FIR filter (#FILTER)

Release Note

release_note

The availability of this function depends on the configuration and on the version scope.

In order to achieve a high surface finish in free-form surface machining, any excitation of machine oscillations must be avoided as far as possible.

FIR axis filters (Finite Impulse Response filters) provide the user with the option of smoothing the axis setpoints for the drives to minimise excitations in the machine.

The precondition for using a FIR filter using the #FILTER command is a configured filter type (P-AXIS-00586) of the corresponding axis.

Notice

notice

This function is an additional option requiring a license.

Syntax:

#FILTER [ON | OFF] [ORDER=.. ORDER_TIME=.. SHARE=.. AX_DEV=.. FCUT=.. ACC_FACT=.. QUALITY=.. ]

ON

Enable FIR filter.

OFF

Disable FIR filter.

ORDER=..

Specify filter order

ORDER_TIME=..

Specify filter order over time in [µs]

SHARE=..

Define the degree of effectiveness (analogous to P-AXIS-00590) of the filter in [%]
value range 0 – 100
default value = 100

AX_DEV=..

Specify the tolerance for tolerance monitoring in [mm, inch *].
Default value = 0 (no tolerance monitoring).
*with active P-CHAN-00439

FCUT=..

Specify the cut-off frequency (analogous to (P-AXIS-00585) of the filter in [Hz]
default value = 30

ACC_FACT=..

Increase the path velocity at block transitions with FIR filter enabled.

The greater the value setting, the less the velocity is reduced at the block transition.

This requires a valid setting of P-AXIS-00013 (a_trans_weight) for the axes.

Value range = 1.0 – 10.0

Default value =: 1.0

QUALITY=..

Specify the filter quality of the filter core curve
value range: 0 < QUALITY <= 1
default value = 1.0

Parameter available as of V3.1.3075.04

Notice

notice

The #FILTER ON/OFF command enables or disables all the FIR filters of the axes in the channel.

It is possible to use FIR filters on all axes. It is also possible to use different filters for each axis by axis-specific configuration in the axis lists.

FIR filters can be globally enabled or disabled and reparameterised across all axes in the NC program during machining (see Programming example).

Notice

notice

Tolerance monitoring can only be configured and activated in the NC program.

Tolerance monitoring is programmed by the parameter AX_DEV. It ensures that every axis remains within the specified tolerance [mm, inch].

Tolerance monitoring always monitors all axes and therefore can only be controlled globally in the NC program.

Tolerance monitoring in only active if AX_DEF was specified with a corresponding tolerance.

For further information see [FCT-C37//Description]

This command replaces the previously available #FILTER ON [HSC] command.