Face Mill Zig, ZigZag

In this tutorial, we show how the Siemens NX Face Mill Zig, ZigZag operation can reduce unnecessary air cutting movements through alternating milling and enable more efficient programming of face milling operations.

Efficient machining of large planar surfaces is one of the classic challenges in NC programming. Especially when the entire surface is intended to be machined with a single toolpath, tool movements and non cutting motions play a critical role in the overall machining time. This is exactly where the Siemens NX Face Mill Zig, ZigZag operation provides valuable optimization potential.

The focus is on face milling surfaces with a tool diameter larger than the actual surface width. The goal is to machine the complete surface in a single pass while minimizing unnecessary air cutting movements.

With the conventional Floor Wall operation, this was previously only possible to a limited extent. Although the toolpath could be positioned centrally across the surface, the machining process always followed the same pattern: the tool approached from one side, machined the surface, retracted to the clearance plane, and then returned to the starting position for the next step over movement. This resulted in additional tool movements and unnecessary air cutting.

This is exactly where the Face Mill Zig, ZigZag operation provides a significant advantage. With the appropriate strategy settings, the tool can alternate the step over movement between both sides. This creates an alternating milling strategy in which both the forward and return movements are used productively for material removal.

The key settings are located within the operation under the strategy parameters. The pattern type is initially set to “Single Pass”, which is already familiar from the conventional Floor Wall face milling operation.

The setting “Cut Order Between Levels” becomes particularly important here. By default, this option is set to “Maintain”. In this case, the toolpath follows the familiar pattern with approach movement from one side and retraction to the clearance plane after each pass.

When the “Alternate Cut Direction” option is activated instead, the toolpath becomes significantly more efficient. The tool approaches from one side, machines the surface, performs the step over movement directly on the opposite side, and then returns in the reverse direction. This allows both cutting directions to be used as active machining passes.