This is the style of program I use for facing various size one offs on a vertical cnc. I have omitted all the stuff about tool selection, rpm, etc., this is just the tool path for a 3/4" dia. tool facing 18 inches by 14 inches.
N100 G54 X0. Y0.
N101 Z0.
N102 G91 G01 Y-0.74 F100. M97 P1000 L10
N103 G28 M30
N1000 G90 X-19.5
N1001 G91 Y-0.74
N1002 G90 X0. M99
Comments:
Line N100; Put the work zero slightly more than one tool diameter positive from the corner of the workpiece nearest machine zero.
N101 Set tool offset at the finished surface.
N102 This increments the Y slightly less than one tool diameter and calls the subroutine starting at N1000 ten times.
N1000 The uses absolute positioning to face across the X distance.
N1001 This increments the Y again.
N1002 This returns in absolute back to X 0. and returns from the subroutine.
The Y travel for each call of the subroutine is 1.48" and the total Y travel is 14.8". For different size cutters and different size parts it is only necessary to change the Y increment, the X travel and the L count.  |