It may help to know what you’re telling the machine to do at each line (see below). Since the line you are starting from doesn’t have a Z value and is in G0 (move as fast as you can mode), the machine will be moving as fast as possible for that layer you’re starting at (hopefully cutting through air and not hitting any clamps, your workpiece, or other objects). You can use the information below to create a sane starting point at an arbitrary point in the file.
You can learn more about G-code from the RS-274 specification (The NIST RS274NGC Interpreter - Version 3 | NIST) or from the Linux CNC documents since Grbl adheres to the Linux CNC implementation of their G-codes (G Codes).
G90 ; All X, Y, Z values will be in absolute coordinates and not offsets of current positions
G21 ; All values are in millimeters
G53G0Z-5.000 ; Move to 5 millimeters below the highest Z point
M05 ; Turn off the spindle/router
M6T201 ; Change to tool number 201
M03S18000 ; Turn on spindle/router clock-wise at 18,000 RPM
G0X31.75Y15.88 ; Move as fast as you can to the given X, Y position offset from your work zero/origin
Z6.35 ; Move as fast as you can to a quarter inch above the work zero
G1Z-2.54F1270.0 ; Move at 1270mm/min cutting speed, -2.54 mm below your work zero
Y819.78F2540.0 ; Move at 2540mm/min cutting speed to the given Y position (X and Z stay the same)
Y15.88 ; Maintain same speed, same X, same Z, and move to Y 15.88
...