HEIDENHAIN TNC 640, User Manual, Page: 642 / 948

Multiple-Axis Machining | Three-dimensional tool compensation (option 9)
13
642
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
Function
If you are executing a program with surface normal vectors and
assigned a compensation value table to the active tool in the
tool table (TOOL.T) in the DR2TABLE column, the control uses
the values from the compensation value table instead of the
compensation value DR2 from TOOL.T.
In doing so, the control takes the compensation value from the
compensation value table defined for the current contact point
of the tool with workpiece into account. If the contact point is
between two compensation points, the control interpolates the
compensation value linearly between the two closest angles.
Angle value Compensation value
40° 0.03 mm (measured)
50° -0.02 mm (measured)
45° (contact point) +0.005 mm (interpolated)
Operating and programming notes:
If the control cannot interpolate a compensation
value, it displays an error message.
M107
(suppress error message for positive
compensation values) is not required, even if positive
compensation values are determined.
The control uses either DR2 from TOOL.T or
a compensation value from the compensation
value table. If required, you can define additional
offsets, such as a surface oversize, via DR2 in the
TOOL CALL
block.
NC program
The software option
3D-ToolComp
(option 92) only functions with
NC programs containing surface normal vectors.
Pay attention when creating the CAM program how you measure
the tools:
NC program output at the south pole of the sphere requires
tools measured on the tool tip
NC program output at the center of the sphere requires tools
measured on the tool center