Polyline Backplotting

CamBam can be used to view toolpaths contained within many gcode files.

GCode files can be opened using File->Open, or dragged onto the main drawing view.

The gcode file is associated with a special 'NCFile' machining operation that will appear in the machining tree view. This operation contains properties that can change the way the gcode is interpretted and displayed. If any options are changed, the toolpaths should then be regenerated.

CamBam currently only supports basic gcode and does not recognise more complex gcode syntax such as subroutines.

Another useful feature of backplotting is the ability to convert the gcode toolpaths to drawing objects. Right click the NCFile object under the machining tree and select 'Toolpath To Geometry' from the context menu.


ArcCenterModeGCode distance mode (absoulte or relative), used to determine I and J coordinates in G02 and G03 (arc) commands.
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.
DistanceModeGCode distance mode (absoulte or relative), used to determine X, Y and Z coordinates.
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.
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.
PlungeFeedrateThe feed rate to use when plunging.
SourceFileThis is the filename of the g-code file which will be created.
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.
WorkPlaneUsed to define the gcode workplane. Arc moves are defined within this plane.
Options are XY, XZ and YZ
Copyright (c) 2018 HexRay Ltd