[Camdude]

Guys, i am in need of some sample code for a puma2000sy with live tools.
i am looking for a threadmill cycle for a1/4-18 thread mill cycle on the side of the part(G19) . my code does not work and i can't find any samples in the operator/program manual.

thanks, phil

[cnc-king]

have you tried your cam system to generate your code. the code will look goofy but it actually works. i am threadmilling a 24 pitch thread on the side of a part in the lathe at the moment and this is what MCX3 generated. this actually cuts a perfect thread


PARTIAL CODE



N10
(TOOL - 10 OFFSET - 10)
( .235 24 PITCH THREAD MILL)
( G54 FIN 5/16-24 THREADS )
M110
G54 G40
G19
G30 U0. V0.
G30 W0.
M35
M290
G30 H0.
G0 C0.
T1010
G97 S4500 M33
G98
M90
G0 C180.
M89
M8
G0 X.97 Z-.179
X.49
G1 G41 Y.0388 F5.
X.4935
Y.0374 Z-.169
X.4969
Y.0336 Z-.1596
X.5004
Y.0274 Z-.1516
X.5039
Y.0194 Z-.1454
X.5074
Y.01 Z-.1416
X.5108
Y0. Z-.1402
X.5143 Z-.1403
Y-.01 Z-.1416
X.5178
Y-.0194 Z-.1454
X.5212
Y-.0274 Z-.1516
X.5247
Y-.0336 Z-.1596
X.5282
Y-.0374 Z-.169
X.5317
Y-.0387 Z-.179
X.5351 Y-.0388
Y-.0374 Z-.189
X.5386
Y-.0336 Z-.1984
X.5421
Y-.0274 Z-.2064
X.5456
Y-.0194 Z-.2126
X.549
Y-.01 Z-.2164
X.5525
Y0. Z-.2177
X.556 Z-.2178
Y.01 Z-.2164
X.5594
Y.0194 Z-.2126
X.5629
Y.0274 Z-.2064
X.5664
Y.0336 Z-.1984
X.5699
Y.0374 Z-.189
X.5733
Y.0387 Z-.179
X.5768 Y.0388
Y.0374 Z-.169
X.5803
Y.0336 Z-.1596
X.5837
Y.0274 Z-.1516
X.5872
Y.0194 Z-.1454
X.5907
Y.01 Z-.1416
X.5942
Y0. Z-.1403
X.5976
Y-.01 Z-.1416
X.6011
Y-.0194 Z-.1454
X.6046
Y-.0274 Z-.1516
X.6081
Y-.0336 Z-.1596
X.6115
Y-.0374 Z-.169
X.615
Y-.0387 Z-.179
X.6185 Y-.0388
Y-.0374 Z-.189
X.6219
Y-.0336 Z-.1984
X.6254
Y-.0274 Z-.2064
X.6289
Y-.0194 Z-.2126
X.6324
Y-.01 Z-.2164
X.6358
Y0. Z-.2177
X.6393 Z-.2178
Y.01 Z-.2164
X.6428
Y.0194 Z-.2126
X.6462
Y.0274 Z-.2064
X.6497
Y.0336 Z-.1984
X.6532
Y.0374 Z-.189
X.6567
Y.0387 Z-.179
X.6601 Y.0388
Y.0374 Z-.169
X.6636
Y.0336 Z-.1596
X.6671
Y.0274 Z-.1516
X.6706
Y.0194 Z-.1454
X.674
Y.01 Z-.1416
X.6775
Y0. Z-.1403
X.681
Y-.01 Z-.1416
X.6844
Y-.0194 Z-.1454
X.6879
Y-.0274 Z-.1516
X.6914
Y-.0336 Z-.1596
X.6949
Y-.0374 Z-.169
X.6983
Y-.0387 Z-.179
X.7018 Y-.0388
Y-.0374 Z-.189
X.7053
Y-.0336 Z-.1984
X.7087
Y-.0274 Z-.2064
X.7122
Y-.0194 Z-.2126
X.7157

[Camdude]

CNC-King
using much simpler code to program on Y-axis.
G50S2000
G00T1010
M35
G28H0
G98
G97S2250M33
M8
G19
C90.
G00X3.775Z-.4564Y0 (rapid position)
G1G98X2.37F50. (tool position inside hole)
G1G41Z-.4014F4. (active CC Z distance = K)
G3K-.055X2.481 (K = difference between major dia and tool dia.)
(x = pitch)
G1G40Z-.4564F50. (tool to center of hole)
this cuts a 1/4_18 NPT with a NPT thread mill

[cnc-king]

I see it is much simpler, did your cam system generate that code? I stopped doing any manual programming since we have Mcam to do that for us. I let MCamX3 generate all my codes. Programs go to the machine with no manual edits needed by me or the operator. If any changes for rpm or feedrates they are incorporated in MCam so it becomes easy if there is a rev change etc.

[Camdude]

Na, had to do it myself as i am now a CAMWORKS user. I used MCAM for about 13 years but new job made me switch. MCAM much easer to configure and use. I really miss it.