Sorting

Zigzag

When the Zigzag option is chosen, the machining direction changes from cut to cut. The tool performs the machining of a cut in the specified direction, then moves to the next cut and machines it in the opposite direction.

One Way

When the One Way option is chosen, all cuts are machined in the same direction. The tool performs the machining of a cut in the specified direction, then moves to the start of the next cut and machines it in the same direction.

Spiral

With the Spiral option, SolidCAM generates a spiral tool path around the drive surface according to the chosen pattern.

The spiral pitch is defined by the Max. Step over parameter.

This cutting method is available for use with all the strategies except for the Projection strategy.

• The CW for closed cuts option enables you to perform the machining in the clockwise direction.

• The CCW for closed cuts option enables you to perform the machining in the counterclockwise direction.

• The Climb option enables you to perform climb milling, which is preferred when milling heat-treated alloys. Otherwise, chipping can result when milling hot rolled materials due to the hardened layer on the surface.

• The Conventional option enables you to perform the conventional milling, which is preferred for milling of castings or forgings with very rough surfaces.

When the direction is chosen as Climb or Conventional, the Advanced button is available for selection. Click Advanced to display the Advanced options for direction of machining dialog box.

Select the Contact point based cutting directions check box to select All contours or Single contour from the list.

All contours The entire tool path is in the set direction. This option is identical to the default one however, it generates the tool path depending on the contact point.
Single contour When this option is selected, each contour is considered as a single contour and is adjusted in the correct direction depending on the proportions of the set machining direction (climb/conventional).

To ensure the correct direction in every situation, the contact point between the tool and the surface is adjusted and checked with respect to the feed direction and the respective side of the tool.

All these factors are taken into consideration while generating the tool path.

With the Standard option, SolidCAM performs the machining from one side of the drive surface and continues to the other side.

With the From center away option, the machining starts from the center of the drive surface and continues outwards.

With the From outside to center option, the machining starts from the drive surface edges and continues inwards.

SolidCAM enables you to define the machining order for a Sim. 5-axis operation. The Machine by list enables you to choose the order of machining of certain areas; it defines whether the surface will be machined by Lanes or by Regions.

The generated tool path usually has a topology of multiple contours (lanes) on the drive surfaces. When the tool path is generated in many zones, it might be preferable to machine all the regions independently.

When the geometry is not completely closed, the Enforce closed contours option enables you to close the geometry and perform the machining of closed contours.

This option is available only with the CW and CCW options chosen for Direction of machining.

When the Standard option is chosen for the Cut order, the Flip step over parameter enables you to change the direction of the cuts.

In the image, the machining initially starts from the top of the model.

With the Flip step over option, the machining is reversed and starts from the edge.

This option is available only in Projection (User-defined and Offset) strategies.

This parameter is available only in the Projection (Radial) strategy.