Fundamentals Of Path Functions; Programming Tool Movements For Machining - HEIDENHAIN TNC 620 User Manual

5
5.2

Fundamentals of path functions

Programming tool movements for machining

You create an NC program by programming the path functions for
the individual contour elements in sequence. You do this by entering
the coordinates of the end points of the contour elements given in
the production drawing. The control calculates the actual path of
the tool from these coordinates, and from the tool data and radius
compensation.
The control moves all machine axes programmed in the NC block of
a path function simultaneously.
Movement parallel to the machine axes
If the NC block contains one coordinate, the control moves the tool
parallel to the programmed machine axis.
Depending on the individual machine, the machining program is
executed by movement of either the tool or the machine table on
which the workpiece is clamped. Path contours are programmed as
if the tool were moving.
Example
50 L X+100
Block number
50
Path function straight line
L
Coordinate of the end point
X+100
The tool retains the Y and Z coordinates and moves to the position
X=100.
Movement in the main planes
If the NC block contains two coordinates, the control moves the tool
in the programmed plane.
Example
L X+70 Y+50
The tool retains the Z coordinate and moves on the XY plane to the
position X=70, Y=50.
140
Programming contours | Fundamentals of path functions
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022