Using a G0 in your code is equivalent to saying "go rapidly to point xxx yyyy". This code causes motion to occur at the maximum traverse rate.
Example:
N100 G0 X10.00 Y5.00
This line of code causes the spindle to rapid travel from wherever it is currently to coordinates X= 10", Y=5"
When more than one axis is programmed on the same line, they move simultaneously until each axis arrives at the programmed location. Note that the axes will arrive at the same time, since the ones that would arrive before the last axis gets to the end are slowed down. The overall time for the move is exactly the same as if they all went at their max speeds and the last axis to arrive stops the clock.
To set values for rapid travel in EMC, one would look for this line in the appropriate emc.ini file:
[AXIS_#] MAX_VELOCITY = (units/second)
The previous value for the rapid rate, [TRAJ] MAX_VELOCITY, is still used as the upper bound for the tool center point velocity. You can make this much larger than each of the individual axis values to ensure that the axes will move as fast as they can.
One thing to remember when doing rapid positioning, is to make sure that there are no obstacles in the way of the tool or spindle while making a move. G0 code can make spectacular crashes, if Z is not clear of clamps, vices, uncut parts, etc.....Try to raise the tool out of the way to a "safe" level before making a rapid.
I like to put a G0 Z2.0 (Z value depending on clamp height) towards the beginning of my code, before making any X or Y moves.
Example:
N100 G0 Z1.5 --move spindle above obstacles
N110 G0 X2.0 Y1.5 --rapid travel to first location