HEIDENHAIN TNC 620 Programming Station, Руководство пользователя

Страница: 238 / 695

Programming contours
6.2 Fundamentals of path functions
6
238
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
6.2 Fundamentals of path functions
Programming tool movements for workpiece
machining
You create a machining 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 TNC calculates the
actual path of the tool from these coordinates, and from the tool
data and radius compensation.
The TNC moves all machine axes programmed in the NC block of a
path function simultaneously.
Movement parallel to the machine axes
The NC block contains only one coordinate. The TNC thus moves
the tool parallel to the programmed machine axis.
Depending on the individual machine tool, the part 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:
N50 G00 X+100*
N50
Block number
G00
Path function "straight line at rapid traverse"
X+100
Coordinate of the end point
The tool retains the Y and Z coordinates and moves to the position
X=100.
Movement in the main planes
The NC block contains two coordinates. The TNC thus moves the
tool on the programmed plane.
Example
N50 G00 X+70 Y+50*
The tool retains the Z coordinate and moves on the XY plane to the
position X=70, Y=50.