Commanding and execution

Homing is commanded either for “Homing ” mode or by the NC command G74 for specific channels. This command can be executed either in a manual block or in an NC program.

When referencing, the axis adopts the reference position P-AXIS-00152 (pos_refpkt) from the axis parameter list and stops.

NC program

Homing is started either:

• implicitly in homing mode with the default homing program rfp.nc or
• explicitly with any NC program that started in ‘Automatic’ mode or with a manual block which is executed in MDI mode.

Homing sequence of axes

The NC command G74 specifies the axes to be referenced and the sequence in which the axes are to execute homing. A

• sequential and a
• parallel command of the axes are possible.

The values programmed with the axis names define the homing sequence. For axes with the same value, homing is triggered simultaneously (see also [PROG]).

Programing Example

Sequential commanding

In the example below, axes Z, X, Y, A and B are commanded sequentially, i.e. Z is referenced before X starts homing, etc.

…

N10 G74 Z1 X2 Y3 A4 B5

…

This mode may be required, for example, to move the Z tool axis out of a collision zone with the workpiece or other axes. The other axes are then referenced.

Programing Example

Parallel commanding

In the example below, homing is executed in parallel (simultaneously) for the axes X, Y A and B.

…

N10 G74 X1 Y1 A1 B1

…

This mode is ideal due to the shorter time required at low homing speeds and the large motion range of the axis.

Another reason may be kinematic axis couplings which do not permit sequential homing.

Programing Example

NC program for referencing

In the example below, the Z axis is first referenced and moved to safety height. In the next NC block, the axes X and Y are then commanded in parallel and afterwards the axes A and B are also commanded in parallel. Finally, spindle S is referenced.

%RPF.NC

N10 G74 Z1

(optional: move Z to safety height)

N15 G01 G90 Z200 F500

N20 G74 X1 Y1 A2 B2 S3

…

(optional: move axes to home position)

N30 G01 X0 Y20 Z0 A90 F1000

N40 SPOS0 S500

...

N40 M30

After homing is completed, the axes can be positioned by a motion command to any position within the software limit switch. It is also possible to execute any initialisation here.

Drive-controlled referencing

Drive-controlled referencing describes homing which is executed independently by the drive. The NC controller commands the drive to reference its axis and at the end of homing it receive confirmation from the drive whether reference was executed successfully.

Homing is only parameterised in the drive.

The CNC support drive-controlled referencing by drives with SERCOS interface.

Notice

Except for P-AXIS-00014 all homing parameters in the axis parameter list only apply to NC-controlled referencing.

NC-controlled referencing

With NC-controlled referencing the entire homing sequence is determined by the NC controller. Homing can be parameterised for each axis using the homing parameters in the axis parameter list. Depending on the homing strategy selected, the reference cam signal may have to be provided on the HLI.

Supported drive types

NC-controlled referencing is supported for the following drive types:

• Drive simulation (by digital filters)
• Profidrive
• Terminal (+/-10V drives with incremental encoders, transparent access via field buses)
• Lightbus
• Real-time Ethernet

Notice

At present, NC-controlled referencing is only supported for drives with SERCOS interface without zero pulse search.

Drive simulation

The NC controller supports the “Simulation” drive type, i.e. every axis can be simulated, for example if there is no physical drive (±10V, stepper motor, etc.) present at the time of machine commissioning or if the controller is to be tested completely without physical drives.

Homing can also be selected for this drive type. Referencing these axes is simulated and this can be set in the axis parameter list by corresponding parameters.

Gantry coupling