[malirami]

I need help. I'm trying to mill a thread on my cnc mill with a FANUC 11M MODEL A Control and I have this alarm :
PS 186 ILLEGAL PLANE SELECT . Do I have to change the way that I'm programing?The subprogram is:G91 G02 I0.500 Z-0.125 F10.0

[Superman]

Fanuc and Okuma are similar

We have to state the I and J on a line doing full arcs

Suggest placing J0. on your line in the subs

I am also assumming you are in the G17 (XY) plane

[malirami]

Thanks , I'm going to try that and Yes I,m using G17 I should have to change that?.

[broby]

If you do not program I or J the controller will assume that the value for them will be 0 (zero), i.e. no need to program I0.500 J0 as J0 is assumed.
I would suggest that your problem is that you may not have the helical move option on your control, thus explaining the reason for the Plane error.
Even if you do not have the helical move option, you should still be able to program arc moves on the XZ or YZ planes using the G17 G18 G19 plane selection commands.

[malirami]

I think so , because I have programed on other machines with different controls and never had a problem.On this one I tried with G18 , G19 and I made the program with GIBBS CAM too but I get the same alarm.

[Superman]

a quick check,
program an arc using X,Y I, J
prove that it runs
now add a Z to the block

We have one machine that interpolates only in 2 axis, ( cannot ramp on arcs )

[malirami]

I tried something like that , but let me see again.thank you superman.

[chopkins]

Try programming 1/4 circles.
Takasaya mills will only spiral 90 deg or less.
This should work.

[malirami]

ok, let me try thta too.

[malirami]

Thanks

[jimmytightpants]

on the mill I run if we want to cut an arc while moving in the Z we have G2.1/G3.1 instead of G2 and G3. see if your machine has something like that.

[malirami]

OK.

[malirami]

Well , when I program:
G02 X0.500 Y0.0 I0.500 J0.0 is no problem, but when I put a Z , I get the
PS186 ILLEGAL PLANE SELECT ALARM. Even if I use G18 or G19 on or before the block.
I tried to program by quarters of circle and is the same.
If I program like this:
G18
G91 G02 I0.500 J0.0 Z-0.125F10.0
M99
I get this alarm:
PS 191 OVER TOLERANCE OF RADIUS
with G19 is the same.

[broby]

I would suggest that you find the data card in the back of the machine (usually) and see if there is any mention of Helical move option or not.
It is definitely looking like your problem is the fact that you do not have the Helical move option.
Next step would be to speak to your machine tool agent and see if you can purchase the option. You then need to see if the cost of the option is worth it for the amount of use you would make of it.
Regards
Brian.

[Superman]

a quick check,
program an arc using X,Y I, J
prove that it runs
now add a Z to the block

Yep,
my little prove-out shows that you can do an arc in any plane,
but as soon as you make the end point different to the start point
you get alarms --

Even if I use G18 or G19 on or before the block.

-NOTE- changing the G17 to G18/G19 when you have defined I and J will bring up a programming alarm, if you want to change plane--- you have to program the arc for that plane ie G18 ( I,K) G19 (J,K)--
so
G18
G91 G02 I0.500 J0.0 Z-0.125F10.0
will never work anyway

You only have 2-axis arc interpolation available
the only work around available to you is to program point to point ( no 3D arcs )( CAD outputs )
or by Z level machining

[malirami]

Thanks for your help , I,m going to call the technician and see what can we do. I need to make 4 pcs. with 6 holes 2 IN. npt on a 16 in. diam. and I, don't think is going to be funny do it by hand.

[Superman]

What programming software is available to you ?
Do you have a basic system for example ?

Do a program, drill the holes out to 1 3/4", copy that program and replace the drill cycle with a subroutine call-up at each of the hole positions, the subroutine would be a bore interpolated around X0 Y0 at different Z levels( then change the X and Y values to incremental for doing at the hole positions ) ( advanced users would program at X0Y0 then translate this bore to the hole centres or very similar ).

ie

O1001
G1 Z-.15 F50.
G91
G41 X1. D1 F10.
G2 I-1. J0.
G1 X-1. 
G90 Z-.3
G91 G41 X1. D1 F10.
G2 I-1. J0.
G1 X-1. 
G90 and so on
.
.
G90 G0 Z.5
M99

or use U / V if possible

O1001
G90 G1 Z-.15 F50.
G41 U1. D1 F10.
G2 I-1. J0.
G1 U-1. 
Z-.3 F50.
G41 U1. D1 F10.
G2 I-1. J0.
G1 U-1. 
. and so on
.
.
G90 G0 Z.5
M99