Newbie- Spiral cutting macro

[jossiR1]

Hi All, Hope someone can help with my little problem.
I'm having trouble trying to m/c a spiral on a flat milled face, what i'm trying to achieve is basically create a turned finish in the form of a continuous spiral using a small pointy engraving tool. I have a macro to generate lots of circles incrementally but with the dwell and the start position being close together it leaves what looks like a line across the face which is not acceptable.

[Matt@RFR]

Do some research on G12/G13.

[christinandavid]

http://www.cnczone.com/forums/showthread.php?t=110522

Take a look at samu's posts #12 & #14 in this thread.

The only other alternative I know of for a precise spiral is many small linear moves - if your control is fast enough to perform calculations. A Heidenhain version of this method was discussed here: -

http://www.cnczone.com/forums/showthread.php?t=105697

DP

[Pondo]

Mastercam has a nice helix boring feature and Gibbscam has a threading feature that can be used the same way. They post out continuous helical spirals at whatever pitch you'd like, OD or ID. I'd approach it as if it were a very fine pitch thread you're cutting and I think it will turn out better.

[JWK42]

Here is a macro I use to mill spiral face grooves in out parts. Maybe you can adapt it to your needs




%
O5555 (SPIRAL GROOVE MACRO)
N30 ( WRITTEN 09-07-2010 08:42:13 )
N40 (MODIFIED 09-07-2010 13:45:59)
N50 #101=1 ( END MILL )
N60 G17 G54 G90
N70 G40 G49 G80
N80 G53 G00 Z0.
N90 G53 G00 X-16.0 Y0.
( TOOL #1 IS A MILL )
N110 G53 G00 Z0.0 ( RESTART TOOL #1 HERE )
N120 G53 G00 X-16. Y0.
N130 T#101 M6
N140 S124 M3
N150 G53 G00 Z4.0
N160 G54 G00 G90 X0. Y0.
N170 G43 Z2. H#101 D#101 M8
N180 #601=.1 ( STARTING RADIUS )
N190 #602=0 ( STARTING ANGLE ZERO = 3 O:CLOCK )
N200 #603=1 ( SET #603 TO -1 TO MINUS RADIUS 1 TO PLUS RADIUS )
N210 #613=-1 ( SET #613 TO -1 FOR CLOCKWISE MILLING 1 FOR C-CLOCKWISE )
N220 #604=.25 ( FULL CIRCLE PITCH OF ONE GROOVE )
N230 #605=90 ( NUMBER OF STEPS PER 360 DEGREE CIRCLE )
N240 #615=4 ( NUMBER OF FULL OR PARTIAL CIRCLES OR GROOVES )
N250 #625=6 ( CUTTING FEED RATE )
N260 #626=3 ( PLUNGING FEED RATE )
N270 ( END OF INPUTS )
N280 #624 =[#615*#605] ( TOTAL NUMBER OF STEPS )
N290 #606=[[#604/#605]*#603] ( STEP RADIUS )
N300 #608=[[360/#605]*#613]( STEP DEGREES )
N310 IF[#613 EQ 1]#623=3 ( MILL C-CLOCKWISE )
N320 IF[#613 EQ -1]#623=2 ( MILL CLOCKWISE )
N330 #610=[COS[#602]*#601]
N340 #611=[SIN[#602]*#601]
N350 G00 X#610 Y#611
N360 Z.1
N370 G01 Z-0.25 F#625
N380 WH[#624 GT 0]DO1
N390 #624=[#624-1]
N400 #601=[#601+#606]( STEP RADIUS )
N410 #602=[#602+#608]( STEP DEGREES )
N420 #610=[COS[#602]*#601]
N430 #611=[SIN[#602]*#601]
N440 #612=[SQRT[[#610*#610]+[#611*#611]]]
N450 G#623 X#610 Y#611 R#612 F#626
N460 END1
N470 G01 Z.1 F50.
N480 G53 G00 Z0. M9
(UNLOAD HERE)
N500 G53 G00 X-16. Y0.
N510 M30 (END OF MAIN PROGRAM)
%

[christinandavid]

Originally Posted by JWK42 N450 G#623 X#610 Y#611 R#612 F#626 %

Sorry - couldn't resist...

DP

[JWK42]

DP

By golly you are right. We fixed it at the machine but never in the office. It does work pretty well. I have never used it to mill a round hole. Would have to add a line to make a full circle cut after the final spiral.