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.
| Angle | The angle from horizontal of linear and spiral toolpaths
Warning! This property is not yet implimented.
|
| 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. |
| CollisionDetection | [NEW!] Makes sure adjacent toolpaths do not overlap.
Multiple Toolpaths are unioned together. |
| CustomMOPFooter | A multi line gcode script that will be inserted into the final gcode post before the machine operation.
See available macros in CustomMopHeader |
| CustomMOPHeader | A 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)
|
| CutFeedrate | The feed rate to use when cutting. |
| CutOrdering | Controls whether to cut to depth first or all cuts on this level first. |
| DepthIncrement | Depth increment of each machining pass. |
| DepthRelativeTo | Controls what the TargetDepth coordinates are relative to.
Warning! Any setting other than Absolute may give unpredictable results.
|
| Enabled | If Enabled is true, then display the toolpaths associated with this machine op and include in gcode output. |
| FinalDepthIncrement | The depth increment of the final machining pass. |
| GCodeOrigin | Defines 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.
|
| GCodeOriginOffSet | This offset is applied to the point determined in the GCodeOrigin to determine the gcode's machine 0,0 origin. |
| InsideOutside | Controls 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. |
| LeadInMove | |
| MaxCrossoverDistance | Maximum 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. |
| MillingDirection | Controls the direction the cutter moves around the toolpath.
Conventional or Climb milling supported. |
| Name | Each 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. |
| OptimisationMode | If 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. |
| PlungeFeedrate | The feed rate to use when plunging. |
| PocketingStyle | Defines 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
|
| PrimitiveIds | List of drawing objects from which this machine operation is defined. |
| RoughingClearance | This 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. |
| SpindleDirection | The direction of rotation of the spindle. |
| SpindleSpeed | The speed in RPM of the spinfle |
| StepOver | The cut is increased by this amount each step, expressed as a % of the cutter width. |
| StockSurface | Starting 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. |
| TargetDepth | End depth of the machining operation. |
| ToolDiameter | This is the diameter of the current tool in drawing units. |
| ToolNumber | The 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. |
| Transform | Used to transform the toolpath.
Warning! The property is experimental and may give unpredictable results. |
| VelocityMode | Instructs 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.
|
| WorkPlane | Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY, XZ and YZ |