First of all, the Fusion 360 post is amazingly well thought out... down to the router speed selection! That said, how on earth do I eliminate or modify the G53 G0 Zx.xxx command at the start of each file? It consistently runs the Z up past the limit. My only option right now is to manually eliminate that line each time I compile. It appears to want to go to a safe Z height before starting, but does not account for machining envelope or Z-clearance values. I have an extremely small Z envelope and have to run pretty tight z clearance on thicker materials. (Less than the 0.5906 that the G53 G0 calls!)
The G53 (machine coordinates, not work coordinates) shouldnt hit your limit switch at all. That's the point of using G53 and not G54 for the first move. It takes no consideration of your clearance heights or work 0. While its not documented in the post processor options, you can change the default value from 10mm to anything you like by editing the value for "End of job Z position (MCS Only)." This will change both the start and end of the job safe Z moves. The next Z move is a G54 and is controlled with Fusion by adjusting your clearance height.
In the post options you can set the Z offset that is used for the G53 safety move, what have you set it to? The default is -10mm (0.393") . this value will always be negative to prevent it hitting the limit switch at the top of Z travel. It only needs to be large enough to reliably prevent hitting the limit switch, how big exactly will depend on the mechanics of the switch and general stiffness of your machine. So test with -0.5mm which may be enough, even -0.25mm may be enough but make sure you test this with a long enough Z movement so gets to full speed going up to the safe height. This ensures that the jerk when it stops does not trigger the switch.
So the Machine Coordinates (G53) switch only applies to X and Y at end of job. That makes sense for material placement. It appears that I need to adopt best practices and set G53 Z at startup. Time to install limit switches! Use Machine Coordinates (G53) at end of job: Yes G53 G0 Z0.5 M5 G53 G0 X5.9055 Y3.937 M30 Use Machine Coordinates (G53) at end of job: No G53 G0 Z0.5 M5 G0 X5.9055 Y3.937 M30 It's a solid post processor- amazingly robust for a DIY CNC! Thanks for the reply.
Makes sense. Time for me to adopt best practices. It appears that moving to +x +y +z and resetting the black box is my present homing routine. Next is to order some limit switches. Not sure why I keep putting that off other than it just seems to work as is. Thanks for the response and links. Very helpful.
