Drilling Machining Operation

Used to create circular holes from selected point lists or circles.


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.
Custom Script

Custom GCode script used for drilling if DrillingMethod=CustomScript

Various macros can be used in this script which will be expanded by the post processor.

| - denotes a new line
$c - Clearance Plane
$d - Hole diameter
$f - plunge feedrate
$h - Z coordinate of each drill point [New! 0.9.8]
$n - tool number
$p - Dwell
$q - Peck distance
$r - Retract height [New! 0.9.8]
$s - Stock Surface
$t - tool diameter
$x - X coordinate of each drill point
$y - Y coordinate of each drill point
$z - Target depth

Cut Feedrate The feed rate to use when cutting.
Depth Increment
[New! 0.9.8]

The depth increment controls the pitch of the spiral toolpath if Drilling Method = Spiral Mill.

This is the depth of cut for each loop of the spiral.

Drill Lead Out
[New! 0.9.8]

For spiral drilling only.

If True, then move toward or away from the center of the hole before retracting.

Drilling Method

Method used to generate the drilling instruction. Options are:

Canned Cycle - Uses G81,G82 or G83
SpiralMill_CW - Clockwise spiral toolpath
SpiralMill_CCW - Counter clockwise spiral toolpath
CustomScript - Uses the CustomScript property script


The time to pause at the bottom of the drill cycle. The unit of time measurement depends on the machine interpreter configuration and may be seconds or milliseconds.

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.
Hole Diameter

Used for spiral mill drilling and is the diameter of the hole required. If this is set to Auto, then the sizes of the selected shapes are used to calculate the hole diameter.

Lead Out Length
[New! 0.9.8]

For spiral drilling only. The distance to move in the lead out direction if DrillLeadOut=True.
If length is positive, move toward the hole center.
If length is negative, move away from the center.

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.

Peck Distance

The incremental depth to drill before a retract. If 0, then doesn't peck drill.

Plunge Feedrate The feed rate to use when plunging.
Primitive IDs List of drawing objects from which this machine operation is defined.
Retract Height
[New! 0.9.8]

For peck canned cycles, retract to this value after each peck.

Roughing / Finishing

This property is currently used only by the Lathe machining operation.

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.
Spiral Flat Base

For spiral drilling only. If True, a full circle is added to the spiral base, to ensure a flat hole bottom.

False will avoid the full circle cut, which may be useful for thread milling.

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.


A general purpose, multi-line text field that can be used to store notes or parameter data.

Target Depth

The Z coordinate of the final machining depth.

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) 2018 HexRay Ltd