Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
51
In this section you will find descriptions of the commands, with which you can directly program dimensions taken from a
drawing. This has the advantage that no extensive calculations have to be made for NC programming.
The commands described in this section stand in most cases at the start of a NC program. The way, in which these
functions are combined, is not intended to be a patent remedy. For example, the choice of working plane may be made at
another point in the NC program. The real purpose of this and the following sections is to illustrate the conventional struct
of an NC program.
Overview of typical dimensions
The basis of most NC programs is a drawing with concrete dimensions.
When implementing in a NC program, it is helpful to take over exactly the dimensions of a workpiece drawing into the
machining program. These can be:
● Absolute dimension, G90 modally effective applies for all axes in the block, up to revocation by G91 in a following block.
● Absolute dimension, X=AC(value) only this value applies only for the stated axis and is not influenced by G90/G91. This
is possible for all axes and also for SPOS, SPOSA spindle positionings, and interpolation parameters I, J, K.
● Absolute dimension, X=DC(value) directly approaching the position by the shortest route, only this value applies only for
the stated rotary axis and is not influenced by G90/G91. This is also possible for SPOS, SPOSA spindle positionings.
● Absolute dimension, X=ACP(value) approaching the position in positive direction, only this value is set only for the rotary
axis, the range of which is set to 0... < 360 degrees in the machine data.
● Absolute dimension, X=ACN(value) approaching the position in negative direction, only this value is set only for the
rotary axis, the range of which is set to 0... < 360 degrees in the machine data.
● Incremental dimension, G91 modally effective applies for all axes in the block, until it is revoked by G90 in a following
block.
● Incremental dimension, X=IC(value) only this value applies exclusively for the stated axis and is not influenced by
G90/G91. This is possible for all axes and also for SPOS, SPOSA spindle positionings, and interpolation parameters I, J,
K.
● Inch dimension, G70 applies for all linear axes in the block, until revoked by G71 in a following block.
● Metric dimension, G71 applies for all linear axes in the block, until revoked by G70 in a following block.
● Inch dimension as G70, however, G700 applies also for feedrate and length-related setting data.
● Metric dimension as G71, however, G710 applies also for feedrate and length-related setting data.
● Diameter programming, DIAMON on
● Diameter programming, DIAMOF off
Diameter programming, DIAM90 for traversing blocks with G90. Radius programming for traversing blocks with G91.
Plane selection: G17 to G19
Functionality
To assign, for example,
tool radius and tool length compensations
, a plane with two axes is selected from the three axes X,
Y and Z. In this plane, you can activate a tool radius compensation.
For drill and cutter, the length compensation (length1) is assigned to the axis standing vertically on the selected plane. It is
also possible to use a 3-dimensional length compensation for special cases.
Another influence of plane selection is described with the appropriate functions (e.g. Section "Support for the contour
definition programming").
The individual planes are also used to define the
direction of rotation of the circle for the circular interpolation
CW or CCW.
In the plane in which the circle is traversed, the abscissa and the ordinate are designed and thus also the direction of
rotation of the circle. Circles can also be traversed in a plane other than that of the currently active G17 to G19 plane (For
more information, refer to Section "Circular interpolation (Page 72)".).
To Next Page
Loading...
Need help?
General
