Additional Zigzag slot

This ToolBox Cycles strategy enables you to machine wide slots. The tool path starts from the slot center and goes toward the walls. By default, the tool enters the material in a zigzag movement.

Geometry definition

The list of available geometries contains only suitable geometries.

Suitable geometries

• Geometry should contain only closed chains (without open edges).
• Ideal slot shape to be machined in this sub-operation consists of two arcs with the same radius and two parallel elements connecting the arcs. Those elements can be curves or lines. Arcs with different radiuses are also suitable.
• SolidCAM determines the center line of the slot.
• Geometry can contain several chains.
• Geometry direction is not significant.
• If you choose an open chain, the Close chain dialog box is displayed suggesting you to close the chain with a line.

Technological parameters

Rough

SolidCAM enables you to perform the slot machining in a number of cutting passes distributed along the tool axis.

Step down

The distance between two successive cutting levels is defined by the Step down parameter.

Zig-zag cuts

This section enables you to define the parameters of the zigzag cuts. The Ramping width parameter enables you to define the width of the zigzag cut. The default value of the parameter is the tool diameter multiplied by two. The Max ramping angle parameter enables you to define the angle between the inclined cuts and the machining plane. The default value is 5 degrees.

Parallel cuts

The Step over value enables you to define the distance between two parallel cutting passes. The default value is 0.25 of the tool diameter.

Offsets

This section enables you to define Wall and Floor offsets for this sub-operation. The Wall offset is applied to the walls of the slot; the specified offset is left unmachined during the current sub-operation. The Floor offset is applied to the floor of the slot; the specified offset is left unmachined during the current sub-operation. When the Floor offset value is specified, SolidCAM performs the machining by the Z-levels defined with the Step down parameter. The machining is performed until the Floor offset level.

Finish

The Wall finish option enables you to perform a final finishing pass cleaning the walls. You can specify the Step down value in a separate field.

The Floor finish option enables you to perform a final finishing cut cleaning the floor.

Compensation

If the Compensation check box is selected, the tool radius compensation options G4x of the CNC-controller are used in the GCode.

Pre-Drilling

This sub-operation can extract, store and use data from a previously applied Drilling operation to calculate approach points automatically.

Use Pre-Drilling Operations

Upon selecting the Use Pre-Drilling Operations check box, the definition windows are activated. When a Drill operation is chosen from the list, the associated X- and Y-coordinates appear in the Drill positions list. The drill diameter and positions data are used for the approach point calculations.

When Pre-Drilling data is defined, the tool performs a vertical entry into the material instead of in the default zigzag movement.

All rules regarding the Geometry definition are applicable. For the Technological parameters, Zig-zag cuts are ignored.

According to the Drill positions data, the tool approaches the slot and performs a vertical entry to the Step down depth. After the slot center is machined at the first cutting level and for each successive level, the tool returns to the approach point at the Step down depth. The machining of the slot center is completed at every cutting level with the width equal to the tool diameter; the Parallel cuts are then performed at each level (first to last) after returning to the approach point at the Step down depth.