cancel
Showing results for 
Search instead for 
Did you mean: 

Using Vectors on a FANUC 31i control and G02/G03 Moves?

Genius
Genius

Hello all,

 

I have a question regarding using Vectors and being able to output G02/G03 moves?

 

We have a Fanuc RoboDrill 5 axis Table-Table B/C and need to use vectors due to some associated alignment software also using G43.4/G43.5, the problem is that when we do a rotation and use vectors within a linear move all works well and as expected, only when trying to do a G02/G03 move does the machine then try and rotate in a way that is not good foe the heart!

I know that it is trying to read the I,J and K values as a vector move but not sure how other use vectors and machine normally/

I really don't want to just use G01 output as it causes other limitations and vastly increases program size?

 

Any thoughts or others findings on this would be greatly appreciated.

Regards

Dave
NX10.0.3MP13
NX11.0.1
Production
TC10
Vericut 7.3,7.4.1,8.0.2
5 REPLIES

Re: Using Vectors on a FANUC 31i control and G02/G03 Moves?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

You cannot use G2 G3 together with G43.4, this type motion for 5axis only. Use G68 G68.2 and for fixed tool axis you can use circular motion. Or - I don't understand you...

I open FANUC manuals - and found description for this error

PS5421 ILLEGAL COMMAND IN

G43.4/G43.5

Your case?

 

Re: Using Vectors on a FANUC 31i control and G02/G03 Moves?

Genius
Genius

Hi @Chigishev,

 

We don't see any error the machine just tries to rotate the "B" and "C" axis below in and extract of the code that will cause an issue

 

( OPERATION Smiley TongueLANAR_MILL_4)
( TOOL NAME :16MM_MILL)
( TOOL DIAMETER :16.000)
G91 G28 Z0.0
G91 G28 X0.0 Y0.0
G90 G53 G00 B0.0 C0.0
T7 M06
G90 G55
G65 P 0524 I1.0 (ACTIVATE ALIGNMENT)
B0.0 C0.0
G49.
G43.4 H07
G00 X57.852 Y7.981 Z10. B0.0 C0.0
G49.
G43.5 S12000 M03 M08
G94 G90 I0.0 J0.0 K1.
Z-9.
G01 Z-12. I0.0 J0.0 K1. F1500.
G03 X50.4 Y0.0 I.548 J-7.981
G02 I-50.4 J0.0

 

We get no alarms until the "B" axis hit a parameter limit, I was just wondering if others had come accross this problem?

Regards

Dave
NX10.0.3MP13
NX11.0.1
Production
TC10
Vericut 7.3,7.4.1,8.0.2

Re: Using Vectors on a FANUC 31i control and G02/G03 Moves?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

If I remember :

1. When you use G43.5 - you must output XYZIJK for each line. No modal.

2. When you use G43.5 - you cannot use G02\G03. But - I see in FANUC manual that G02\03 compatible for G43.5, may be - you must change some parameters.

 

 

Re: Using Vectors on a FANUC 31i control and G02/G03 Moves?

Genius
Genius

Hi @Chigishev,

 

The machine doesn't like outputting all XYZIJK on the same line for G02/G03 it gives anothr alarm as we were trying to Helix down and it errors on the line that has XYZIJK I think it is related having a maxium of 5 cooridinates?

 

Regards

Dave
NX10.0.3MP13
NX11.0.1
Production
TC10
Vericut 7.3,7.4.1,8.0.2

Re: Using Vectors on a FANUC 31i control and G02/G03 Moves?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
You no need to output G02 XYZIJK - it is wrong. You must output IJK for each G01 G0 lines while G43.5 is active.

I try to make some sample for you. You want to make helix motion, with some fixed tool axis vector. Right?

Your prog may be like here:

G43.5 G01 X..Y..Z..I..J..K.. H F
G01 X..Y..Z..I..J..K.. H F
G0 X..Y..Z..I..J..K.. H F
G49
G68.2XYZ....... params for G68.2, as you want orient tool
G0
G1
G2 XY (Z for helical) IJ

G69
G49



Learn online





Solution Information