Profile Machining Operation

The clearance plane (offset from the work plane).

The clearance plane should be clear of the stock and any holding devices to allow free movement to any location.

Makes sure adjacent toolpaths do not overlap. Multiple Toolpaths are unioned together.

Set CornerOvercut to True to add an extra machining move, which will cut into inside corners that would not ordinarily be cut. This will result in some stock overcutting but is useful in cases where machined parts will be fitted together such as slot joints or inlays.

A multi-line gcode script that will be inserted into the gcode post after the current machining operation.

A multi-line gcode script that will be inserted into the gcode post before the current machining operation.

The feed rate to use when cutting.

Controls whether to cut to depth first or all cuts on this level first.

The total width of the cut. If this width is greater than the tool diameter, multiple parallel cuts are used.

Depth increment of each machining pass. Determines the number of passes to reach the final target depth.

True: The toolpaths associated with this machining operation are displayed and included in the gcode output
False: The operation will be ignored and no gcode or tool paths will be produced for this operation.

The depth increment of the final machining pass.

Defines holding tabs (bridges) to prevent cut parts moving while cutting.

See the holding tab reference for more information.

Controls whether to cut Inside or Outside the selected shapes.
For open shapes there is not inside or outside, so the point order controls which side of the line to cut.

Defines the type of lead in move to use.

Lead Move Type: None | Spiral | Tangent
Spiral Angle: Used by spiral and tangents to control ramp angle.
Tangent Radius : The radius of the tangent lead in
Lead Move Feedrate : The feedrate to use for the lead move. If 0, Cut Feedrate is used.

Refer to the lead move section for more information.

Defines the type of lead out move to use.

Refer to the lead move section for more information.

Maximum distance as a fraction (0-1) of the tool diameter to cut in horizontal transitions.

If the distance to the next toolpath exceeds MaxCrossoverDistance, a retract, rapid and plunge to the next position, via the clearance plane, is inserted.

Controls the direction the cutter moves around the toolpath.

Conventional | Climb | Mixed

Each machine operation can be given a meaningful name or description.
This is output in the gcode as a comment and is useful for keeping track of the function of each machining operation.

An option that controls how the toolpaths are ordered in gcode output.

New (0.9.8) - A new, improved optimiser currently in testing.
Legacy (0.9.7) - Toolpaths are ordered using same logic as version 0.9.7.
None - Toolpaths are not optimised and are written in the order they were generated.

The feed rate to use when plunging.

List of drawing objects from which this machine operation is defined.

Currently only supported by 3D Profile and Lathe machining operations.

This is the amount of stock to leave after the final cut.

Remaining stock is typically removed later in a finishing pass.

Negative values can be used to oversize cuts.

A composite property that enables the creation of pseudo 3D objects from 2D shapes by creating radii and slopes.

See the side profiles reference for more information.

The direction of rotation of the spindle.

CW | CCW | Off

The pulley number or dial setting of the spindle for the target speed.

The speed in RPM of the spindle.

Used to select a point, near to where the first toolpath should begin machining.
If a start point is defined, a small circle will be displayed at this point when the machining operation is selected. The start point circle can be moved by clicking and dragging.

The cut is increased by this amount each step, expressed as a fraction (0-1) of the cutter diameter.

The feed rate to use for crossover moves.

This is the Z offset of the stock surface at which to start machining.

Select a CAM Style for this machining operation. All default parameters will be inherited from this style.

The Z coordinate of the final machining depth.

This is the diameter of the current tool in drawing units.

If the tool diameter is 0, the diameter from the tool information stored in the tool library for the given tool number will be used.

The shape of the cutter

If the tool profile is Unspecified, the profile from the tool information stored in the tool library for the given tool number will be used.

EndMill | BullNose | BallNose | Vcutter | Drill | Lathe

Used to transform the toolpath.

Instructs the gcode interpreter whether or to use look ahead smoothing.

Constant Velocity - (G64) Smoother but less accurate.
Exact Stop - (G61) All control points are hit but movement may be slower and jerky.
Default - Uses the global VelocityMode value under machining options.

Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY | XZ | YZ