Circular movement under M128

[davidtan20]

The following program is about a simple pocket at YZ plane, linear moves are ok, but machine refuses circular moves, says "too small radius for circular move",is that true under M128 machine can't do circular move except under XY plane?


16 CYCL DEF 7.0 DATUM SHIFT
18 CYCL DEF 7.1 X 0.0000
20 CYCL DEF 7.2 Y 0.0000
22 CYCL DEF 7.3 Z 0.0000
24 CYCL DEF 247 DATUM SETTING ~
Q339=+1 ; DATUM NUMBER
26 TOOL CALL 10 Z S3500
28 TOOL DEF 10
30 M13
38 L B-119.36 C1.113 FMAX
40 M128
44 L X-1. Y.7307 FMAX
46 L Z-1.0511 FMAX
48 L X-.1 F500.
50 L X-.0818 Y.7806 Z-1.0518 F200.
52 L X-.0636 Y.828 Z-1.068
54 L X-.0455 Y.8686 Z-1.0973
56 L X-.0273 Y.8989 Z-1.1372
58 L X-.0091 Y.9162 Z-1.1842
60 L X.0091 Y.9191 Z-1.2342
62 L X.0273 Y.9073 Z-1.2829
64 L X.0455 Y.8817 Z-1.3259
66 L X.0636 Y.8447 Z-1.3597
68 L X.0818 Y.7995 Z-1.3812
70 L X.1 Y.75 Z-1.3875
72 L Y.6875 F500.
74 L Z-1.2625
76 L Y.8125
78 L Z-1.3875
80 L Y.75
82 L Z-1.575 F200.
84 L Y.5
86 L Z-1.075
88 L Y1.
90 L Z-1.575
92 L Y.75
94 L Z-1.7625
96 L Y.375
98 CC X.1 Y.375
100 C X.1 Y.3125 DR+
102 L Z-.95
104 CC X.1 Y.375
106 C X.1 Y.375 DR+
108 L Y1.125 Z-.8875
110 CC X.1 Y1.125
112 C X.1 Y1.1875 DR+

222 L X-19.5 FMAX M91
224 L Y-.1 FMAX M91
226 L B0.0 C0.0 FMAX
228 M30
230 END PGM 100 INCH

 

[Jaydenn]

Davidtan,
To me, the first step will be to delete the M128 and try to run the program. Does it work?
If it runs, then you have your answer...

Second, you say you are pocketing in the "YZ" plane, but your "TOOL CALL" specifies that "Z" is the primary plane. If you are in fact working in "YZ", then your primary plane should be "X". That may have something to do with it.

Third, if all else fails, try setting NX to output your toolpaths as "Linear Only".

Good luck,
J

NX 6.0.5.3

 

[davidtan20]

I am thinking that arc plane supposed be YZ and arc-output should be in yz coordinate, but I got xy, because my mom_pos_arc_plane = xy always no matter under M128 or spatial in PB_CMD_set_circular_plane, I thought maybe I need change mom_parameter for switch, I have tried mom_kin_arc_valid_plane but always XYZ...

 

[moldmaker2011]

Could be a simple TOOL DEF problem, check your TOOL Table. If your using a Tool Def call without giving a radius of the tool that will give you the same error

 

[davidtan20]

I have taken carefully a look at the coordinate of the first circular motion
as following:
X Y Z
L 0.1 0.375 -1.7625 (start point)
CC 0.1 0.375 -1.7625 (arc center )
C 0.1 0.3125 -0.950 (end point )

but If force output X Y Z then got following

X Y Z
L 0.1 0.375 -1.7625
CC 0.1 0.375 -1.700
C 0.1 0.3125 -1.700

the first one is not right, second one is moving on YZ plane and right. the question is this circle move has to be X Y for the CC & C ? how about X Y Z ? I am going to try it.

 

[davidtan20]

I have tried that it did not work for CC C circular move in X Y Z, and no detailed message for that.

people suggest me that forget M128. I don't want to do that, must be someone out there knows how to fix that, first of all thank you here.

1) call tool Z, here "Z" is for vertical CNC from my understanding
2) Under M128 all the coordinates are totally different from CYCL 19 and Spatial, that would be very dangerous if I delete M128 to run the NC program.

 

[davidtan20]

After tryout on our CNC, I found out that if you got circular motion involved under M128, you can only work on XY YZ XZ major planes, and the coordinates gotta be XY YZ XZ in C and CC accordingly, L is ok with X Y Z because it moves from point to point anyway. Becareful, I had DR+ and DR- ( arc direction )problem.

thank all and case is closed.