Making it smaller,

[CharlieM]

I wrote this code to cut an elipse out of 1/8" plate.

Sence I don't know how to use cutter comp, this is a tool path useing a 3/16 Dia. end mill.

After cutting the elipse, I want to make it .003 smaller all around.

What would my code look like?


G01 X.1875 Y.0000 F4
G02 X.3318 Y.3379 R.4675
G02 X.5654 Y.4975 R.7308
G02 X1.3721 Y.4975 R1.0338
G02 X1.6056 Y.3379 R.7308
G02 X1.6056 Y-.3379 R.4675
G02 X1.3721 Y-.4975 R.7308
G02 X.5654 Y-.4975 R1.0338
G02 X.3318 Y-.3379 R.7308
G02 X.1875 Y.0000 R.4675
G00 X.0000 Y.0000

Thanks for any help.

Charlie

[dcoupar]

You didn't say what control you're programming for, so assuming Fanuc style, put 0.0015 in D offset #10.

G01 G42 X.1875 Y.0000 D10 F4
G02 X.3318 Y.3379 R.4675
G02 X.5654 Y.4975 R.7308
G02 X1.3721 Y.4975 R1.0338
G02 X1.6056 Y.3379 R.7308
G02 X1.6056 Y-.3379 R.4675
G02 X1.3721 Y-.4975 R.7308
G02 X.5654 Y-.4975 R1.0338
G02 X.3318 Y-.3379 R.7308
G02 X.1875 Y.0000 R.4675
G00 G40 X.0000 Y.0000

[JWK42]

CharlieM
This macro is written for a Haas control but if you have macro programming available you can adapt it for your use. The macro finds the tool radius or diameter from your tool table and uses it to do either inside or outside milling around the ellipse. Or you can set #606 manually the same the other variables. You can change from climb to conventional milling by changing the G word in N450 to G2 or G3 to suit your needs. You can also make multiple passs around the ellipse.


%
O1154 (ELLIPSE MACRO)
N10 (WRITTEN 08-18-2008 14:48:01)
N20 (RETURNED 11-24-2008 09:57:26)
N30 G17 G54 G90
N40 G40 G49 G80
N50 G53 G00 Z0.
N60 G53 G00 X-20. Y0.
N70 T1 M06
N80 #601= 4 (ELLIPSE WIDTH IN X AXIS)
N90 #602= 2 (ELLIPSE HEIGHT IN Y AXIS)
N100 #603= 0 (CENTER OF ELLIPSE IN X AXIS)
N110 #604= 0 (CENTER OF ELLIPSE IN Y AXIS)
N120 #650= 0.125 (DEPTH OF EACH MILLING PASS IN Z AXIS)
N130 #651= 3 (NUMBER OF MILLING PASSES)
N140 #652= 0 (TOP OF PART IN Z AXIS)
N150 #625= 180 (ENTER NUMBER OF POINTS TO PLOT 32 IS MINIMUM)
N160 #616= 1 (ENTER 1 FOR OUTSIDE MILLING -1 FOR INSIDE MILLING)
N170 #626= 1 (ENTER TOOL NUMBER)
N180 #606= #[ 2400 + #626 ] ( FIND TOOL RADIUS FROM TOOL TABLE)
N190 (FOR DIAMETER TOOL TABLE REMOVE PARENTHESES BELOW )
N200 ( #606= [ #606 / 2] )
N210 IF [ #625 LT 32.0 ] #625= 32.0
N220 #606= [ #606 * #616 ]
N230 #645= [ #625 / 4 ]
N240 #644= [ FIX[ #645 ] ]
N250 #643= [ #644 * 4.0 ]
N260 #605= #643
N270 #601= [ [ #601 / 2 ] + #606 ]
N280 #602= [ [ #602 / 2 ] + #606 ]
N290 #607= [ 2 * [ 3.14159 / #605 ] ]
N300 #607= [ #607 / 0.017453 ]
N310 #610= [ #601 + #603 ]
N320 G00 X#610 Y#604
N330 Z [ #652 + 0.125 ]
N340 G01 Z#652 F6.
N350 WH [ #651 GT 0 ] DO1
N360 G91
N370 G01 Z - #650 F3.
N380 G90
N390 #608= 1.
N400 WH [ #605 GT 0 ] DO2
N410 #620= [ #602 * [ SIN[ #607 * #608 ] ] + #604 ]
N420 #621= [ #601 * [ COS[ #607 * #608 ] ] + #603 ]
N430 #622= SQRT[ [ #620 * #620 ] + [ #621 * #621 ] ]
N440 #622= [ #622 + 0.0005 ]
N450 G03 X#621 Y#620 R#622 F20.
N460 #608= [ #608 + 1 ]
N470 #605= [ #605 - 1 ]
N480 END2
N490 G01 X#610 Y#604
N500 #605= #643 (RESET COUNT)
N510 #651= [ #651 - 1 ]
N520 END1
N530 G01 Z [ #652 + 0.125 ] F50
N540 G53 G00 Z0. M09
N550 G53 G00 X-20. Y0. A0.
N560 M30 (END OF MAIN PROGRAM)
%