Backplotting + NCFile object

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 from Windows Explorer.

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 interpreted 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.

New [0.9.8]

As of version 0.9.8, the contents of the gcode file referenced in the NCFile object, will be written to the gcode output of the parent drawing. Also, by double clicking the NCFile machining operation in the drawing tree, the gcode source file will be opened in the configured gcode editor.

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.


Arc Center Mode GCode distance mode (Absolute or Relative), used to determine I and J coordinates in G02 and G03 (arc) commands.
Custom MOP Footer A multi-line gcode script that will be inserted into the gcode post after the current machining operation.
Custom MOP Header A multi-line gcode script that will be inserted into the gcode post before the current machining operation.
Cut Feedrate The feed rate to use when cutting.
Distance Mode GCode distance mode (Absolute or Relative), used to determine X, Y and Z coordinates.
Enabled True: The toolpaths associated with this machining operation are displayed and included in the gcode output
False: The operation will be ignored and no gcode or tool paths will be produced for this operation.
Max Crossover Distance

Maximum distance as a fraction (0-1) of the tool diameter to cut in horizontal transitions.

If the distance to the next toolpath exceeds MaxCrossoverDistance, a retract, rapid and plunge to the next position, via the clearance plane, is inserted.


Each machine operation can be given a meaningful name or description.
This is output in the gcode as a comment and is useful for keeping track of the function of each machining operation.

Optimisation Mode

An option that controls how the toolpaths are ordered in gcode output.

New (0.9.8) - A new, improved optimiser currently in testing.
Legacy (0.9.7) - Toolpaths are ordered using same logic as version 0.9.7.
None - Toolpaths are not optimised and are written in the order they were generated.

Plunge Feedrate The feed rate to use when plunging.
Source File The filename of the gcode file which will be read, back plotted and inserted into output gcode.
Start Point

Used to select a point, near to where the first toolpath should begin machining.
If a start point is defined, a small circle will be displayed at this point when the machining operation is selected. The start point circle can be moved by clicking and dragging.

[New! 0.9.8]

Select a CAM Style for this machining operation. All default parameters will be inherited from this style.


A general purpose, multi-line text field that can be used to store notes or parameter data.

Tool Diameter

This is the diameter of the current tool in drawing units.

If the tool diameter is 0, the diameter from the tool information stored in the tool library for the given tool number will be used.

Tool Number

The ToolNumber is used to identify the current tool.

If ToolNumber changes between successive machine ops a toolchange instruction is created in gcode. ToolNumber=0 is a special case which will not issue a toolchange.

The tool number is also used to look up tool information in the current tool library. The tool library is specified in the containing Part, or if this is not present in the Machining folder level. If no tool library is defined the Default-(units) tool library is assumed.

Tool Profile

The shape of the cutter

If the tool profile is Unspecified, the profile from the tool information stored in the tool library for the given tool number will be used.

EndMill | BullNose | BallNose | Vcutter | Drill | Lathe

Work Plane Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY | XZ | YZ
Copyright (c) 2018 HexRay Ltd