5 Axis Help

Hi all, I am having some problems getting a 5axis toolpath to run on our 200 IVS, this is the first time that I have programmed in 5 axis and its just a single pass swarf machining operation following a constantly varying curve that also changes angle.

Here is the start of the unedited NC code from powermill:

(O2)
N10 ( Date : 23.02.10 16:02:40 )
N15 ( Programmed by : powermill )
N20 ( DP Version : 1490 )
N25 ( Option File : Mazak-Integrex-200Y-IV-Matrix-5ax-Inv-Time )
N30 ( Output Workplane : Output_1 )
N35 G53 G17 G98
N40 G90 G80 G21
N45 G98
N50 G28 U0.0
N55 G28 V0.0 W0.0
N60 M200
N65 T12T0 M6
N70 G97 S5093 M203
N75 M201
N80 G52.5
N85 G53.5
N90 ( Toolpath : 4 )
N95 M148
N100 G69.5
N105 M211
N110 G00 B12.195 C-90.
N115 G53.5
N120 G01 X-44.768 Y6.52 Z24.25 F3000.
N125 Z-31.34
N130 X-46.838 Z-36.129
N135 X-46.88 Z-36.227 F88.
N140 X-46.786 Y6.639 Z-36.235 F876.
N145 X-46.754 Y6.771
N150 X-46.792 Y6.902 Z-36.227
N155 X-46.89 Y7.02 Z-36.212
N160 G93 X-48.24 Y7.209 Z-36.079 B12.691 C-91.516 F911.404

And just for reference this is a sample code sent to me from Mazak UK that I have ran on our machine to make sure all parameters etc work:

O10580(G43.4 TEST)
G109L1

(PARAMETERS)

(O 3 SET TO 5)
(F161 BIT 1 TO 1)
(G54 DIA X NEGATIVE VALUE)
(TOOL LENGTH IN ISO PAGE POSITIVE VALUE)
(MAZ TOOL DATA CAN BE LEFT)
( X VALUES ARE RADIAL)

(F93 BIT 3 TO 1)
(F94 BIT 7 TO 0)

G17

T32M06

G53.5

G52.5 (ISO)

G54 (OFFSET)

G122.1 (RADIUS)


M200

M212

C180.

M250

B90.

M250



G43.4 H32 X40. Y0. Z50. C180. B90. (CALL )

G01 B0. F100. (F100. DEGREES / MIN DUE TO B AXIS)

G00 Y-70.

G01 X41. Y70. Z49. B1. C179. F100. ( F100. LINEAR MM/MIN )

G49

G28 V0.

G28 U0.


M30

...............

Ok I have copied over the relevant parts from the sample program to my NC code, but I am getting a "971" Tooltip point control error.

Any ideas?

Dan

I think you need the G43.4 to do 5 axis moves.

I have copied over the info from the g43.4 sample to my NC code, but that gives me an alarm.

Is it necessary to use G43.4 to do the following moves?

N160 G93 X-48.24 Y7.209 Z-36.079 B12.691 C-91.516 F911.404
N165 X-49.066 Y7.337 Z-35.996 B12.996 C-92.355 F1510.131
N170 X-50.252 Y7.454 Z-35.887 B13.441 C-93.578 F1113.301
N175 X-50.854 Y7.665 Z-35.822 B13.657 C-93.926 F1947.643
N180 X-51.504 Y7.823 Z-35.755 B13.902 C-94.386 F1932.218
N185 X-52.548 Y7.99 Z-35.649 B14.317 C-95.205 F1278.356
N190 X-53.582 Y8.189 Z-35.54 B14.737 C-95.907 F1291.329
N195 X-54.266 Y8.336 Z-35.466 B15.021 C-96.313 F1959.029
N200 X-54.946 Y8.49 Z-35.39 B15.308 C-96.68 F1977.343
N205 X-55.624 Y8.651 Z-35.314 B15.6 C-97.012 F1997.707
ete etc
.....

pic of required movement

[imgs= ][/imgs]


Dan

It is in Mazak's sample you listed above (G43.4 H32 X40. Y0. Z50. C180. B90. (CALL )
). G43.4 is how the machine keeps track of the tool tip when B is moving.

Yes, I have put that into my NC code, but for some reason that gives a 971 alarm, but the sample runs fine.

Dan

Did you put the G122.1 in also?

No, in my post I have set it to output X as dia.

Dan

G43.4 is not available in diameter mode !
edit your blocs by change all X in X0.5*
put a G122.1, you don't have choice !

Ahh, Ok,

Thats a simple mod to the post and i'll keep that one just for G43.3 work.

Will let you know how it goes.

Dan

Ok, its all working, turns out that my Powermill post was inverting the axis to some degree, and also after putting in the g122.1 everything works fine.
So even tho' the customer has put the job on hold....I now have a fully working 5 axis post now :)

Dan