Make sure Setting 36, PROGRAM RESTART is turned ON.
Cursor down to slightly ahead of the point you want to restart; normally I like to restart on the line below a Z clearance move.
The way PROGRAM RESTART is the controller scans all the way through the prpogram to get the correct offsets, tools and tool diameters activated. Then it moves to the location defined by the program line immediately above your restart point, this is why I try to make sure this line has the tool up away from the work, then it moves to your start point.
If you are using MIRROR G100/G101 in a program funny things can happen, if you are using loops will L counts you cannot start in the loop only somewhere before it. If you turn Single Block on before restarting the controller scans very slowly.
I suggest turning Rapids down to 5%. Push Cycle Start and hold you finger over the Single Block key; as soon as the spindle starts or any axis moves push Single Block. Now you can speed up the rapids and Single Block to your start point. Keep an eye on clearances, I have hits clamps during restart because the machine goes to the preceding Z position as I mention then scoots across to the restart point without lifting Z. If there is a clamp that is too high in the way bang goes your tool.