Fadal Controls have a powerful Macro Language option.  Our Custom Macro Programming manual doesn't support Fadal macro but some of our users have been kind enough to submit Tips for Fadal Machining Centers.

A Face Milling Macro
Submitted by Fred Fikes (5/2/98)
Fred594@aol.com

A Face Milling Macro
Notice the use of the INPUT statement in this macro.  Why can't Fanuc and the rest add an INPUT statemtent to their language?

N1 O1000 (FACE MACRO PROGRAMMED BY FRED FIKE 4/25/98)
N2 M0 ( SAVE VARIABLES,BLOCK SKIP ON. RESET VARIABLES, BLOCK SKIP OFF)
/N3 #PRINT "ENTER LEFT EDGE POSTION IN X"
/N4 #INPUT V1
/N5 #PRINT "ENTER LOWER EDGE POSTION IN Y"
/N6 #INPUT V2
/N7 #PRINT "ENTER LENGTH OF WORKPIECE IN X"
/N8 #INPUT V3
/N9 #PRINT "ENTER WIDTH OF WORKPIECE IN Y"
/N10 #INPUT V4
/N11 #PRINT "ENTER CUTTER DIA."
/N12 #INPUT V5
/N13 #PRINT "ENTER SFM"
/N14 #INPUT V6
/N15 #PRINT "ENTER NUMBER OF FLUTES OR INSERTS"
/N16 #INPUT V7
/N17 #PRINT "CHIP LOAD"
/N18 #INPUT V11
N19 #PRINT "ENTER DEPTH OF CUT IN Z"
N20 #INPUT V8
N21 G0 G90 G80 G40 G49
N22 T1 M6
N23 #R0=V6/V5*3.82
N24 S+R0 M3 E1
N25 #R4=V7*V11
N26 #R5=R0*R4
N27 #:FWD
N28 #R0=V1+V3+V5/2+.25
N29 #R1=V2+V4
N30 X+R0 Y+R1
N31 Z1. M8 H1
N32 #R0=V8
N33 G1 Z+R0 F50.
N34 #R3=V2+V4
N35 #:WORK
N36 #R0=V1-V5/2-.25
N37 G1 X+R0 F+R5
N38 #IF R3=<V2+V5/2 THEN GOTO:END
N39 #R3=R3-V5/2
N40 G0 YR3
N41 #R0=V1+V3+V5/2+.25
N42 G1 XR0
N43 #IF R3=<V2+V5/2 THEN GOTO:END
N44 #R3=R3-V5/2
N45 G0 YR3
N46 #GOTO:WORK
N47 #:END
N48 G0 Z1.
N49 #PRINT "ENTER 1 IF PART CLEANED UP OR 0 IF PART DID NOT CLEAN UP"
N50 #INPUT V9
N51 #IF V9=0 THEN GOTO:HERE
N52 #GOTO:CONT
N53 #:HERE
N54 #PRINT "ENTER INCREMENT IN Z"
N55 #INPUT V10
N56 #V8=V8+V10
N57 #GOTO:FWD
N58 #:CONT
N59 M5 M9
N60 G49 Z0
N61 X0 Y0 E0
N62 M30
%>

Return to Top of Page