Fanuc 16i-m Helical Interpolation Problem

[Goran P.]

Hi,

I'm having trouble getting my machine to do the helical interpolation, I'm not sure if it is a programming error or the parameter is disabled to do so. This is the code i'm inputing into the machine:

T1
M06 ( 2" MITSUBISHI)
G00 G90 G54 X0. Y0. S700 M03
G43 H1 Z2. M08
Z.1
G01 Z0. F45.
G03 Y.4685 I0. J.2343
Y-.4685 Z-.025 I0. J-.4685 (This is where I get the alarm)
Y.4685 Z-.05 I0. J.4685
Y-.4685 Z-.075 I0. J-.4685
Y.4685 Z-.1 I0. J.4685
Y-.4685 Z-.125 I0. J-.4685
...


The alarm I am getting is; 021 Illegal Plane Axis Commanded

I'm desparate for some help, Thanks in advance...

Goran P.

[Sump Cleaner]

Goran,

Sounds like a parameter issue. For the 16i, set #9930 bit 3 to 1 to enable helical interpolation.

JK

[Goran P.]

Thanks for reply JK.

However i'm not parameter literate, this is what i have for 9930;

0 1 0 0 0 1 1 1

what should i change it to?

[Sump Cleaner]

Goran,

Change #9930 to:

0 1 0 0 1 1 1 1

It works like this;

______bit7__bit6__bit5__bit4__ bit3__ bit2__bit1__bit0
9930___0____1____0____0_____1_____1____1____1

JK

[Goran P.]

JK,

I changed the parameter and the helical interpolation works fine now. Thank you very much for your help.

Goran

[Sump Cleaner]

No Problem...

JK

[Mitsui Seiki]

Deleted

[CNCRim]

The program don't look right, the program is Y Z and the vector is I J........ It should be K J or vice versa.

[Mitsui Seiki]

Originally Posted by newtexas2006 The program don't look right, the program is Y Z and the vector is I J........ It should be K J or vice versa.

It does if you do a circular interpolation with changing Z depths.

[ChattaMan]

Newtexas2006.....
X0 is modal so there's no need for it in the prog. As he says...it works now.

[bsamc2000]

We just purchased a machine with this same controller. How do I tell if mine have scale and rotation?

[sinha_nsit]

Originally Posted by Goran P. G00 G90 G54 X0. Y0. S700 M03 G43 H1 Z2. M08 Z.1 G01 Z0. F45. G03 Y.4685 I0. J.2343

The program is OK.
The centre of the first arc, however, is not exactly at the mid-point. So, the tool will first go to Y0.4686, and then come back to Y0.4685. This is, of course, only a theoretical issue, with no practical significance. If, however, the "error" is too large (set by a parameter), an alarm condition will be generated.