right at the top of the file we see (SketchUcam actually puts warnings into the Gcode)
G90 G21 G49 G17 F3
M3 S3000
G00 Z1.000
(Pass: 1)
X13.267 Y17.107
(PLUNGE Warning: limiting Z to min_z 1mm)
G01 Z1.000 F3

I see problems there....
the G21 indicates mm mode, but F3 says feed at 3mm a minute , really? that is very slow, in fact some controllers cannot even go that slow (though Mach is probably ok). But even cutting steel would/should be faster, I get 135 to 230mm/min for a 2 flute end mill at 1355 to 2371 RPM, assuming high carbon steel and an HSS tool. At 3mm/min your tool is rubbing more than cutting, making it blunt way before time.

The line (PLUNGE Warning: limiting Z to min_z 1mm) indicates that you have not set Z_MAX and Z_MIN correctly.
The setting is explained in the help, in the highlighted in red section entitled after install - things to do, which you can read here
http://swarfer.github.io/sketchucam/afterinstall.html
and you can also access via the big blue question mark in the SketchUcam toolbar right on your computer without needing an internet connection.

This is what the Gcode should look like
G90 G21 G49 G17 F3
M3 S3000
G00 Z1.000
(Pass: 1)
X13.267 Y17.107
G00 Z0.500 ; just above surface, surface is Z=0
G01 Z-1.000 F3 ; no warning message, and plunge down to first layer height of -1mm
G02 X12.7519 Y17.5024 I1.2515 J2.1642 F25
X12.3566 Y18.0175 I1.769 J1.7666
X12.1082 Y18.6174 I2.1659 J1.2485
X12.0234 Y19.2611 I2.4153 J0.6454
....

Tips:
1: for cutting steel, turn ramping on and ramp at 3 to 5 degrees.
2: for the holes, instead of the drawn circle with an inside cut, rather use a sized plunge hole.
With ramping on the bit will never plunge into the hole (end mills are bad at that!), instead ramping down in a spiral. For those 8mm holes it will do 2 cuts, one to clear the center (a 6mm hole), and another to bring it to final size. There are options for how it does that, one doing depth first, the other doing diameter first, so you need to read the help and use the setting that suites your machine.

 

so, solved yet @52Gary ?