Inputting Probe Thickness Parameter

I have a CNC3 3018 Pro CNC machine, which I am getting to grips with slowly.
I have purchased a Z Probe device, which has a height of 19.1 mm, and connected it so that I see the appropriate actions when the Z Probe button is clicked in Candle.
I have tried adding the following to the Probe Commands in Candle: ;G10L20P0Z19.1;G91G21G0Z10
But when I remove the Probe device and jog Z down to the surface of my workpiece, the Z coordinates do not reach exactly 0
Am I doing something incorrectly?
Is there a parameter in the machine commands that is affecting my results?
Do I need semicolons in the Probe Commands?
Should I have spaces between the elements in Probe Commands?
Is there another way of doing this?
I might add that I have spent a lot of time searching for specific instructions for this, but they all seem to stop short of this final step.
Thanks in advance for helping an old man!

Where is your probe command?
I think it should be something like this:

G91 G38.2 Z -50 F300; G92 Z 19.1; G0 Z 5

or double probing:

G91 G38.2 Z-50 F300;G90 G10 L20 P1 Z19.1;G0 Z10;G91 G38.2 Z-50 F100;G90 G10 L20 P1 Z19.1;G0 Z10

Take this with "grain of salt" have not tested it, yet.

Thanks for your prompt reply.
I do have the double probing commands in front of the G10L20P0Z19.1;G91G21G0Z10 sequence in the Candle parameters
and re-trying the system I DO get what appears to be a sensible result in that the machine position after probing is 29.1, which makes sense.
It may be that my probe test device actually measures 19.1 mm but when pressed by the probe some allowance needs to be made.
Also I was checking using paper beneath the probe on the work surface, and of course this does have some thickness.

BTW, I used the G10L20P0 sequence as I read somewhere that the use G92 was now discouraged.

Cheers, Don

OK, let me disassemble the following for you:

G91 G38.2 Z-50 F300; G90 G10L20P1Z19.1;G0 Z10;G91 G38.2 Z-50 F100;G90 G10 L20 P1 Z19.1;G0 Z10

G91 - Switch to incremental distance mode
G38.2 Z-50 F300 - Straight Probe, seek 50mm, speed 300mm/min, error if no contact
G10L20P1Z19.1 - Set Work Coordinate Origin (and resultant Offsets), set Z to probe height
G0 Z10 - pull up 10mm (remember still in incremental distance mode (G91)
G91 G38.2 Z-50 F100 - Straight Probe, seek 50mm, speed 100mm/min, error if no contact
G90 G10 L20 P1 Z19.1 - Set Work Coordinate Origin (and resultant Offsets), set Z to probe height
G0 Z10 - pull up 10mm

As you can see, G38.2 is the one that does the job for seeking for your touch plate, and I have not seen it in your first post

All relevant codes are explained here: https://wiki.shapeoko.com/index.php/G-Code

I should have been clearer:
The double probing sequence G21G91G38.2Z-30F100; G0Z1; G38.2Z-2F10 is the default in Candle Settings/Probing commands, and I just showed the commands I ADDED on the end.
I should have realised that not everyone is familiar with Candle.
Thanks for the explanation of the codes.
As I said, I do seem to have things OK, but might just have to tweak the Z19.1 bit to get things exact.
However, I have found that with the limited Z range of my 3018 machine, and the thickness of the workpieces that I may use, the Z probe I have purchased is too tall, and I shall have to fabricate a thinner one myself. The purchase was not wasted, though, as it gave me one element in my testing that I knew was OK.
Thanks for your help, ZASto

For Z probe I use a piece of single sided FR-4 PCB material. Thickness is 1,6mm :)
Instead alligator clip I use a neodymium magnet with hole for M3 screw, so if I forget to "unclip" it, no damage is done.

Works perfect with Mach3, bCNC and some other software.