Drilling 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.

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

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.

For spiral drilling only.

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

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.

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.

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.

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.

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

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

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

The direction of rotation of the spindle.

CW | CCW | Off

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.

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.

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.