1. A job with many holes that have to be spotted, drilled, and tapped. Your CAD/CAM will repeat the hole pattern for each tool. Each tool has to be set up in the CAD/CAM, and instructed to process the points. All this takes time. After processing, the hole pattern is listed in full for each tool. This may make the CNC file hundreds of lines longer than necessary!
N10 G00 G20 G40 G49 G80 G90 G98
(1/4" SLOT DRILL)
N12 T3 M06
N14 S10000 M03
N16 G00 G54 G43 X0.25 Y0.1 Z1. H03 M08
N18 Z0.1
N20 G99 G81 Z.1 R.05 F12.
N22 X0.5 Y0.1
N24 X0.75 Y0.1
N26 X1.0 Y0.1
N28 X1.25 Y0.1
.
.
many points
.
.
N446 G80 M09
(13/64" DRILL)
N448 T4 M06
N450 S3761 M03
N452 G00 G54 G43 X0.25 Y0.1 Z1. H04 M08
N454 Z0.1
N456 G99 G73 Z1. R.05 Q.1 F18.
N458 X0.5 Y0.1
N460 X0.75 Y0.1
N462 X1.0 Y0.1
N464 X1.25 Y0.1
.
.
many points
.
.
N882 G80 M09
(1/420unc TAP)
N884 T3 M06
N886 S1000 M03
N888 G00 G54 G43 X0.25 Y0.1 Z1. H03 M08
N890 Z0.1
N892 G99 G84 Z.75 R.05 F50.
N894 X0.5 Y0.1
N896 X0.75 Y0.1
N898 X1.0 Y0.1
N900 X1.25 Y0.1
.
.
many points
.
.
N1318 G80 M09
etc.
Consider doing it this way:
Just process one tool in your CAD/CAM. After postprocessing, use EditCNC to convert the hole pattern to a subroutine, copy, paste and edit the one tool to make three. Add a sub call to the tools and voila! You have a program that's quicker to make, and perhaps hundreds of lines shorter! AND... if the hole pattern is a circle or grid, you can do the whole thing with EditCNC!
N10 G00 G20 G40 G49 G80 G90 G98
(1/4" SLOT DRILL)
N12 T3 M06
N14 S10000 M03
N16 G00 G54 G43 X0.25 Y0.1 Z1. H03 M08
N18 Z0.1
N20 G99 G81 Z.1 R.05 F12.
N22 M97 P1000
N24 M09
(13/64" DRILL)
N26 T4 M06
N28 S3761 M03
N30 G00 G54 G43 X0.25 Y0.1 Z1. H04 M08
N32 Z0.1
N34 G99 G73 Z1. R.05 Q.1 F18.
N36 M97 P1000
N38 M09
(1/420unc TAP)
N40 T3 M06
N42 S1000 M03
N44 G00 G54 G43 X0.25 Y0.1 Z1. H03 M08
N46 Z0.1
N48 G99 G84 Z.75 R.05 F50.
N50 M97 P1000
N52 M09
N54 G91 G28 Y0 Z0
N56 G90
N58 M30
N1000 (P1000: HOLE PATTERN)
N1002 X0.5 Y0.1
N1004 X0.75 Y0.1
N1006 X1.0 Y0.1
N1008 X1.25 Y0.1
.
.
many points
.
.
N426 G80
M99
%
2. A job with several identical pockets, each with roughing and finishing cuts. If programmed on your CAD/CAM, every move makes a line in the CNC file. Use the CAD/CAM to make one pocket, and, as in the example above, convert the cuts to a subprogram to be repeated. You can use the G90/G91 facility in EditCNC to convert the pocket cuts to incremental coordinates. That way, the subprogram can be repeated anywhere on the machine.
An added bonus to this method is that any alterations to the pocket, contour or hole pattern can be made in the subprogram rather than reprocessing a whole program on your CAD/CAM.
