Machining radius by Z-axis in polar interpolation mode

[Vectrum]

Hi,

Can anyone help me with programming radius in polar interpolation.

We got millturn machine Doosan Lynx 220 without Y axis ( only X, Z, C)

Is it possible to run it simultaneously by 3 coordinates and make a radius by Z coordinate ?

I have to do part with 2 parralel face pockets what comes deep inside with radiuses, it looks like U - pockets.

Trying to work with the next code, but I've got alarm - selected incorrect plane ((

GO X44. Z10.
G112
G01 X40. C16. Z0. F0.5
G02 C0. Z-10. R5. (there is alarm)
G03 C-16. Z0. R5.
G01 X40. C-16. Z0.
G113

Thanks for your answers in advance

 

[Nerdlinger]

Im having trouble envisioning what you are trying to do, but maybe check your use of G17/18/19…whichever one is active tells the machine which plane the programmed arc is to lie on. This is typically G18 (X/Z) on a lathe. Good luck!

 

[EKrol]

A 220LM is not a millturn :O haha. You cannot add Z values to G02/G03 on a non y axis lathe. At least on our lathes that don't work. If you want to do that you have to convert it to C-axis an Z-axis. You can put G01 Z-10 C720 F1000. in there or something like this.

 

[Vectrum]

A 220LM is not a millturn :O haha. You cannot add Z values to G02/G03 on a non y axis lathe. At least on our lathes that don't work. If you want to do that you have to convert it to C-axis an Z-axis. You can put G01 Z-10 C720 F1000. in there or something like this.

I'm newbie in English language as recently moved from Ukraine to the UK, sorry for that.
And yes, You right, LM220 is not millturn as it hasn't Y axis.

Regarding to your reply ... it's possible in my machine to add Z value with X and C, but with G01 only, there is a problem.
G112
G01 X40. C16. Z-10. F500 (works)
G02 X40. C-16. Z-20. R10. F0.5 (doesn't work)

Anyway thanks

 

[EKrol]

I'm newbie in English language as recently moved from Ukraine to the UK, sorry for that.
And yes, You right, LM220 is not millturn as it hasn't Y axis.

Regarding to your reply ... it's possible in my machine to add Z value with X and C, but with G01 only, there is a problem.
G112
G01 X40. C16. Z-10. F500 (works)
G02 X40. C-16. Z-20. R10. F0.5 (doesn't work)

Anyway thanks

Typ "Millturn" into google search. You will see what it actually is You have to turn off G112 and use G01 to do Z-axis and C-axis movement. You cannot do C and Z axis movement at the same time with your lathe with g02 g03 in G112 mode. If you want to do it you have to change the values to Z and C values in G01 mode.

 

[sinha]

Post the drawing to understand what exactly is desired to be done.

 

[sinha]

Im having trouble envisioning what you are trying to do, but maybe check your use of G17/18/19…whichever one is active tells the machine which plane the programmed arc is to lie on. This is typically G18 (X/Z) on a lathe. Good luck!

Plane selection does not matter in polar interpolation. Polar interpolation uses the plane defined for it, through parameters 5460 (linear axis) and 5461 (rotary axis). Usually, it is front face where one axis is X axis and the other axis is the virtual C axis.
The issue is whether helical interpolation is possible on this plane (X/Z/C moving simultaneously). There is no information about it in the Operators Manual. Therefore, it may not be possible.
The manual just says circular interpolation, not helical interpolation:

 

[sinha]

G02 C0. Z-10. R5. (there is alarm)

There will be.
You cannot have Z in circular interpolation, in polar mode.

It is not clear what exactly you want to do, but it seems that cylindrical interpolation is what you need.

 

[Tom]

To do that in G112 mode I believe you need the helical interpolation option from FANUC, this option is normally activated on machines with a Y axis