XNC.ini README NOTES
=============================

There are multiple Biesse machine models.
Earlier machines such as the 24FT usually expected Gcode files to have extension .XNC
Later models such as RoverG6 and Klever expect .ISO as the file extension.
The driver itself produces a .TMP temporary file which is then postprocessed to become the required .XNC or .ISO
----------------------------------------------------------------------------------------------------------------

The optional ini file XNC.ini has these parameters:


headerstyle2
		When present, this takes over as the style for creation of the header line(s).
		This style always starts this way...
			N10 G71 HC=1 LX=3600.00 LY=1200.00 PLPZ=16.0 LZ=16.00 rest-of-header-line
		where the X Y Z values are substituted and the rest-of-header-line is a copy of the headerstyle2 string supplied.

		For example:
			headerstyle2 = "PCSG=0.0 PDM=0 PUOS=0 NFIL=1 FIL=1 BLO=0 ACC=0 RUO=0 KA=1"
		with a sheet size of 2400 x 1200 and thickness 32mm would create a header line like this:

			N10 G71 HC=1 LX=2400.00 LY=1200.00 PLPZ=32.0 LZ=32.00 PCSG=0.0 PDM=0 PUOS=0 NFIL=1 FIL=1 BLO=0 ACC=0 RUO=0 KA=1


labelpath
		When label ZPL files are generated they are placed in the same folder as the ISO file initially.
		These have to be transferred to the machine and placed in some folder where the controller can pick them up.
		Here we specify the path to this folder, so this will be referenced in the ISO file instead of the actual path.

		For example:
			labelpath = "C:\WNC\Home\d_xnc\p_p\Prog\Labels\"
		...would cause the ISO file to be generated with label reference paths like this:
			N60 ST1="C:\WNC\Home\d_xnc\p_p\Prog\Labels\"
		Note the trailing backslash must be supplied in the path string quoted above


platefix
		If present and set to 1, this allows driver to guess and fix SINGLE PART plate x,y orientation in the header line.
		EzyNest versions 4.2.0.6 and earlier can get the plate orientation wrong in single part processing

		Default is same as
			platefix=0

sawtool
		An extra tool number can be specified here for the saw.
		For example, if there are actually 8 tools in the toolchanger turret, specify 9 in your setup and then add this line to scm.ini:
			sawtool=9
		Then when you use tool 9 to make cuts in the X or Y directions, and you will get Gcodes generated to use the saw (aggregate tool).

drillNoVF
		If present and set to 1, this suppresses the VF=feedrate element in the drilling lines
		Default is same as drillNoVF=0

ZSafetyCheck
		If present, Z depths are limited in this way:

		Routing Z Safety Check, don't allow z < -ZSafetyCheck
		Drilling Z Safety Check, don't allow z depth > ZsafetyCheck


----------------------------------------------------------------------------------------------------------------
Also the XNC driver has this additional way of controlling output:



   The drill cycle G98 or G99 selection can now be overridden by the use of pecklift as a flag.
   Here's the new logic:

   When setting up the drill strategies, if you set pecklift zero, then the old logic applies.
   That is, if the hole is a through hole, then select G98 (slow) else G99 as the drill cycle.

   If you set pecklift nonzero, then its value is used to select G98 or G99.
   A value of 0.5 (or anything < 0.9) selects the slow cycle G98.
   A value of 1.0 (or anything > 0.9) selects the fast cycle G99.