[HPT]

FANUC controller I use can not handle circular milling with G12/G13. I need to enlarge the hole from 4.0" to 4.6". Is there any other way to do this with FANUC?

[mrainey]

Have you tried using G02/G03?

[HPT]

G02/G03 wouldn't be a short program if compared to G12/G13.

[mrainey]

Half a dozen lines instead of one don't seem like too much. If you had a number of the holes to do on the part, you could put the lines in an incremental subroutine. For long-term use, maybe you could simulate G12/G13 by creating a macro with variables.

[mrainey]

Here's an example I found at CNC Concepts ( www.cncci.com ). They have a ton of useful manual programming tips there.

GREETINGS FROM SOUTH AFRICA! I HAVE RECENTLY STARTED PROGRAMMING IN MACRO B AND HAVE WRITTEN THIS PROGRAM TO CUT PILLAR HOLES, ETC IN MOULD PLATES. THIS PROGRAM CUTS A HOLE OF ANY DIAMETER AT ANY POSITION WITH ANY DEPTH OF CUT USING ANY DIAMETER CUTTER. THERE IS NO NEED FOR RADIUS COMPENSATION AS YOU CAN CHANGE THE CUTTER DIAMETER OR THE HOLE DIAMETER TO GET THE SIZE YOU REQUIRE. YOU CAN SET THE DEPTH OF CUT TO MORE THAN THE TOTAL DEPTH OF THE HOLE TO JUST TAKE ONE CUT. THE 180 DEG. LEAD-IN AND LEAD-OUT WITH A RADIUS PLACES LESS STRAIN ON THE CUTTER AS IT COMES INTO CONTACT WITH THE MATERIAL TO BE CUT. HERE IS THE PROGRAM :

:8000(PILLAR HOLES)
#100=1.0(CUTTER DIAMETER)
#101=30.0(X CENTRE)
#102=30.0(Y CENTRE)
#103=0.0
#104=30.0(DEPTH OF HOLE)
#105=50.0(DIA OF HOLE)
#106=3000(SPNDLE SPEED)
#107=500.0(FEED)
#108=10(TOOL POS)
#110=20.0(DEPTH OF CUT)
G00G91G28Z0.0
G91G28X0.0Y0.0
T#108M06
G00G90G54X#101Y#102S#106M03
G43Z10.0H#108M08
N1WHILE[-#104LE#103]DO1
#103=[#103-#110]
IF[-#104GT#103]GOTO20
G1Z#103F[#107/3]
G03X[#101+#105-#100/2]R[[#105-#100]/4]F#107 I-[#105/2-#100/2]J0.0
X#101R[[#105-#100]/4]
G00Z10.0
END1
N20#103=-#104
G01Z#103F[#107/3]
G03X[#101+#105-#100/2]R[[#105-#100]/4]F#107[[#10-#100]/4]
G00Z10.0 M09
G00G91G28Z0.0
G91G28X0.0Y0.0
M30

[HPT]

Thanks!
This will help.

[timlkallam]

Here is a link to a circle milling program its free .
www.kentechinc.com/tip7.html