[jolulank]

Hello everyone,

I have this problem, when I program G02 or G03, well in this particula case is a G03 the movement is odd. Let me explain

G00 X14.0 Z.26
G1 Z.16 F.01
X10.1894
G03 X4.5239 Z.7336 I-.0009 K7.2767
G1X4.6653 Z.8043
G00 etc.

Well, at the start of the G03 the tool instead of continuing the move, starts a radius move that goes inside the part (making the radius) and at the end finishes ok but after making a big curve inside the part.

I have tried everything I can think of, but I believe that there is a parameter that is causing it. If it is a PC parameters then I have no way of finding out as I only have the NC parameters description.

The machine is a Leblond Makino, Baron 25 fanuc 10T

Any help will be aprecciated

jolulank

[fordav11]

in my simulator your tool movement looks strange but nothing like you describe.
your tool moves away from the chuck. is this external or internal tool?
where is your Z0? it should be set on the face and the Z's should be minus but all of your Z's are positive.
did you generate the program with software or by hand?
what are you actually trying to machine..... give your part dimensions etc or a simple sketch and I can give you some working code.

[jolulank]

Yes, the tool should move away from the chuck; I am machinning an impeller and decided that my zero in z should be the face of the plate rather than the edge of the suction area because the port between plates is a critical dimension, but the move is correct. In fact I am using the same program in a Mori Seiki SL-3 but one of the PCBs malfunctioned so I had to change to this machine, but the program is running perfect in the Mori Seiki.
I generated the program with mastercam.

I am trying to machine an impeller similiar to these ones

pump impeller products, buy pump impeller products from alibaba.com

Thanks


jolulank

in my simulator your tool movement looks strange but nothing like you describe.
your tool moves away from the chuck. is this external or internal tool?
where is your Z0? it should be set on the face and the Z's should be minus but all of your Z's are positive.
did you generate the program with software or by hand?
what are you actually trying to machine..... give your part dimensions etc or a simple sketch and I can give you some working code.

[fordav11]

ok I see now. so describe more this 'big curve' you mentioned above. with a sketch if possible.
usually when that kind of thing happens either the direction of circular interpolation is wrong, the radius center point is wrong, the sign of I or K is wrong or the end point is wrong or the start point is wrong. that means the G02/G03 line or the start position above it.
if it cuts the part correctly but keeps going then the end point is wrong. since it works on the other machine and runs fine in my simulator (it cuts a concave curve just fine) it's a strange one. maybe try using R instead of I & K.

[jolulank]

Here is a dxf file for that part.
The other thing is tahat I know the machine's previous owner could not program any kind of radius movement. That is why I think is a parameter related issue.

Like I said, this big curve is one of the side plates of the impeller. And ind the dxf file that is attached and I added some offset lines to make the toolpath of the roughing.

I will ckeck the begin and end points,

Thanks for your help

jolulank

ok I see now. so describe more this 'big curve' you mentioned above. with a sketch if possible.
usually when that kind of thing happens either the direction of circular interpolation is wrong, the radius center point is wrong, the sign of I or K is wrong or the end point is wrong or the start point is wrong. that means the G02/G03 line or the start position above it.
if it cuts the part correctly but keeps going then the end point is wrong. since it works on the other machine and runs fine in my simulator (it cuts a concave curve just fine) it's a strange one. maybe try using R instead of I & K.

[fordav11]

the program is ok as-is IMO. It simulates fine as my pics above show.
please explain the incorrect tool movement part below......

Well, at the start of the G03 the tool instead of continuing the move, starts a radius
move that goes inside the part (making the radius) and at the end finishes ok but after
making a big curve inside the part.

also please try something simple like a 90 degree radius and explain the actual
tool movement on the machine (this cuts a 2" 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]

I'll try it right away.

jolulank

the program is ok as-is IMO. It simulates fine as my pics above show.
please explain the incorrect tool movement part below......

also please try something simple like a 90 degree radius and explain the actual
tool movement on the machine (this cuts a 2" 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]

Once in position it does a CCW 270 degree arc instead of the 90 degree ccw move


thanks again for the help

jolulank

the program is ok as-is IMO. It simulates fine as my pics above show.
please explain the incorrect tool movement part below......

also please try something simple like a 90 degree radius and explain the actual
tool movement on the machine (this cuts a 2" 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
%

[G0G90]

Try a negitive R ... does it give you the 90 degrees?

[jolulank]

It does the same move with the negative R

the program is ok as-is IMO. It simulates fine as my pics above show.
please explain the incorrect tool movement part below......

also please try something simple like a 90 degree radius and explain the actual
tool movement on the machine (this cuts a 2" 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
%

[angelw]

Once in position it does a CCW 270 degree arc instead of the 90 degree ccw move


thanks again for the help

jolulank

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

Regards,

Bill

[fordav11]

try G3 X6.0 Z-1.0 I0 K-2.0

[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

[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