Defining counters with FUNCTION COUNT

Application

The FUNCTION COUNT function allows you to control a simple counter from within the NC program. For example, this function allows you to count the number of manufactured workpieces.

Description of function

The count is retained even after a restart of the control.

The control only takes the FUNCTION COUNT function into account in the Program Run operating mode.

The control shows the current counter value and the defined target number on the PGM tab of the Status workspace.

PGM tab

Input

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

  • Change the following contents as needed:
  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions, e.g. with M91
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 FUNCTION COUNT TARGET5

; Set the target value of the counter to 5

The NC function includes the following syntax elements:

Syntax element

Meaning

FUNCTION COUNT

Syntax initiator for the counter

INC, RESET, ADD, SET, TARGET or REPEAT

Define counting function

Counting functions

Counting functions

The FUNCTION COUNT function provides the following possibilities:

Syntax

Function

INC

Increase count by 1

RESET

Reset counter

ADD

Increment the counter by the desired value

Input: 0...9999

SET

Set the counter to the desired value

Input: 0...9999

TARGET

Set the nominal count (target value) to the desired value

Input: 0...9999

REPEAT

Repeat the NC program from the defined label if the target value has not yet been reached.

Fixed or variable number or name

Notes

 
Notice
Caution: Data may be lost!
Only one counter can be managed by the control. If you execute an NC program that resets the counter, any counter progress of another NC program will be deleted.
  1. Please check prior to machining whether a counter is active.
  • The machine manufacturer uses the optional machine parameter CfgNcCounter (no. 129100) to define whether you can edit the counter.
  • You can use Cycle 225 to engrave the current counter value into the workpiece.
  • Cycle 225 ENGRAVING

Example

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

  • Change the following contents as needed:
  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions, e.g. with M91
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 FUNCTION COUNT RESET

; Reset counter value

12 FUNCTION COUNT TARGET10

; Set target number of machining operations

13 LBL 11

; Jump label

* - ...

; Machining operation

21 FUNCTION COUNT INC

; Increase counter value

22 FUNCTION COUNT REPEAT LBL 11

; Repeat machining operation if the target number has not been reached

23 M30

24 END PGM