HEIDENHAIN CNC Pilot 4290 - Manual (Page 179)

HEIDENHAIN CNC PILOT 4290 167
4.12 Special Functions
4.12.7 Load Monitoring
The load monitoring function checks the performance and work
values of the drives and compares them to limit values which have
been determined during a reference machining cycle.
The CNC PILOT considers two limit values:
■ If the first limit value is exceeded, the tool is marked as worn out
and the tool life monitoring inserts the replacement tool during the
next program run (see “
4.2.4 Tool Programming”).
■ Second limit value exceeded: The load monitor reports a broken
tool and stops the program run (feed stop).
Defining a monitoring zone G995
G995 defines the monitoring zone and the axes to be monitored.
■ G995 with parameter: Beginning of monitoring zone n
■ G995 without parameter: End of the monitoring zone (not
required, if another monitoring zone follows)
The zone number must be unambiguous in the NC program. A
maximum of 49 monitoring zones per slide are possible.
Parameters
H:
Zone number—range: 1 to 999
Q: Code for axes (drives to be monitored):
■ 1: X axis
■ 2: Y axis
■ 4: Z axis
■ 8: Spindle
■ 16: Spindle 1
■ 128: C axis 1
Add the codes if you want to monitor more than one drive.
(Example: Monitoring the Z axis and main spindle: Q=12.)
Type of load monitoring G996
With G996 you can temporarily switch off the load monitoring and
define the type of monitoring.
Parameters
Q:
Scope of monitoring—default: 0
■ Q=0: Monitoring not active (effective for the entire NC
program; even previously programmed G995 are rendered
ineffective)
■ Q=1: Rapid traverse movements not monitored
■ Q=2: Rapid traverse movements monitored.
H: Type of monitoring—default: 0
■ H=0: Torque and work monitoring
■ H=1: Torque monitoring
■ H=2: Work monitoring.
Example: Load monitoring
. . .
MACHINING
. . .
N.. G996 Q1 H1 [Torque monitoring—does
not monitor rapid traverse paths. ]
. . .
N.. G14 Q0
N.. G26 S4000
N.. T2
N.. G995 H1 Q9 [Monitors the spindle
and X axis]
N.. G96 S230 G95 F0.35 M4
N.. M108
N.. G0 X106 Z4
N.. G47 P3
N.. G820 NS.. [Monitors the feed paths
of the roughing cycle]
N.. G0 X54
N.. G0 Z4
N.. M109
N.. G995 [Ends the machining cycle]
. . .
The “code for axes“ is defined in bit
numbers for load monitoring (control
parameter 15).