Fundamentals

Application

In the Program Run operating mode you produce workpieces by having the control execute NC programs either block-by-block or in full sequence.

You also execute pallet tables in this operating mode.

Related topics

 
Notice
Caution: Danger due to manipulated data!
If you execute NC programs directly from a network drive or a USB device, you have no control over whether the NC program has been changed or manipulated. In addition, the network speed can slow down the execution of the NC program. Undesirable machine movements or collisions may result.
  1. Copy the NC program and all called files to the TNC: drive
 
Notice
Danger of collision!
When you edit NC programs outside the Program workspace, you have no control over whether the control will identify the changes. Undesirable machine movements or collisions may result.
  1. Edit NC programs in the Program workspace only

Description of function

 
Tip

The following information also applies to pallet tables and job lists.

When you select a new NC program or when an NC program has been completely executed, the cursor is at the beginning of the program.

If you want to start machining at a different NC block, you first need to select the desired NC block by using the Block scan function.

Block scan for mid-program startup

By default, the control runs NC programs in Full Sequence mode after the NC Start key has been pressed. In this mode, the control runs an NC program continuously up to its end, or up to a manual or programmed interruption.

In Single Block mode you execute each NC block separately by pressing the NC Start key.

The control shows the status of the machining process with the Control-in-operation icon in the status overview.

Status overview on the TNC bar

The Program Run operating mode provides the following workspaces:

When opening a pallet table, the control displays the Job list workspace. You cannot modify this workspace.

The Job list workspace

Icons and buttons

The Program Run operating mode contains the following icons and buttons:

Icon or button

Meaning

Open File

With Open File you can open a file (for example, an NC program).

When you open a file, the control closes the file that was already open.

Execution cursor

The execution cursor shows which NC block is currently being executed or is marked for execution.

Single Block

If this toggle switch is active, then you run each NC block separately with the NC Start key.

If Single Block mode is selected, then the operating mode's icon in the control bar changes.

Q info

The control opens the Q parameter list window, where you can see and edit the current values and descriptions of the variables.

The Q parameter list window

Compensation tables

The control opens a selection menu with the following tables:

  • D
  • T-CS
  • WPL-CS

Compensation during program run

F LIMIT

Use this function to activate a feed-rate limit and define its value.

Feed rate limit F LIMIT

Automatic program start

Starts machining at a defined time automatically

Automatic program start

Program run options

When you select this button, the control opens the Program run options window with the following selection possibilities:

GOTO Cursor

The control marks the table row currently selected for execution.

This button is available when a pallet table is open.

The Job list workspace

AFC

Use this option to activate or deactivate Adaptive Feed Control (AFC (#45 / #2-31-1)).

The AFC toggle switch in the Program Run operating mode

AFC settings

The control opens a selection menu with the following selection possibilities for AFC (#45 / #2-31-1):

  • AFC.TAB for AFC basic settings
  • AFC.DEP settings file for teach-in cuts of the active NC program
  • AFC2.DEP log file of the active NC program
  • Stop Teach

The AFC settings button

Skip block

If the toggle switch is active, the control does not execute NC blocks dimmed with a / character.

Hiding NC blocks

If the toggle switch is active, then the control dims the NC blocks to be skipped.

Appearance of the NC program

Pause at M1

If the toggle switch is active, the control stops the execution at every NC block with M1.

Overview of miscellaneous functions

If the toggle switch is inactive, then the control dims the M1 syntax element.

Appearance of the NC program

ACC

If this toggle switch is active, the control activates Active Chatter Control (ACC (#145 / #2-30-1)).

Active Chatter Control (ACC) (#145 / #2-30-1)

Edit

If this toggle switch is active, then you can edit the pallet table.

This button is available if a pallet table is open.

The Job list workspace

GOTO block number

Mark an NC block to be run without considering any previous NC blocks

GOTO function

Manual traverse

While a program run is interrupted, you can move the axes manually.

If Manual traverse is active, the operating mode's icon in the control bar changes.

Manual traverse during an interruption

3D ROT

While a program run is interrupted, you can move the axes manually in the tilted working plane (#8 / #1-01-1).

Manual traverse during an interruption

Approach position

Return to contour after manual traverse of the machine axes during an interruption

Returning to the contour

Block scan

Use the Block scan function to start program run at any desired NC block.

The control takes the preceding parts of the NC program up to this NC block into account mathematically; for example, whether the spindle was switched on with M3.

Block scan for mid-program startup

Tool Retract

If the NC program is stopped during a thread cycle, you can retract the tool.

The Retract application

Open in the editor

The control opens the active NC program in the Editor operating mode and selects the currently selected NC block, even for called NC programs.

This button is available when an NC program is open.

