Programming instructions

3-26
Motion Commands, Dimension Inputs NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
3.11 Axis Homing Cycle 'G74'
The preparatory function G74 axis homing cycle allows traversing to the
reference point along one or more axes in an NC-program or via MDI NC-
block entry.
G74 <[Axis Name][CoordinateValue=0]> <Feed>
Example G74 X0 Z0 F10000
G74 is non-modal. In the homing cycle, each programmed axis is moved
at the homing velocity that has been entered in the axis parameters.
•
G74 deactivates the tool path and tool length correction using G40,
sets the machine zero point (G53), switches to feed programming
(G94) and to absolute dimension input (G90).
•
The coordinate values of the programmed axes in a G74 NC-block
must be declared to be zero.
•
If a number of axes are programmed in a G74 NC-block, the axis
movement of the axes is not performed with interpolation.
•
A feedrate programmed in a G74 NC-block will also remain active for
other types of interpolation.
Note:
The reference dimensions and the homing cycle traversing
speed are set by the machine builder in the drive parameters.
3.12 Traverse to Positive Stop
The function Feed to Positive stop allows one or more axes to feed to a
mechanical stop without causing a drive error. Possible applications are:
to preload an axis slide at this stop position during machining, or to use
the axis position at the stop as a reference position for further machining.
Feed to Positive Stop 'G75'
The preparatory function G75 feed to positive stop causes the axes which
are programmed together with the preparation function in the NC NC-
block to traverse in the direction of the programmed coordinate value.
G75 <[Axis Name][Coordinate Value]> <Feed>
Example G75 X100 Z50 F500
G75 is active only for the NC-block in which it is located. The axes are
traversed in the direction of the programmed coordinate value using the
feed which is programmed in the G75 NC-block. If a mechanical resis-
tance—for example, a mechanical stop—is detected during this distance,
the torque which is defined by the axis parameter Cxx.044 Reduced
Torque at Positive Stop is limited based on a percentage of the peak cur-
rent. The command value is not increased further; the distance-to-go and
the torque preload are maintained.
Syntax
Notes on programming G74
Syntax