HEIDENHAIN MANUALplus 620 351
4.29 Other G Functions
Read interpolation information G904
G904 transfers all the current interpolation information on the current
slide to the variable memory.
Feed rate override 100% G908
G908 sets the feed override for traverse paths (G0, G1, G2, G3, G12,
G13) block by block to 100%.
Program G908 and the traverse path in the same NC block.
Interpreter stop G909
The MANUALplus pre-interprets the NC blocks. If variables are
assigned shortly before the evaluation, “old values” would be
processed. G909 stops the pre-interpretation.. The NC blocks are
processed up to G909. After G909 the subsequent NC blocks are
processed.
Apart from G909, the NC block should only contain synchronous
functions. (Some G functions generate an interpreter stop.)
Spindle override 100% G919
G919 is used to deactivate/activate the spindle speed override.
Deactivate zero-point shifts G920
G920 deactivates the workpiece zero point and zero-point shifts.
Traverse paths and position values are referenced to the distance
tool tip – machine zero point.
Interpolation information syntax
Syntax: #an(axis,channel)
n = number of the information
axis = name of the axis
channel = slide number
Interpolation information
#a0(Z,1) Zero-point shift of the Z axis of slide $1
#a1(Z,1) Actual position of the Z axis of slide $1
#a2(Z,1) Nominal position of the Z axis of slide $1
#a3(Z,1) Lag error of the Z axis of slide $1
#a4(Z,1) Distance to go in the Z axis of slide $1
#a5(Z,1) Logical axis number of the Z axis of slide $1
Parameters
Q Spindle number (default: 0)
H Type of limit (default: 0)
0: Activate spindle speed override
1: Spindle override at 100%—modal
2: Spindle override at 100%—for the current NC block
To Next Page
Loading...
Need help?
General
