Klartext Portal – The Information Site for HEIDENHAIN Controls

When a program interruption occurs, the immediate need is to retract the tool reliably. If you then wish to continue machining, you acknowledge an NC stop with the “manual traverse” soft key. In this way you make sure that the program continues to be referenced and that in the control, for example, the current condition of cycles remains saved. You then simply withdraw the tool using the axis direction key for the tool axis.

An example: If an interruption has taken place during tapping, then simply retract the tool with the press of a button, reliably and completely without problems, because the TNC suitably interpolates the motion of the spindle.

Machining continues: You then bring the tool back to the position before program interruption with the “approach position” soft key.

If the program run does not continue after an interruption, confirm the NC stop with the “Internal stop” soft key. You can then change the operating mode and retract for example in MANUAL MODE—but without the convenient support of the control. Automatic re-approach is then at first no longer possible.


In tilted systems, manual tool motions such as retracting are often real challenges. These are no problem, though, with the TNC. With the “3D-ROT” soft key, select whether you wish to retract

  • in the tilted coordinate system,
  • in the untilted coordinate system,
  • or only in the tool axis direction.

Modify the retraction direction at any time as well. Approach is also flexible with the TNC: With active 3D-ROT function simply select the appropriate axis sequence during the approach run, and change between manual and automatic traverse according to needs. Thus, in tilted systems, the TNC enables users to be in full control of all situations during approach and retraction.

Supported retraction from a thread

Using the “mid-program startup” function (block scan) enables users to reliably start up in mid-program, for example following an internal stop. Select the mid-program startup function, and input the block number where the TNC should continue the machining run. The control then simulates the program run until the start-up position, loads all requisite process data and checks whether the correct tool is in the spindle. Pre-positioning is started with the “approach position” soft key. If needed, the TNC inserts the required tool.Always use the mid-program startup as the situation requires:

Interrupt the approach routine at any time and modify the approach sequence of the axes to adapt the approach direction. This functions both in tilted and untilted condition, and can also be combined with manual approach motions, which is handy when the work space is tight, especially with tilted machining. Take note of the following tip before you start: Make sure the start position is approached from the right direction. For this purpose the control must have implemented the position and status before the entered block. Unnecessary tool changes are avoided in the mid-program startup, by the way, when you enter the subsequent block number at which actual machining should begin instead of the number of a TOOL CALL.

NC mid-program start-up with block scan.

Recurring positioning and processing steps are frequently saved in subprograms, and this enables machining programs to be designed more concisely as well as reducing programming effort. With the example of thread tapping, identical positions are repeatedly approached for centering, core hole drilling and thread cutting. The control applies the first call of a subprogram when in the block scan you specify a block number located in a subprogram.

In the tapping example, the TNC would start at the specified position with the centering tool. If however the tap is to be used, then the block number with suitable subprogram call would firstly be specified in the block scan. Proceed in steps when you want to start a subprogram:Enter the block number that calls the sub program in the input form for the block scan and confirm with NC START. Then enter the block number for the machining position into the subprogram via the input form and confirm with NC START. This multi-level strategy is suited both for mid-program start-ups in subprograms as well as for specific start-ups in called machining programs. It can also be expanded to any number of steps.

Automatically or manually specifying the axis sequence for positioning