GSK 980TDi, Руководство пользователя

Страница: 88 / 570

Official GSK Agents in South Africa
Tel: +27 11 626 2720, design@efamatic.com
GSK980TDi Turning CNC System User Manual
72
Ⅰ
Programming
X
：
distance of linear axis, unit: mm/inch;
C
：
distance of rotary axis, unit: mm/inch;
The linear axis can use the diameter programming and the rotary
axis uses only the radius;
The polar coordinates in the polar coordinate interpolation plane is prepared below:
X: length between current tool and the origin, its unit: mm/inch;
C ： angle unit of current rotary axis: deg;
G16 is the polar coordinates of current coordinates being complied,
and G15 is to cancel it. The Cartesian coordinate system is used
without G16. G16/G15 is valid in the only polar coordinate
interpolation.
The radius programming is applied to the linear axis and the rotary
axis below:
● Length compensation : the length compensation is not applied to the rotary axis, and the length
offset should be command before G12.1 mode, and cannot be changed in the polar coordinate
interpolation.
● Tool radius compensation: the tool nose direction is 0.
● Machine motion
：
the linear axis is vertical to the rotary axis.
● Circular interpolation in the interpolation plane: the address of the arc radius is determined by
the 1st axis(linear axis) in the interpolation
plane.
• When the linear axis is X or its parallel axis, I and J are used in Xp-Yp plane
• When the linear axis is Y or its parallel axis, J and K are used in Xp-Zp plane
• When the linear axis is Z or its parallel axis, K and I are used in Zp-Xp plane
The arc radius can also use R command.
● Command speed: tangential speed in the polar coordinate plane.
When the tool approaches the center of the workpiece, the speed component of C axis
exceeds its maximum cutting federate (set by No.27). F value is calculated by the followings:
L
：
the distance (mm) between the center of the tool and that of the workpiece
R
：
maximum cutting feedrate of C axis
（
deg/min
）
Conclusion
：
F
＜
L×R× π /180
（
mm/min
）
It is suggested that the workpiece should not be machined near the polar because the
feedate override must be changed in some occasion to avoid the overload of the rotary axis.
● Movement along the axis in the non polar coordinate interpolation plane in the polar
coordinate interpolation mode: The tool traverses normally along these axes and is not relevant
to the polar coordinate interpolation, the parameter specifies one
axis to execute the polar coordinate interpolation before
executing the polar coordinate interpolation, the axis which does
not specify the polar coordinate can moves along the normal
path in G00 or G01, but the axis which polar coordinate is not
specified is disabled (i.e. the block is ignored and the axis does
not move) in arc or ellipse command.
Specified position
Current position Angle
Radius