machine:

• Start the pump to start cooling the laser before you try to connect, that way it has been running for atleast 10 minutes before you start cutting. 
  
• To connect to the machine, turn it on, and make sure the ethernet cable is connect to the 3D printer machine. To check connection, open up windows command prompt, and ping 192.168.1.16 (thats the laser's static IP). If you get a response, great! If not, power cycle the laser's board (make sure it actually power cycles by watching the LEDs on the board turn off).
  
• From there, you can use VNC Viewer to connect to the linux OS running on the BeagleBoard of the laser. You can connect to it using the 162.168.1.16 IP. It should connect you to a linux desktop.
  
• Click on LinuxCNC, and connect using the HSLC preset (Hackerspace Laser Cutter), (should be under a bunch of CRAMPS options).
  
• To transfer your .ngc files, use WinSCP to upload them to the laser cutter. Open WinSCP, and connect to 192.168.1.16, and any username/password should be 'machinekit'.* 

Note on the GCode:

From the Miles-Milling article for the BeagleBoard:

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. 

That means you can use any normal gcode designed for linuxCNC, just make sure the cut depth is < 0 in order for the laser to turn on. From my understanding, we do not yet have a way to vary the laser intensity through gcode, we have to do that manually.

Max Power:

The max current is 18 mA! Any more and you risk dramatically shortening the laser's lifespan. Here is a conversation about it.

Materials/Feeds/Speeds from the Reddit Wiki

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

Other Materials:

Materials you can cut, and those YOU SHOULD NEVER CUT

Other Links:

A collection of links from the K40 community

As I find out more, I'll add to this post and spread the knowledge around :D:D:D:D:D

[Brian Bartholomew]

Thank you! I predict black markings on stainless for pocket-sized
circular slide rule money clips in my future...

http://atxhackerspace.org/wiki/Laser_Cutter_Materials

Etching can be done on almost anything [...] aluminum [...]
stainless steel

Etching
Anodized aluminum Vaporizes the anodization away.
[no entry for stainless]

We have a very limited amount of an expensive coating called
'cermark' that was purchased by Martin. This marking compound
costs $100 for a small bottle, and must be diluted with
ethanol and applied to metal (not ceramics or stone) before
being etched to leave behind a permanent dark black mark.

http://www.instructables.com/id/Metal-Marking-Control-Panels-with-a-C02-Laser/

[after laser darken marks with 3-in-one oil or spraycan clear coat]

http://www.evilmadscientist.com/2013/laser-moly/

Unfortunately, a spray can of CerMark costs $60

[instead try] $10 spray can of dry moly lube

Very interesting! Looks like the Cermark products use
molybdenum (20-30%) and vanadium compounds (10-20%), based on
their MSDS

If you wish to experiment further with it: you can just buy
moly powder on ebay, mix it with some acrylic paint and apply
a thin layer. A spray gun would probably give a more even
result.

I wonder if the laser can remove a resist for chemical etching, which
would produce cavities which can be filled with black epoxy. Markings
below the surface are more wear resistant.

For stainless I'd let an established company do the etching, so they
can handle the Chromium solution produced.

https://discuss.inventables.com/t/paint-resist-laser-ablation/11759/6

[laser removes black spray paint on PCB copper]

http://hackaday.com/2008/08/03/laser-etching-printed-circuit-boards/

the magical chemical i'm using is 99% rubbing alcohol from
safeway on a paper towel. It takes off the residue without
destroying the resist pattern. Oh, and the paint I’m using is
Rust-Oleum "Painter’s Touch" flat black from Home Depot.

rustoleum flat black high temp grill paint aerosol

[Christopher Hoffman]

Got a chance to test out some setting this morning. May I present, my findings!

Engraving:

I used CamBam to generate some pockets from a simple text insert of 'Hoffman' onto normal index cards. I originally tried it with default settings, with a speed of 1000 mm/min (I was in millimeters, make sure to convert it to inches if you prefer that).

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.

[GRB352]

Great stuff!, I'm glad you figured out how to get "Raster style" instead of "vector style" pockets. I will use your settings next time.

There is a way to do vector pockets right, and they do seem faster:
https://youtu.be/5g4HeYXfNwA

but raster (hatch region fill) mode I think will work better for lasering pictures onto wood. 

https://youtu.be/guTw1Vjgl2U

Cambam has a "image height map" plugin that should do it, but I get poor results from it. I think using cura to convert image to litho-stl, then doing a "3d profile" operation in Cambam is the way to go for that (its basically a fancy pocket), hopefully the 3d profile op has region fill style as an option.

[Christopher Hoffman]

The problem is that we don't currently have a way to control the laser intensity through gcode, we have to do it manually. If we can figure out a way to connect it to the control board, then we can do raster style images like that, until then we can only do simple things controlling the intensity by hand.

[GRB352]

While controlling laser intensity is one way to do it. There are two other variables that can be modified to do it.

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.

[Christopher Hoffman]

Oh, didn't think of method 2! We'd have to create a script that goes over the generated gcode though. This laser is set to turn on anytime z < 0, so by default it would constantly be on for each layer. each layer would have to be modifed so all other other Z heights are >=0, Almost trivial to do that though, depending on how the 3D profile works (I've only played with it once.)

[GRB352]

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. 

 

[GRB352]

when moving from one work area to another it will still go above Z=0 and turn the laser off to move to another area to work, no matter how deep it thinks it is cutting. 

[Christopher Hoffman]

Ok, spent a few hours yesterday playing with cutting/engraving acrylic and birch plywood.

First, the results!

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!

[GRB352]

Hey do you know the work area dimension after they were (somewhat) recently modified? I want to design my panel around widest faceplace I could laser.