Bas Relief 3D Bas Relief Machining Operation

Bas Reliefs will soon be replaced with the new 3D Profile machining operation.

Bas Reliefs can be used to carve 3D objects from 3D mesh files. Currently 3DS and STL files are supported.

Bas Reliefs can generate front and back toolpaths as well as molds.


BackStockSurfaceThe Z depth that represents the back stock surface when using back face methods.

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)

CutDirectionDirection of long profile cut
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.

EnabledIf Enabled is true, then display the toolpaths associated with this machine op and include in gcode output.
FlipAxisThe axis around which you would flip the stock to machine the back face.
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.
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.
MultiplePassIncrementDepth increment of each machining pass.
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.
PrimitiveIdsList of drawing objects from which this machine operation is defined.
ProfileMethodThe method used to determine the toolpath from the 3D model.
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
StartCornerCorner to start profiling
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.
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.
ToolProfileThe shape of the cutter
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.

VolumeMaxA Point, used with VolumeMax to define a clipping volume.
VolumeMinA Point, used with VolumeMin to define a clipping volume.

If a VolumeMin and VolumeMax coordinate are both 0, the 3d profile will not be clipped.

WorkPlaneUsed to define the gcode workplane. Arc moves are defined within this plane.
Options are XY, XZ and YZ
XStepoverAmount to step x for each height test point.
YStepoverAmount to step x for each height test point.
Copyright (c) 2018 HexRay Ltd