G19 with I J K questions

[mgb1974]

Trying to test out a machine to figure out whats going on with it. Wont machine a radius around a half circle. Machine goes crazy.

When it gets to line N202 the machine says G02 error and when it gets to line N214 says G03 error

Do these lines of code look correct??

(ARC XZ I J K G02)
N198 G01 X0.0 Y-1.0 Z0.0 F6.5
N202 G19 G02 X0 Y1.0 I-1.0 J0.0
N206 G00 X0.0 Y0.0 M00

(ARC XZ I J K G03)
N210 G01 X0 Y-1.0 Z0.0 F6.5
N214 G19 G03 X0.0 Y1.0 I-1.0 J0.0
N218 G00 X0.0 Y0.0 M00

Thanks

[vwilmot]

Are you using a Right Angle Head? If so, which direction is it pointed, left or right? May be as simple as making your G2's a G3 and G3's a G2.

[tobyaxis]

Originally Posted by mgb1974 Trying to test out a machine to figure out whats going on with it. Wont machine a radius around a half circle. Machine goes crazy. When it gets to line N202 the machine says G02 error and when it gets to line N214 says G03 error Do these lines of code look correct?? (ARC XZ I J K G02) N198 G01 X0.0 Y-1.0 Z0.0 F6.5 N202 G19 G02 X0 Y1.0 I-1.0 J0.0 N206 G00 X0.0 Y0.0 M00 (ARC XZ I J K G03) N210 G01 X0 Y-1.0 Z0.0 F6.5 N214 G19 G03 X0.0 Y1.0 I-1.0 J0.0 N218 G00 X0.0 Y0.0 M00 Thanks

If I remember correctly (it has been a while) but G18 and G19 Plane Designations are for Cutter Compensation Direction Designation. In other words you do not need to call them if your not using any Cutter Comp.

Program it straight like this. (LEFT SIDE 90 DEGREE HEAD)

G90G0X1.Y-1
G1Z-1.F30.
X.5F15.
Y-.5
Z-.5
Y-1.5
Z-1.
Y-1.
X1.

BTW: I do not believe that the Axis Designations Change when using G18/G19 so that is why your machine is going nuts.

It is a CNC not a CAD program so the Axis Designations will be applied to the Type of head your using.

[JWK42]

This is from my Maho manual, which supports all 3 systems.

G17
Circle end point X and Y
Tool Axis Z
Circle center I and J
Pitch of helix if needed K

G18
Circle end point X and Z
Tool Axis Y
Circle center I and K
Pitch of helix if needed J

G19
Circle end point Y and Z
Tool Axis X
Circle center J and K
Pitch of helix if needed I

It appears that you are using the wrong end point words as well as circle center words with your G19 system.

Edit--

I just ran the program below on our Haas Simulator and it shows the axis movements on the DRO.
I switched to G19 for the one line and then back to G17.
On a Haas control the I-J-K is "The distance and + / - direction from the start of the arc to the center of rotation" In this case you would use J1. since you start at Y-1. and the center is Y0. and K0 since you start at Z0. and the center as Z0. The I word would be used only if you were doing a helix move in X axis. When I ran this line N203 using G02 started at Y-1. Z0. and went up to Y0. and Z1. and back down to Y1. Z0. Line N214 using G03 started at Y-1. Z0. and went down to Y0. and Z-1. and back up to Y1. Z0.



%
O01000 (HAAS VF-3YT VERTICAL)
N30 G17 G54 G90
N50 T1 M06
N60 G90 G00 X0. Y-1.
N80 G01 Z0.125 F50. M08
(ARC XZ I J K G02)
(Should be ARC YZ J K G02)
N198 G01 X0. Y-1. Z0. F10.
N202 G19 G02 Y1. Z0. J1. K0. F10.
N206 G17 G00 X0. Y0. M00
(ARC XZ I J K G03)
(Should be ARC YZ J K G03)
N210 G01 X0 Y-1. Z0. F6.5
N214 G19 G03 Y1. Z0. J1. K0. F10.
N218 G17 G00 X0. Y0. M00
N90 G53 G00 Z0. M09
N100 G53 G00 X0. Y0. A0.
N140 M30 (END OF MAIN PROGRAM)
%

[beege]

Some machines don't allow arcs in anything but G17 (XY plane) The old Cincinatti 850SX was one of them.

ALL machines require a plane change for arcs in different planes! Cutter comp is not a factor in this case, although if you have to use comp in other planes, the WHOLE contour has to be prefaced by a plane change, before turning comp on.

Also, in both comp and circle generation, the geometry has to be visualized from the +X, +Y, +Z quadrant. In G19, the G02 arc will look clockwise from the right side of a VMC, and look counter-clockwise from the left side.

I, J and K are all arc center designations, I relates always to X, J relates to Y, and K relates to Z. So... an arc in the YZ plane (G19) is going to have a Y component, a Z, a J and K center point, or you could cheat by using an R instead.

Hope this helps!

[mgb1974]

thanks guys for all the help. I think I have it figured out now just have to try it on the machine.

[tobyaxis]

Don't forget to post your results.

[mgb1974]

That fixed the problem with the G19 thanks guys again!!!