Drill Drilling Machining Operation

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

Properties

ClearancePlane

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.

CustomMOPFooterA multi line gcode script that will be inserted into the final gcode post before the machine operation.

See available macros in CustomMopHeader

CustomMOPHeaderA multi line gcode script that will be inserted into the final gcode post before the machine operation.


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

| - denotes a new line
$f - cut feedrate
$t - tool diameter
$n - tool number
$x - X coordinate of 1st toolpath point
$y - Y coordinate of 1st toolpath point
$z - Z coordinate of 1st toolpath point
$r - Clearance Plane
$s - Stock Surface
$q - Peck distance (drilling only)
$p - Dwell (drilling only)
$d - Hole diameter (drilling only)

CustomScriptCustom GCode script used for drilling
CutFeedrateThe feed rate to use when cutting.
DepthRelativeToControls what the TargetDepth coordinates are relative to.


Warning! Any setting other than Absolute may give unpredictable results.

DrillingMethodMethod used to generate the drilling instruction
DwellThe time to pause at the bottom of the drill cycle
EnabledIf Enabled is true, then display the toolpaths associated with this machine op and include in gcode output.
GCodeOriginDefines which drawing point will be at the machines 0,0 location.


Settings other than DrawingOrigin will use the select extremety point.
This point is calculated from all drawing objects used in all machine operations.

GCodeOriginOffSetThis offset is applied to the point determined in the GCodeOrigin to determine the gcode's machine 0,0 origin.
HoleDiameterThe diameter of the hole required.
MaxCrossoverDistanceMaximum distance as a % of the tooldiameter to be cut in horizontal transitions.
If distance to next toolpath exceeds this then a rapid to next position via the clearance plane is inserted.
NameEach machine operation can be given a meaningful name or description.
This is output in the gcode as a comment and is very useful for keeping track of the function
of each machining operation.
OptimisationModeIf OptimisationMode=Default, then toolpaths are ordered to minimise rapids between toolpaths.
If OptimisationMode=None, then toolpaths are not optimised and are written in the order they were generated.
PeckDistanceThe incremental depth to drill before a retract
PlungeFeedrateThe feed rate to use when plunging.
PrimitiveIdsList of drawing objects from which this machine operation is defined.
RoughingClearanceThis is the amount of stock to leave after the final cut.
Remaining stocl is typically removed later in a finishing pass.
Negative values can be used to oversize cuts.
SpindleDirectionThe direction of rotation of the spindle.
SpindleSpeedThe speed in RPM of the spinfle
StockSurfaceStarting depth of the machining operation offset from the workplane. This can be the string NaN
to tell the gcode generator to follow the geometry as in heightmaps.
TargetDepthEnd depth of the machining operation.

Warning! - TargetDepth for drilling is currently different to other machining operations in that the target depth is relative to the stock surface whereas in other machine operations, target depth is a final Z coordinate. This behaviour is under review and may change in later versions.

ToolDiameterThis is the diameter of the current tool in drawing units.
ToolNumberThe ToolNumber is used to identify the current tool.
If ToolNumber changes between successive machine ops a toolchange instruction is given.
ToolNumber=0 is specially case which will not issue a toolchange.
TransformUsed to transform the toolpath.

Warning! The property is experimental and may give unpredictable results.

VelocityModeInstructs the gcode interpretter whether or to use look ahead smoothing.


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

WorkPlaneUsed to define the gcode workplane. Arc moves are defined within this plane.
Options are XY, XZ and YZ
Copyright (c) 2017 HexRay Ltd