Site ExplorerSite Explorer
Close site explorer

TRACYL Surface Transformation

Programming TRACYL with G-Code

On a daily basis, programmers of turn-mill centers are given the task of producing milled elements such as pockets, surfaces, grooves, or similar features on a turned workpiece. Thanks to the excellent graphical support provided by the ShopTurn programming system and the easy handling of the milling cycles, even beginners succeed very quickly with the programming. But even with G-code, the creation of such elements is not rocket science, as the following example shows: To make a pocket with the dimensions of 50 × 80 × 5 mm on a cylinder diameter of 100 mm, a turn-mill center with a swiveling milling head is used.

The following steps need to be performed:

  1. The G54 zero point and the G19 surface milling level are switched on, and the axes are moved into a basic position.
    G54 G19
    G0 X800 Y0 Z800 B1=0

  2. The tool is called up and engaged at 90° with the Cycle800.

  3. The master spindle is changed over to the milling spindle, with the speed and turning direction provided and prepositioned.
    G95 S4500 M3
    G0 X120 Z-50

  4. The surface transformation is called up with the command TRACYL, with the value in parentheses being the circumference diameter on which the surface is calculated. The standard pocket cycle POCKET then follows. It defines the pocket as if it were on a flat surface. Note that the radius programming of the x-axis is automatically activated during the cycle.

  5. With TRAFOOF, the transformation is deselected, a changeover to the turning spindle as the master spindle occurs, and the axes are cleared.
    G0 X300 Z300

Siemens accepts no liability for the general validity or functional safety of the program example shown.