Programming instructions

NC Programming 17VRS Motion Blocks
4-51
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
4.7 Coordinate Transformation
Coordinate transformation is available for:
•
Face machining, and
•
lateral cylinder surface machining
Lateral cylinder surface machining
Face machining
Fig. 4-51: Lateral cylinder surface and face machining
The commands G30 (de-selecting coordinate transformation), G31 (face
coordinate transformation), and G32 (lateral cylinder surface coordinate
transformation) form the G code group „transformation functions“ (no. 17).
Selection of Face Machining ‘G31’
The function G31 „select face machining“ is used to switch the CNC to a
fictive Cartesian coordinate system. The defined fictive linear axis are
used in the interpolation instead of the assigned real main axes. The path
feedrate with the transformation function must be specific, as with milling,
as a relative speed between the tool and the workpiece using the F-value.
The programmed path feedrate is reduced in such a way that the maxi-
mum rpm of the rotary axis is not exceeded. This is especially true with
movement near the center of rotation.
G31
•
The CNC supports the transformation function for the XY plane (G17).
The real axes involved in the transformation must have the axis
meaning X and C.
•
The real Y axis (if present) becomes an auxiliary axis which has the
meaning V. When the transformation is deactivated, the NC reestab-
lishes the original status.
•
The zero offsets are canceled (G53) when coordinate transformation
is selected (G31); tool path compensation and tool length correction
are deactivated (G40, G47). The CNC switches to radius programming
(G15).
•
The X axis must be in the positive area when the change to coordinate
transformation occurs.
•
After the changeover to coordinate transformation, the zero offsets for
the fictive axes become active, depending on which ones are set. The
zero offsets of the real main axes assigned to the fictive axes are not
in effect.
•
After the change to coordinate transformation, it is possible to program
directly using absolute (G90) or incremental (G91) dimensional input.
•
It is possible to open a new program during coordinate transformation
by using NC-block search; however, coordinate transformation (G31)
must be set with the basic settings for this function (G54, G48, etc.) in
MDI before starting the program.
•
The fictive axes cannot be passed on to other processes (FAX, GAX).
Syntax
Boundary conditions