Pocket Pocket Machining Operation

Pockets are used to clear out stock within boundary shapes.

If selected shapes contain other shapes, CamBam will automatically detect these as 'Islands'. That is, the area around them will be cleared and the islands will remain prominent.


AngleThe angle from horizontal of linear and spiral toolpaths

Warning! This property is not yet implimented.


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.

CollisionDetection[NEW!] Makes sure adjacent toolpaths do not overlap.
Multiple Toolpaths are unioned together.
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)

CutFeedrateThe feed rate to use when cutting.
CutOrderingControls whether to cut to depth first or all cuts on this level first.
DepthIncrementDepth increment of each machining pass.
DepthRelativeToControls what the TargetDepth coordinates are relative to.

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

EnabledIf Enabled is true, then display the toolpaths associated with this machine op and include in gcode output.
FinalDepthIncrementThe depth increment of the final machining pass.
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.
InsideOutsideControls 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.
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.
MillingDirectionControls the direction the cutter moves around the toolpath.
Conventional or Climb milling supported.
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.
PlungeFeedrateThe feed rate to use when plunging.
PocketingStyleDefines the type of lead in move to use.

LeadInType : None | Spiral | Tangent
SpiralAngle : Used by spiral and tangents to control ramp angle.
TangentRadius : The radius of the tangent lead in

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
StepOverThe cut is increased by this amount each step, expressed as a % of the cutter width.
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.
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) 2018 HexRay Ltd