Hello Guest it is May 24, 2019, 05:50:31 PM

Author Topic: guide to raster laser engraving with a 5 volt gate, ttl, or relay using lazycam  (Read 4023 times)

0 Members and 1 Guest are viewing this topic.

To engrave with lazycam you need to set your desired 5 volt laser controller output pin to your z direction pin and your step pin to 0. Set your step pin to active high. Make sure you have no other output on for that pin and that your at the right focus depth before you change the z pins.

Load your image in your CAD program and convert it to a black and white bitmap: aka monochrome or 1bit. The quality of your black and white image will determine the quality of your engraving. You do this because you have no way of controling exactly when the laser will fire unless the pixels all have either an on value or an off value; black being on and white being off. If you don't do this before uploading, you'll have a whole mess of z values which is great for a router, but will not work for  this operation. The same holds true with jpegs for some reason. Stick to bitmap (.bmp) format.

Upload the image in lazycam and set the max depth to 0.001, as shallow as it goes. Any jump of z more than about .001 in either the positive or negative direction might cause your table to pause every time your laser fires. If Z values of -0.001 cause constant pauses in your engraving cycle, you might need to convert your image to greyscale and change the color black to a shade of grey. The shade will determine the z depth (i.e. 50% black will give you a depth of .0005, 90% will give you .0009). Make sure your z equals between -0.0003 and -0.001 to fire the laser. Valuesbetween -0.0001 and -0.0003 usually don't work. The x stepover rate in xy raster mode will also determine if you have a smooth or chopy cycle. The higher the x stepover rate, the slower you have to go.  At an x stepover rate of .01- 60% black gives me 90 ipm's and 100% black gives me 80 ipm's.

There are 4 ways this post proccessor can ruin your piece. Post the tap file with my post proccessor but do not send it to mach3 automatically. This post proccessor must be edited manually. Delete the last negative z value and save. If you don't, you will get a line underneath your engraving. If you load the tap file in mach3 and you haven't first jogged your z axis up, then your laser will trigger and stay on. If your z value is positive when you start the cycle, then your laser will trigger and stay on. If you abort in the middle of your cycle while the Z axis is in a negative value, then your laser will trigger and stay on. Always jog the z axis up and zero it before you load the gcode. Don't abort in the middle of the cycle unless you have some other way of turning off your laser. Pull the plug if you have too.

If your unsure of the maximum possible feedrate before it starts getting chopy, set your z pins to 0 and toggle the feedrate overide while it's runing the cycle.

This is only if you have a 5 volt relay, gate, or ttl to control your laser. If not then try the crapy laser engraving plugin.

Shoot me a message if you have problems.
« Last Edit: September 14, 2009, 03:55:37 PM by ohpakron »