[mcluka]

Hello,

My CNC (FANUC ROBODRILL Alpha T21iD) doesn't read the G3 code, when it comes to it, it just stops and throws out an error (21 ILLEGAL PLANE AXIS COMMANDED). I have read that you could change the G3 with G17, G18 or G19, but I would like to know if anyone of you guys had the same problem and how did you fix it.

Regards,

L

[Heavy_Metal]

Hi,

Use G17 for XY-plane, G18 for XZ-plane or G19 for YZ-plane.

Regards,
Heavy-Metal.

[mcluka]

Thanks for your answer. As a matter of fact I did use the G17 code because I was working in the x-y plane, I am posting here a sample of my program so you will see that. I really have no clue why the G3 code doesn't work, might be a problem with the old software that is installed on the CNC controller...

%
O5000 (ZUNFINISH.TAP)
( MCV-OP ) (09-AUG-2013)
(SUBROUTINES: O3 .. O0)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T8
(TOOL -1- MILL DIA 15.0 R0. MM )
G90 G00 G40 G54
G43 H8 D8 G0 X94.047 Y11.857 Z50. S941 M3
M8

[Heavy_Metal]

Hi,

The D8 is for your radius-compensation.
Try an other number like D50 and use 7.5 for the compensation (0.5 x 15mm mill).
I don't see the lines with the G3 code, do you use a CAM program that generate the code so the D is not always necessary ?

Regards,
Heavy_Metal.

[mcluka]

yes, I'm using SolidCAM, I didn't post the whole program, just the first lines. I'm guessing that there is a problem with the integration of the g-code generated by SolidCAM and the my CNC controller which is around 13-14 years old. I already had many problems with transfering data to it and now with reading the data... Any ideas what could it be?

Thanks for your time!

L

[Heavy_Metal]

Hi,

Try to generate a simple code with the G3 function with R or I, J or K.
G0 X50. Y50.
G1 X70. F500
G3 X75. Y55. R5. F200
G1 Y70. F500
G3 X70. Y75. R5. F200

Look also for F (feed) in radius/corners that are not to fast.

Maybe your controller needs after the G2/G3 lines a G1 and SolidCAM doesn't generate that.
Are you sure there is no G3 in a XZ or YZ plane ?

You can also remove the radius compensation (D) and try the nc-code again.

Try the next code, it's milling a 40 mm round hole.
G0 G90 X50. Y50.
Z20.
G1 Z10. F1000
G91 G41 X20. D50 F500 (D50 = radius compensation)
G3 I-20.
G1 G90 G40 X50.
G0 G90 Z20.

Regards,
Heavy_Metal.

[dcoupar]

Why not post the section of the program where the problem is occurring? You know, so maybe those that are trying to help you can stop guessing? Would 10 blocks either side of the problem area be too much to ask?

[mcluka]

Attachment 195720 Here is a picture of the item I'm trying to make. Here I am posting the program for the outside shape. With this program I would remove the material to get the outside octagon like shape.

Here is a part of my program generated by SolidCAM with the FANUC postprocessor which is included in SolidCAM.

%
O5000 (VCJ.TAP)
( MCV-OP ) (11-AUG-2013)
(SUBROUTINES: O3 .. O0)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T1
(TOOL -1- MILL DIA 15.0 R0. MM )
G90 G00 G40 G54
G43 H1 D31 G0 X113.157 Y32.504 Z50. S1132 M3
M8
(------------------------------)
(IROUGH-OUTSIDE - SPIRAL-POCKET)
(------------------------------)
X113.157 Y32.504 Z10.
Z2.
G1 Z-24.92 F6000
G3 X112.5 Y31.074 Z-25. R2.056 F451
G2 X112.312 Y29.246 R14.23 F534
X112.15 Y28.434 R14.23
G3 X111.983 Y27.364 R10.08 F465
X111.559 Y18.269 R105.436 F437
G1 X111.527 Y13.699 F465
Y10.048
X111.521 Y9.131
X111.52 Y4.559
X111.496 Y3.698
G2 X110.186 Y-0.024 R7.124 F534
X104.072 Y-4.69 R12.017
X95.905 Y-6.195 R34.417 F522
X79.647 Y-6.502 R295.868 F425
G3 X79.433 Y-6.51 R2.871 F264
G1 X79.03 Y-6.54
G3 X78.778 Y-6.57 R2.871 F534
X78.287 Y-6.696 R2.871
G2 X77.721 Y-6.883 R14.23
X74.084 Y-7.5 R14.23
G3 X72.748 Y-8.062 Z-24.92 R2.056
X72.601 Y-8.236 R1.028 F6000
G1 X72.549 Y-8.313


@dcoupar

As I have said before, as soon as CNC reaches a G3 code it stops and throws out an error: 21 ILLEGAL PLANE AXIS COMMANDED, from there on I can't do anything. I have searched for solutions for this error and came across: Fanuc Alarm: 21 ILLEGAL PLANE AXIS COMMANDED - Helman CNC

As you can see in my program, the G17 code for the X-Y plane is turned on, so I really have no clue what to do... Today or tomorrow I will try the programs that Heavy_Metal has written down (Thanks mate!).

Regards,

L

[Heavy_Metal]

Hi L.

Remove the Z-25. in the G3 line and look whats happening.

(------------------------------)
X113.157 Y32.504 Z10.
Z2.
G1 Z-24.92 F6000
G3 X112.5 Y31.074 Z-25. R2.056 F451
---
G3 X72.748 Y-8.062 Z-24.92 R2.056

Maybe there are more lines you have to check.


Regards,
Heavy_Metal.

[samu]

You effectively call an helical move cause there is a Z movement in the same time you turn an arc. Helical interpolation is an option an alarm out if this option is not turned on.

[integymachine]

Your feedrate requires a decimal. And no feedrate at g1 line.

Sent from my MOTWX435KT using Xparent BlueTapatalk 2

[mcluka]

Well this is what SolidCAM generates, I can't really effect on that, the only thing I can do is to change it in notepad, but thats a loooot of work...

[Heavy_Metal]

Hi L,

Is there a Lead In / Lead Out function in the program (SolidCAM) that moves in Z, or maybe auto rounding/corners.
Is your drawing ok, and the curves/path in SolidCAM.
As you can see there are Z-values in G2/G3 lines.
G3 X112.5 Y31.074 Z-25. R2.056 F451


There is a same radius, R2.056 from Z-24.92 to Z-25. and back to Z-24.92 so I think there is a Lead In and Lead Out function.
G1 Z-24.92 F6000
G3 X112.5 Y31.074 Z-25. R2.056 F451
---
---
X74.084 Y-7.5 R14.23
G3 X72.748 Y-8.062 Z-24.92 R2.056

Check all of these things.

Regards,
Heavy_Metal.

[mcluka]

Heavy_Metal and others, thanks for your time and help, we have fixed our problem, how we did it is here: http://www.cnczone.com/forums/solidc...e_g3_code.html

Thanks again!

Regards,

L