Engraving Machining Operation

Engraving machining operations 'follow' their selected shapes, including Z movements.


Clearance Plane

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.

Custom MOP Footer A multi-line gcode script that will be inserted into the gcode post after the current machining operation.
Custom MOP Header A multi-line gcode script that will be inserted into the gcode post before the current machining operation.
Cut Feedrate The feed rate to use when cutting.
Depth Increment
[New! 0.9.8]
Depth increment of each machining pass. Determines the number of passes to reach the final target depth.
Enabled 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.
Final Depth Increment The depth increment of the final machining pass.
Max Crossover Distance

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.


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.

Optimisation Mode

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.

Plunge Feedrate The feed rate to use when plunging.
Primitive IDs List of drawing objects from which this machine operation is defined.
Roughing / Finishing

This property is currently used only by the Lathe and 3D Profile machining operations.

Roughing Clearance

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.

Spindle Direction

The direction of rotation of the spindle.

CW | CCW | Off

Spindle Range The pulley number or dial setting of the spindle for the target speed.
Spindle Speed The speed in RPM of the spindle.
Start Point

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.

Stock Surface

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

[New! 0.9.8]

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

[New! 0.9.8]

A general purpose, multiline text field that can be used to store notes or parameters from plugins.

Target Depth

The Z coordinate of the final machining depth.

For engraving operations, the Z coordinate of the source drawing object point will also be added to the toolpath so that the engraving toolpath can 'follow' the shape's Z contour.
Tool Diameter

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.

Tool Number

The ToolNumber is used to identify the current tool.

If ToolNumber changes between successive machine ops a toolchange instruction is created in gcode. ToolNumber=0 is a special case which will not issue a toolchange.

The tool number is also used to look up tool information in the current tool library. The tool library is specified in the containing Part, or if this is not present in the Machining folder level. If no tool library is defined the Default-(units) tool library is assumed.

Tool Profile

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.

Warning! This property is experimental and may give unpredictable results.
Velocity Mode

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.

Work Plane Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY | XZ | YZ
Copyright (c) 2017 HexRay Ltd