Newbie- My CNC doesn't read G02 X Y I J

[Bazz]

Hi all, first time posting here, please be kind

Here's my problem:
when I run a program with G02/G03 X Y R, everything is fine,
but if I use the I and J code machine goes in "Alarm 21 wrong plane....."
The machine is a Kira 40HB with Fanuc 21 control.
This programs run perfectly fine on a Makino.
Change the programs to R would take alot of time, so if I can find the way to get the machine to read the I and J code it would be great.
I think, but I'm not sure, one o more parameters need to be switched on to enable the control to read the I and J code.
Any help please will be very much appreciated.

Cheers

[Stu_M3]

Looking at a pic of your machine it appears the spindle is in the Y axis, I am unfamiliar with this type of machine but maybe you are working in the XZ plane(G18) and therefor the plane needs to be specified at the start, do you have to programme zx moves instead of xy ?

Regards Stu.

[Kiwi]

These are the letters for the different planes:
G17 ( X & Y plane) use I & J
G18 ( X & Z plane) use I & K
G19 ( Y & Z plane) use J & K

[Bazz]

Guys,
Thank you all for your posts.

Yesterday when I came across the problem I didn't have time to look at it carefully.

I tried a few things today and found that actually the problem is different.
The machine read without problems I and J codes in G02/G03 cycles.

The problem is it doesn't aloud a Z movement in G02/G03 mode. This even if I use the R code. And that's what my programs do.

the alarm is "021 ILLEGAL PLANE AXIS COMMANDED"

Yes, it is a 3 axis horizontal machine with index table Stu.
And it has a X Y and Z movement in the G2 command
here is part of the prog:

X119.829Y-30.36
Z1.
G1Z0.F800
Y-26.64Z-.314F2200.
G2X112.014Y-26.568Z-.994I-3.829J8.64
G1Y-30.432Z-1.32
G2X119.829Y-30.36Z-2.I3.986J-8.568
G1Y-26.64Z-2.314
G2X112.014Y-26.568Z-2.994I-3.829J8.64
G1Y-30.432Z-3.32
G2X119.829Y-30.36Z-4.I3.986J-8.568
G1Y-26.64Z-4.314
G2X114.195Y-27.276Z-4.8I-3.829J8.64
X112.014Y-26.568R9.45
G1Y-30.432

Those are proven programs of jobs that I run an a Makino machine, but now need to run on this Kira

I think the machine is capable to execute a Z movement in G02/G03 and it would save me lots of time avoiding to repost the progs.

Any idea/suggestion?

Ta.

[dcoupar]

Sounds like the "Helical Interpolation" option is not turned on.

[Al_The_Man]

See if you have 9930 bit #3 set to 1, if not you may have to 'purchase' it from Fanuc.
Al.

[Bazz]

THANK YOU VERY MUCH GUYS!!

It's everything sorted!