The machine keeps its position in Machine Co-ordinates. The 0.0.0 position is determined by the position of your "Home"switches - if any. If you do not have home switches connected then the machine will "Ref All Home" anywhere.- but for this explanation we must assume you have them fitted.
The "Home" position will probably not be relevant for machining, and certainly not relevant to your "program co-ordinates" position. To set the program co-ordinates position, you jog to the 0.0.0 position of your program and zero the DRO's for each axis. (NOT Ref All Home - but the zero x zeroy etc,) If you check the Program Co-ordinates position, this will now show 0.0.0, whereas the Machine Co-ordinates position will show the offset of the present position from the machines "Home" position.
A G0 move is relative to the Program Co-ordinates 0.0.0 position, whereas a G53 is relative to the Machine Co-ordinates position.
G53 is "Move in Absolute Co-ordinates" and is used where you want the machine to move to a particular position (relative to the machine co-ordinates) for a specific purpose e.g. tool changing, irrespective of any other offsets (Program or Tool offsets) that are being used. It should not, as far as I know, be used for general machining purposes.
Using G0 you can then take advantage of Constant velocity, where the next line commences moving before the present line is finished, and the program melds the two into a smooth change of directio i.e. constant velocity.
Using G53 - this cannot take place, because the overriding instruction is go to a specific point (and in constant velocity that point is never reached)
Without Constant Velocity, cutting arcs, which on most Cam programs are made up of many, many little straight lines, each line must complete and STOP, before the next line can start, giving a very jerky movement, and this is the effect you are seeing.
I suspect you have the 0.0.0 position of Machine and Program co-ordinates co-incidental, and therefore, although I don't know why, you are using a string of G53 commands for general machining. Being co-incidental doesn't matter - it is using the G53 that is making the difference. G53 should only be used for single movements to specific places.