Hi,
the instruction on pg 41 is correct, namely you can start a program from any line.....however it may not work as you expect. Gcode programs are modal, always have been. For example
this is a drill file I use regularly for drilling holes in a PCB:
Code:
G0 Z2
M3 S24000
G4 P6.00
N00150 G82 X-31.9900 Y8.5500 Z-2.5000 F300 R2.0000 P0.100000
X-32.0100 Y29.5100
X-42.4900 Y19.0000
X-21.4600 Y19.0600
N00250 G82 X-53.2800 Y13.4700 Z-2.5000 F300 R2.0000 P0.100000
X-55.2800 Y13.4700
X-57.2800 Y13.4700
X-59.2800 Y13.4700
X-61.2800 Y13.4700
X-63.2800 Y13.4700
N00370 G82 X-31.4500 Y48.9100 Z-2.5000 F300 R2.0000 P0.100000
X-37.6750 Y3.4250
X-45.3500 Y38.8500
X-46.5500 Y64.0000
X-49.3750 Y13.4250
X-49.4500 Y38.9000
X-53.0500 Y38.8500
X-5.4500 Y27.3000
X-56.1250 Y18.8750
X-57.7500 Y38.8000
X-58.1500 Y73.6000
X-58.7250 Y18.7750
X-61.2500 Y18.7000
X-63.8000 Y18.7000
X-12.6500 Y38.5000
X-14.6500 Y36.0000
X-18.4000 Y35.3500
X-20.2500 Y39.4000
X-20.6250 Y36.8250
X-21.5500 Y3.8500
X-25.8000 Y62.8500
N00640 G82 X-38.7400 Y12.2900 Z-2.5000 F300 R2.0000 P0.100000
X-38.7400 Y25.7300
X-25.2900 Y25.7500
X-25.3400 Y12.2700
G0 Z50
X0 Y0
M30
At the top of the file the spindle is turned on and run at 24000rpm (M3 S24000 )
Note that once Mach has read one of the drill cycle lines, for example:N00370 G82 X-31.4500 Y48.9100 Z-2.5000 F300 R2.0000 P0.100000
that each subsequent line is interpreted as a new hole at the XY location on the line but with the other parameters as has been set by the previous drill cycle line.
If you attempt to start Mach at this line the spindle will not start, I mean Mach hasn't read it so why would it start? It would interpret: X-49.3750 Y13.4250
probably as a linear G0 move, it would have no idea that it's supposed to drill a hole, it has not read the drill cycle line and so is not in drill mode.
In order for a line of Gcode to be interpreted correctly Mach needs the history of the job so that it knows what mode its in otherwise it may well misinterpret what its supposed to do.
Another example is something like this:
g0 x0 y0
g91
g1 x10 y10 f500
g1 x10 y10
g1 x10 y10
Because of the g91, ie incremental mode each successive line:g1 x10 y10 will cause the machine to advance 10 mm in X and 10mm in Y. If you started the code at;g1 x10 y10 f500
when the machine is still in absolute mode, Machs normal mode, then it will drive to x10 y10 but then stay there. Only if its in incremental mode would it carry on.
I suggest you do some experiments because if you have a clash between absolute/incremental mode you will get wildly unexpected results. Its for this reason that <Run From Here> was invented
way back in Mach3 days. Mach4 needs it also.
Craig