Hello and sorry if this is a pretty bad question lol how do you set the x,y,z origins to engrave with a laser on your CNC and then switch to cut out with the router and maintain the proper origin? brain is struggling to figure this out since the laser is say fixed to the front side of the router the beam and bit sit in two different places can’t wait to hear how this is done Mi am hoping to engrave some wood then cut it out with the router given the thickness of the wood
If your laser mount came with a drawing showing where the beam is centered, and you know it is in line with the endmill, then using that information along with the dimensions of your spindle mount, you should be able to figure it out and get it pretty close. Then after the math, take a very fine engraving endmill, engrave a thin line, and using the offset you came up with in the math portion of this problem, jog your machine the required distance so that the laser is now directly above and centered on the endmills XY zero point. Then reset the the XY zero and start engraving with the laser. If your measurements were accurate, you should burn on top the engraved line. If you do not want to do the math, engrave a line with the engraving bit. then engrave a parallel line with the laser in both the X and Y axis using the same XY origin point. Then measure them and repeat the red part above making fine adjustments until they are perfect. Or as good as you want. Sadly I do it the hard way. I cut on my router than move it to the laser machine to engrave. To do this accurately, I always zero on the center of my work piece. Always Zeroing on the center with both tools is another option for you. It may be the easiest if this is a one time project. If not, calculate the offset so you can easily repeat it whenever you need to,
having calculated or measured the offset I would create 2 macros to move back and forth between the 2 tools. lets say the laser mounted 3.2 inches from the spindle in Y (-3.2" from the router tool in Y) and 0.26 to the right of the spindle (0.26" in X) so, macro to move to the laser, router is set as X0 Y0 in current WCS (usually G54) G20 G90 G17 G0 X-0.26 Y3.2 now press the setZero X and setZero Y buttons abnd you can run your laser gcode. to switch from laser to router G20 G90 G17 G0 X0.26 Y-3.2 and press setZeroX and setZeroY one could add code to those macros to do the 'setzero' automatically, note, I edited this post to correct this to L20 instead of L2 Code: (from the Gcode definition at linuxcnc.org) G10 L20 Set Coordinate System G10 L20 P- axes [LIST] [*]P - coordinate system (0-9) [/LIST] G10 L20 is similar to G10 L2 except that instead of setting the offset/entry to the given value, it is set to a calculated value that makes the current coordinates become the given value. router to laser G20 G90 G17 G0 X-0.26 Y3.2 G10 L20 P0 X0 Y0 laser to router G20 G90 G17 G0 X0.26 Y-3.2 G10 L20 P0 X0 Y0 now, we can further embroider on the system by always using G54 for the router and G55 for laser, now we only need 1 macro having set the router to the proper zero position in G54, this macro will set the laser X0 Y0 to this place G20 G90 G17 G54 G0 X-0.26 Y3.2 G10 L20 P2 X0 Y0 Note that I have left out setting the laser focus height. I don't see a way to automate this without having an entire tool offset table since the laser focus distance is not related to our router Z0 because our tool stickout varies. I would use a piece of plastic or wood cut to the right length so I can stick it on the surface of the work and jog the laser till it touches the laser body, and setZeroZ there, easiest way I can think of.
Well just read through those two very informative post and mind is blown at the moment. lol will read them again and digest Has anyone seen a video tutorial on this? I have searched to no avail
