PROGRAMMING
96-8000
141
June 1999
4.2 PROGRAM S TRUCTURE
A CNC part program consists of one or more blocks of commands. When viewing the program, a block is the
same as a line of text. Blocks shown on the CRT are always terminated by the îš“ ; îš“ symbol which is called an
EOB. Blocks are made up of alphabetical address codes and the îš“ / îš“ symbol. Address codes are always an
alphabetical character followed by a numeric value. For instance, the specification of the position to move the X-
axis would be a number preceded by the X symbol.
The îš“ / îš“ symbol, sometimes called a slash, is used to define an optional block. A block that contains this
symbol can be optionally deleted with the BLKDEL button when running a program.
There is no positional requirement for the address codes. They may be placed in any order within the block.
The following is a sample program as it would appear on the CRT. The words following the îš“:îš” are not part of the
program but are put here as further explanation.
This program will drill four holes and mill a two-inch hole in a four-inch square plate with X and Y zero at the
center. The program with comment statements would appear like this.
% :PROGRAM MUST BEGIN AND END WITH %
O1234 (OP1 SAMPLE MILL PART) :PROGRAM # AND COMMENT STATEMENT
N1 (TOOL #1 IS A ½ INCH STUB DRILL) :(******) NOTES TO OPERATOR
N5 G40 G49 T#1 M06 :
N100 G00 X0 Y0 Z.5 G43 H1 M3 S1400 T2 :RAPID TO POS, OFFSET 1, SPIN FWD
N101 G01 Z.2 F30. :FEED 30 INCH/MINUTE TO Z DEPTH
N102 G83 G98 Z-.625 R.03 Q.2 F5. :PECK TO Z-.625 START .03 ABOVE
N103 X1.5 Y1.5 :DRILL ANOTHER HOLE AT NEW X,Y
N104 Y-1.5 :DRILL 3RD HOLE, PECK DEPTH IS .20
N105 X-1.5 :DRILL FOURTH HOLE
N106 Y1.5 :DRILL FIFTH HOLE
N107 G00 G80 Z.5 :CANCEL CANNED CYCLE
N108 T2 M06 :TOOL CHANGE TO TOOL #2
N2 (T #2 IS 5/8 90 DEG. COUNTERSINK) :N### ARE LINE NUMBERS
N200 G00 X0 Y0 Z.5 G43 H2 M3 S500 :OFFSET 2, SPINDLE SPEED 500 RPM
N201 G01 Z.2 F30. :FEED TO Z AT 30 INCH PER MINUTE
N202 G82 G98 Z-.27 R.0 F5. :SPOT DRILL CYCLE, DRILL AT X0 Y0
N203 X1.5 Y1.5 :SEC HOLE R=START PLANE ABOVE ZERO
N204 Y-1.5 :3RD HOLE G98=RETURN TO INIT POINT
N205 X-1.5 :FOURTH HOLE
N206 Y1.5 :FIFTH HOLE
N207 G00 G80 Z.5 :RAPID TO Z.5
N208 G28 X0 Y0 Z2.0 :ZERO RETURN AFTER MOVE TO X0, Y0
N209 T#3 M06 :TOOL CHANGE
N3 (TOOL #3 IS A ½ END MILL) :N #S ARE FOR YOUR CONVENIENCE
(SET DIAMETER VALUE TOOL #3) :COMMENTS ARE IGNORED BY CONTROL
N300 G00 X0 Y0 Z.5 G43 H3 M3 S1000 :G43 = OFFSET Z IN MINUS DIRECTION
N301 G01 Z.2 F30. :G01 CAN BE SPECIFIED AS G1
N302 Z-.625 F5. :FEED TO DEPTH
N303 G01 G41 X-1.00 :COMPENSATE CUTTER LEFT OF LINE
N304 G03 I1.0 D1 :CUT CIRCLE CCW WITH TOOL DIA D1
N305 G00 G40 X00 :RAPID TO CENTER, G40 CANCELS COMP
N306 G00 Z.5 :RAPID OUT OF PART
N307 G28 :ZERO RETURN, Z GOES FIRST THAN X,Y
M30 :RESET PROGRAM TO BEGINNING
% :END OF TAPE
To Next Page
Loading...
Need help?
General
