HEIDENHAIN TNC 620 User Manual page 308

7
Programming notes
The FK free contour programming feature can only be
used for programming contour elements that lie in the
working plane.
The working plane for FK programming is defined
according to the following hierarchy:
1. Using the plane defined in an FPOL block
2. Using the working plane defined in the TOOL CALL
(e.g. TOOL CALL 1 TOOL CALLZ = X/Y plane)
3. The standard X/Y plane is active if none of these
applies
The display of the FK soft keys depends on the spindle
axis in the workpiece blank definition. If for example you
enter spindle axis Z in the workpiece blank definition,
the control only shows FK soft keys for the X/Y plane.
You must enter all available data for every contour
element. Even the data that does not change must
be entered in every block—otherwise it will not be
recognized.
Q parameters are permissible in all FK elements, except
in elements with relative references (e.g. RX or RAN), or
in elements that are referenced to other NC blocks.
If both FK blocks and conventional blocks are entered in
a program, the FK contour must be fully defined before
you can return to conventional programming.
The control needs a fixed point that it can use as the
basis for all calculations. Use the gray path function keys
to program a position that contains both coordinates of
the working plane immediately before programming the
FK contour. Do not enter any Q parameters in this block.
If the first block of an FK contour is an FCT or FLT block,
you must program at least two NC blocks with the gray
path function keys to fully define the direction of contour
approach.
Do not program an FK contour immediately after an LBL
command.
308
Programming Contours | Path contours – FK free contour programming (option 19)
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2017