Do you know if it's a CN10 control. I program for a 1998 Masterwood 327 with a CN10.
There's a roughly 10 line header in the g-code file that contains the part x, y, and z dimensions and some other stuff, including the machine park position for that particular part. Say your running a small part at the far end of the machine, you can have the machine park close to the part instead of going home after each part.
As for the G-code itself, it's not standard code, but it's close.
First, there are no rapid moves. The machine does them automatically.
To route, the first line is the start location of your route, and starts with G172, and subsequent lines are either G101, G102, or G103. These are the same as standard G1,G2 and G3 codes. Feed rates are probably in meters/minute. F2 = 2 meters per minute, S is spindle speed in thousands of RPM.
So, say you want to route a 100mm square with the lower left corner at 0,0 here's what you do. Lets use a 16,000rpm spindle speed and a feedrate of 2m/min. YOU also need to call the tool number of the router. We have two, tools #41 and 42. Our tool 41 has an ATC, so it's called as 41/1, 41/2..... 41/5 (for 5 position tool changer). You can also specify an entry (plunge) rate with the E word, as the first move will plunge into the part if the starting Z depth is not 0. Z zero is the top of the part, and Z+ is down into the part.
G172 X0 Y0 Z2 S16 T41 E1
G101 X100 Y0 Z2 F2
G101 X100 Y100 Z2 F2
G101 X0 Y100 Z2 F2
G101 X0 Y0 Z2 F2
This is routing 2mm deep.
You can also use cutter comp with G41/G42, but you must have a lead-in and lead out move.
Something like this. Also just remebered that Y+ is down, so I'd actually program this way. I also ramp in and out during the lead-in and lead out:
G172 X-10 Y-10 Z0 S16 T41 E1
G41
G101 X0 Y-10 Z2 F2
G101 X0 Y100 Z2 F2
G101 X100 Y100 Z2 F2
G101 X100 Y0 Z2 F2
G101 X-10 Y0 Z2 F2
G40
G101 X-10 Y-10 Z0 F2
To drill holes, use G100
G100 X10 Y10 Z10 T5
will drill a 10mm deep hole at 10,10 with tool #5. To drill multiple holes at the same time, you create a sort of "vitrual tool".
I think it's something like:
#T81 = 1,2,3,4
#X81 = 4,3,2,1
G100 X10 Y10 Z10 T81
This will drill 4 holes with tools 1-4, with tool #1 at 10,10 and all 10mm deep.
The X81 reverses the tools if the program is run in a mirrored runfield, if your machine has mirrored runfields.
I don't have access to a manual until Monday, but let me know if you need any more info. If this works at all.