i use a lot the command G4 P... for delay and be sure in some point machine not "round" corners
but i have several time its not work
when mach arrive this line its just hold ,do nothing no any error message
 this sample its not working ,mach hold witout error:
G1 Y506.0852 Z15.1 F4000
G1 Y505.7232 Z15.4 F4000
G1 Y505.3649 Z15.8 F4000
G1 Y505.0102 Z16.2 F4000
G1 Y504.6593 Z16.5 F4000
 G4 P10
G0 Z56.5


and this sample its work:
G1 X1545. F8000
G1 Y1202. F8000
G1 X772.5 F8000
G4 P10
G53 Z0.
M05

any idea?

In config you can set the type of G4 microseconds or seconds.

Are you expecting a 10 second delay?

You can also use X  as G4 X1. will wait for 1 second

Decimal points

From the manual:

G04 – Dwell
A dwell is simply a pause in the program. The duration of the dwell is specified by P or X in milliseconds with no decimal point. If a decimal point is used, then P or X specifies seconds. The dwell may also be specified with U without a decimal point for milliseconds. No machine movement will take place during a dwell. No auxiliary codes will be turned off, i.e. if the spindle is on it will stay on, coolant will stay on, etc.
The dwell must be the only G code in the block.
Format 1: G04 P__ Format 2: G04 X__ Format 3: G04 U__
Example: Program a 5 second dwell after positioning to X1.0, Z1.0 (using no decimal point to specify milliseconds).

G0 G54 G18 G40 G80 Safe start line
T0101
Tool change S2500 M3 Start spindle
G0 X1.0 Z1.0
Rapid to XZ position G4 P5000 Dwell for 5 seconds
M30
Program end and rewind
Example: Program a 5 second dwell after positioning to X1.0, Z1.0 (using decimal point to specify seconds). G0 G54 G18 G40 G80 Safe start line
T0101
Tool change S2500 M3 Start spindle
G0 X1.0 Z1.0
Rapid to XZ position G4 P5. Dwell for 5 seconds
M30
Program end and rewind

If you want an exact stop with no CV rounding, call out a G09 on the line you want a sharp corner with.  Faster than G04. 

Steve