The Editor operating mode

Tools

The control opens the Tool management application in the Tables operating mode.

Tool management

Internal stop

For example, if an NC program is interrupted due to an error or a stop, the control activates this button.

Use this button to abort program run.

Reset program

If you select Internal stop, the control activates this button.

The control places the cursor back to the beginning of the program and resets any modally active program information as well as the program run-time.

Feed rate limit F LIMIT

The F LIMIT button allows you to reduce the feed rate for all operating modes. The reduction applies to all rapid traverse and feed rate movements. The value you have entered remains active across power cycles.

The F LIMIT button is available in the MDI application and in Editor operating mode.

When you select the F LIMIT button in the function bar, the control will open the Feed rate F LIMIT window.

Use the +, -, *, /, (, and ) keys for calculations in the numerical input fields.

If a feed rate limit is active, the control highlights the F LIMIT button in color and displays the defined value. In the Positions and Status workspaces, the feed rate is displayed in orange.

Status displays

You deactivate the feed rate limit by entering a value of 0 in the Feed rate F LIMIT window.

Interrupting, stopping or canceling program run

There are several ways to stop a program run:

  • Interrupt program run (e.g., with the miscellaneous function M0)
  • Stop program run (e.g., with the NC Stop key)
  • Cancel program run (e.g., with the NC stop key and the Internal stop button)
  • Terminate program run (e.g., with the miscellaneous functions M2 or M30)

Upon major errors, the control automatically aborts program run (e.g., during a cycle call with stationary spindle).

Message menu on the information bar

If you run your NC program in Single Block mode or in the MDI application, the control will switch to the interrupted state after the execution of each NC block.

The control shows the current program run status with the Control-in-operation icon.

Status overview on the TNC bar

Below are some of the functions you can execute in an interrupted or canceled state:

  • Selecting an operating mode
  • Manual traverse of axes
  • Checking variables and changing these if necessary using the Q INFO function
  • Changing the setting for the optional programmed interruption with M1
  • Changing the setting for the programmed skipping of NC blocks with /
 
Notice
Danger of collision!
Certain manual interactions may lead to the control losing the modally effective program information (i.e., the contextual reference). Loss of this contextual reference may result in unexpected and undesirable movements. There is a risk of collision during the subsequent machining operation!
  1. Do not perform the following interactions:
    • Cursor movement to another NC block
    • The jump command GOTO to another NC block
    • Editing an NC block
    • Modifying the values of variables by using the Q parameter list window
    • Switching the operating modes
  2. Restore the contextual reference by repeating the required NC blocks

Programmed interruptions

You can set interruptions directly in the NC program. The control interrupts the program run in the NC block containing one of the following inputs:

  • Programmed stop STOP (with and without miscellaneous function)
  • Programmed stop M0
  • Conditional stop M1

Resuming program run

After stopping the program with the NC Stop key or a programmed interruption, you can resume program run by pressing the NC Start key.

After canceling the program run with an Internal stop, you must start the program run at the beginning of the NC program or use the Block scan function.

After an interruption of the program run within a subprogram or program section repeat, you need to use the Block scan function for mid-program startup.

Block scan for mid-program startup

Modally effective program information

The control saves the following data during a program interruption:

  • The last tool that was called
  • Current coordinate transformations (e.g., datum shift, rotation, mirroring)
  • The coordinates of the circle center that was last defined

The control uses the stored data for returning the tool to the contour (Approach position button).

Returning to the contour

 
Tip

The saved data remains active until it is reset (e.g., by selecting a program).

Notes

 
Notice
Danger of collision!
Program cancellation, manual intervention, forgotten resetting of NC functions or transformations can lead to the control performing unexpected or undesirable movements. This can lead to workpiece damage or collision.
  1. Rescind all programmed NC functions and transformations within the NC program
  2. Run a simulation before executing an NC program
  3. Check both the general as well as the additional status display for NC functions and transformations, such as an active basic rotation, before executing an NC program
  4. Carefully prove-out the NC program in Single Block mode
  • In the Program Run operating mode, the control marks active files with the status M, such as a selected NC program or tables. If you open such a file in another operating mode, the controls shows the status on the tab of the application bar.
  • When positioning an axis, the control checks whether the defined speed has been reached. The control does not check the speed in positioning blocks where FMAX is the feed rate.
  • You can adjust the feed rate and the spindle speed during program run with the potentiometers.
  • If you modify the workpiece preset during a program run interruption, you must re-select the NC block to resume.
  • Block scan for mid-program startup

  • HEIDENHAIN recommends switching the spindle on with M3 or M4 after every tool call. That way you avoid problems during program run, such as when restarting after an interruption.
  • The execution cursor is always displayed in the foreground. The execution cursor may cover or hide other icons.