Altering Fusion 360 post processors to allow mill to pause and wait for spindle to ramp up

If you want to hard code in a dwell time for your spindle to ramp up so you are not fiddling with your feed override knob, then here is what you do to the post processors;

You will want to open up the post processor config file and locate a block of code similar to this. You can hit "ctrl+f" to do a search for "if (tool.spindleRPM" and that will likely get you down to the right section of code.

if (tool.spindleRPM < 1) {
error(localize("Spindle speed out of range."));
return;
}
if (tool.spindleRPM > 99999) {
warning(localize("Spindle speed exceeds maximum value."));
}
writeBlock(
sOutput.format(tool.spindleRPM), mFormat.format(tool.clockwise ? 3 : 4)
);

Just after that last semi colon, add a dwell command and choose the seconds you wish to have in the dwell. The modified code should look something like this:

if (tool.spindleRPM > 99999) {
warning(localize("Spindle speed exceeds maximum value."));
}
writeBlock(
sOutput.format(tool.spindleRPM), mFormat.format(tool.clockwise ? 3 : 4)
);
onDwell(2);

I set mine to give a 2 second dwell. So, every time a M3 / 4 is called that dwell will piggy back and cause a dwell before the next lines of code are read.

 

Also if you are using mach3, there is a setting in the spindle set-up window that will add a user defined dwell on spindle start and stop.