fanuc 10T weird G02/G03 move

[jolulank]

It does look like figure # 2 the start point is the same but the finish Z is -1.0

Thanks a lot for all the help. I am still trying some alternative programming on my own but no luck yet.

jolulank

Is the 270 degree arc move as in attached Fig1 or Fig2?

Regards,

Bill

Attachment 149634Attachment 149635

[angelw]

It does look like figure # 2 the start point is the same but the finish Z is -1.0

Thanks a lot for all the help. I am still trying some alternative programming on my own but no luck yet.

jolulank

jolulank,
I'm not aware of any parameter that will affect circular motion in the way you have described.

Particularly given that the previous owner could not program any circular moves, there may be a problem with the actual control. I had a client some years back with a Takasawa lathe equipped with a 6TB control that could not process a circular path if the start point was not on the centre line of the arc. An arc could be programmed to finish at any angle, but if it didn't start at 3 or 12 o'clock (0 or 90 deg) then the control would raise an alarm. After I had convinced Fanuc that it was not a programming error, an eprom was replaced and that resolved the problem.

Your error is different to the above, but I would not disregard a control issue. Your program coordinates work out OK within the bounds of rounding to the least input increment, so I don't believe there is an issue with the program. Fanuc over here are very helpful, and that may be the case in your area. If you can't get a resolve, it may be beneficial to give them a call and discuss the issue.

Using R instead of I and K is a bit of a fudge in my opinion, and can result in an erroneous tool path without it being obvious if either the start or end point coordinates are wrong. In this case, and within reason, the control simply shifts the arc centre to make the circular tool path pass through the two given points. Conversely, when I and K are used, the control does a check based on the start coordinates and the arc centre described by I and K, to see if the given end point exists on the arc trajectory within a tolerance set in parameter. If it does not, an alarm is raised.

Regards,

Bill

[jolulank]

Thanks Bill,

I will look into that. It does sound reasonable what you said. I know some fanuc guys that can help me with this.

Thanks to everyone.

jolulank

jolulank,
I'm not aware of any parameter that will affect circular motion in the way you have described.

Particularly given that the previous owner could not program any circular moves, there may be a problem with the actual control. I had a client some years back with a Takasawa lathe equipped with a 6TB control that could not process a circular path if the start point was not on the centre line of the arc. An arc could be programmed to finish at any angle, but if it didn't start at 3 or 12 o'clock (0 or 90 deg) then the control would raise an alarm. After I had convinced Fanuc that it was not a programming error, an eprom was replaced and that resolved the problem.

Your error is different to the above, but I would not disregard a control issue. Your program coordinates work out OK within the bounds of rounding to the least input increment, so I don't believe there is an issue with the program. Fanuc over here are very helpful, and that may be the case in your area. If you can't get a resolve, it may be beneficial to give them a call and discuss the issue.

Using R instead of I and K is a bit of a fudge in my opinion, and can result in an erroneous tool path without it being obvious if either the start or end point coordinates are wrong. In this case, and within reason, the control simply shifts the arc centre to make the circular tool path pass through the two given points. Conversely, when I and K are used, the control does a check based on the start coordinates and the arc centre described by I and K, to see if the given end point exists on the arc trajectory within a tolerance set in parameter. If it does not, an alarm is raised.

Regards,

Bill

[gbowne1]

I don't know that much about lathe programming but I've never used a G02/G03.

[duivenhok]

maybe a silly question but should't you be useing G02 for making a clockwise radius??

%
G50 S250
G0 T0101
G97 S250 M3
G0 Z1.5
X2.0
G1 Z1.0 F.1
G3 X6.0 Z-1.0 R2.0
G0 X10.0 Z10.0
T0100 M5
M30
%

[jolulank]

It is a CCW radius, and I tried almos anything, finally, since it is a big radius I decided to turn it into .050 inch lines. You can not tell the difference.

It seems to be a problem with one of the eproms.

Thanks to all that help me with this problem

jolulank

maybe a silly question but should't you be useing G02 for making a clockwise radius??

%
G50 S250
G0 T0101
G97 S250 M3
G0 Z1.5
X2.0
G1 Z1.0 F.1
G3 X6.0 Z-1.0 R2.0
G0 X10.0 Z10.0
T0100 M5
M30
%

[stevo1]

maybe a silly question but should't you be useing G02 for making a clockwise radius??

Jolulank,
Don't dismiss the suggestion by duivenhok until you try it. Some time back we were having issues on a Mori with a 6t control that we converted a program from another Mori with a Yasnak control and the 6t needed to be using a G2 when every bit of logic said it needed a G3. The radius would dig inside the part working in the opposite direction. We changed the code, ran the part and shortly after never worked on the machine again so I never got the chance to look into why the code was backwards.

Stevo

[jolulank]

You are rigth Stevo, I should not dismiss the suggestion, it just was taking too much of my time with due times long overdue, but as soon as possible I will try duivenhok's suggestion. Thanks to both.

jolulank

Jolulank,
Don't dismiss the suggestion by duivenhok until you try it. Some time back we were having issues on a Mori with a 6t control that we converted a program from another Mori with a Yasnak control and the 6t needed to be using a G2 when every bit of logic said it needed a G3. The radius would dig inside the part working in the opposite direction. We changed the code, ran the part and shortly after never worked on the machine again so I never got the chance to look into why the code was backwards.

Stevo

[stevo1]

Keep us posted. I am curious to see what comes of this.

Stevo

[angelw]

You are rigth Stevo, I should not dismiss the suggestion, it just was taking too much of my time with due times long overdue, but as soon as possible I will try duivenhok's suggestion. Thanks to both.

jolulank

jolulank,
Irrespective of whether the G02/G03 are reversed on your machine, the example code should not have resulted in a 270 degree move. Whether G02 or G03 should be used can simply be determined by running the program in air and observing the direction, CCW, or CW, taken by the tool. If the required result was a convex radius, and the tool moved as shown in Fig2. of my earlier of Post, then G03 is correct.

We've seen your comments that you've tried everything to fix this issue, not that you've specifically used I and K instead of R format, as suggested by Ford. If you have used I and K, what was the result?

Regards,

Bill

%
G50 S250
G0 T0101
G97 S250 M3
G0 Z1.5
X2.0
G1 Z1.0 F.1
G3 X6.0 Z-1.0 I0.0 K-2.0
G0 X10.0 Z10.0
T0100 M5
M30
%

[CNCRim]

My suspect the reason you got a big circle before exit because there is not enough room for too compensate....... give a bigger number and try feed in both direction instead just Z.

[sinha_nsit]

Definition of CW and CCW in circular interpolation generally depends on whether it is front-type or rear-type lathe. One has to look at the arc from the positive side of the third axis, following right-hand coordinate system.