Advice on converting Machine Code from Imperial to Metric

[JAZZCNC]

Mach 3 uses generic Fanuc code that's why it works.

The fact it only uses one X coordinate on line #4 makes no difference to mach3. Without seeing the rest of the code and knowing what it's cutting then difficult to say if good or bad code.

Just changing G20 to G21 isn't enough for it to work correctly. G21 will make it the correct size but it won't change the feed rates so all the F codes will be wrong. For instance, F20 on line #8 will mean you'll travel at 20 mm/min instead of 20 inches a minute which was originally coded. So you'll need to multiply all the F numbers by 25.4 to get the correct mm/min feed rate.

When using imperial G-code it's easier to set up an imperial profile in mach3 as this will avoid the feed rate issue.
It's simple to do, just copy the profile you are using now, change the units to imperial, and change all the Steps per settings by multiplying them by 25.4 because now mach3 is working in STEPS PER INCH rather than STEPS PER MM
So let's say you have the STEPS PER at 160, which is a common metric setting if using 10mm pitch screws with 1600 micro steps set on the drives with no ratios applied. This now needs to be 160 x 25.4 = 4064 STEPS PER INCH.

The Velocity and acceleration are the opposite, now you divide by 25.4 because let's say you are set for 10,000 mmm/min this will become 10,000 Inch/Min.!!!

Then restart Mach3 for the units to reset.