Ball Mill

[Tornos100]

I am new to running and programming a Citizen L20 swiss screw machine. I am going to be machining a handle made out of tit. After a long radius is turned using a G3 code, is it possible to go over the same radius at a shallower depth with a ball end mill? I need to put a shallow line at 90^ increments. The line actually starts out shallow and gets deeper in the center then gets shallower again. Can a G3 code be used for an endmill the same way it is used for a turning tool? Thanks for your help!!

[UK-Engineer]

"Can a G3 code be used for an endmill the same way it is used for a turning tool?"

Yes - All you have to do is change the plane selection before milling e.g

M5 G98
M58 S3=2000
T700
M18 C0
G50 W-0.59
G0 X* Z* Y* T*

G19 - Plane select for Y and Z

G3 Y* Z* R* F*
G1 Y*

G0 X* T0

G18 - Std Plane select for X and Z

G50 W0.59
M20 M60 G99

If you want to "wrap" milling tool round bar you'll need G12.1/G16 plane and any Y axis moves become C and values are radiall

E.g

M5 G98
M58 S3=2000
T700
M18 C0
G50 W-0.59
G0 X* Y* Z* T*
G1 X* F*
G12.1
G16 C*

G3 Z* C* R*
G1 Z*
G0 X*
G13.1
G18
G0 X* T0
G50 W0.59
M20 M60 G99


Good luck

[Tornos100]

UK-Engineer:
Thanks for your help. I am not making the part at this moment, just needed to know if it was possible. Thanks again!

[PixMan]

UK-Engineer,

Are you sure about needing to change the interpolating plane for this? It seems to me that the turning operation is already done in G18 X-Z mode. No? Since the L-series has live tools rotating 90º to the workpiece, as the gang tools are also oriented, the G19 Z-Y mode would be for use if using a t-slot type of cutter in the "side" of the work. This is a ball mill, presumably using the tip.

The only difference is that the machine stops the spindle, lights up the live tool spindle and moves (in most cases) in the "G98" mode instead of "G99". Maier CNC screw machines can use live tools in either mode.