Ik was aan het stoeien met artcam, en merkte op dat de mach3 postprocessor die te vinden is op het web geen tool change ondersteund, waardoor je per tool een g-code bestand moet maken..
Ik heb dus wat kleine modificatie aangebracht in de postprocessor...
Wie weet loopt iemand hier ook tegen aan en heeft hij er baat bij..
Gr Robo
Code: Selecteer alles
;
; G - Code configuration file - with Arc Support
;
; History
;
; Who When What
; === ======== ========================================
; TM 13/05/99 Written
; BEM 20/05/99 Removed line numbers
; BEM 21/03/00 Added DESCRIPTION and FILE_EXTENSION fields
; BEM 19/06/01 Added support for circular arc output
; move to home pos at end instead of 0,0,ZH
; bem 07/09/01 Added G17 to define plane for circular arcs
; Robo20/07/09 Cleanup, Start, tool change, feedrate metric fix, name change
;
DESCRIPTION = "RoboCNC Mach3 Arcs Toolchange (mm) (*.tap)"
;
FILE_EXTENSION = "tap"
;
UNITS = MM
;
; Cariage return - line feed at end of each line
;
END_OF_LINE = "[13][10]"
;
; Block numbering
;
LINE_NUM_START = 0
LINE_NUM_INCREMENT = 10
LINE_NUM_MAXIMUM = 999999
;
; Set up default formating for variables
;
; Line numbering
FORMAT = [N|@|N|1.0]
; Spindle Speed
FORMAT = [S|@|S|1.0]
; Feed Rate
FORMAT = [F|#|F|1.0]
; Tool moves in x,y and z
FORMAT = [X|#|X|1.3]
FORMAT = [Y|#|Y|1.3]
FORMAT = [Z|#|Z|1.3]
; Arc Centre Cordinates
FORMAT = [I|@|I|1.3]
FORMAT = [J|@|J|1.3]
; Home tool positions
FORMAT = [XH|@|X|1.3]
FORMAT = [YH|@|Y|1.3]
FORMAT = [ZH|@|Z|1.3]
;
; Set up program header
;
START = "G00 G17 G21 G40 G49 G80 G90"
START = "T[T] M06 ([TOOLDESC])"
START = "G00 [ZH]"
START = "G00 [XH] [YH] [S] M03"
;
; Program moves
;
RAPID_RATE_MOVE = "G00 [X] [Y] [Z]"
;
FIRST_FEED_RATE_MOVE = "G01 [X] [Y] [Z] [F]"
FEED_RATE_MOVE = "[X] [Y] [Z]"
;
FIRST_CW_ARC_MOVE = "G02 [X] [Y] [I] [J] [F]"
CW_ARC_MOVE = "G02 [X] [Y] [I] [J]"
;
FIRST_CCW_ARC_MOVE = "G03 [X] [Y] [I] [J] [F]"
CCW_ARC_MOVE = "G03 [X] [Y] [I] [J]"
;
; Robo CNC Tool change
;
TOOLCHANGE = "G00 [ZH]"
TOOLCHANGE = "M05"
TOOLCHANGE = "T[T] M06 ([TOOLDESC])"
TOOLCHANGE = "[F] [S] M03"
;
; End of file
;
END = "G00 [ZH]"
END = "G00 [XH] [YH]"
END = "M30"