Documentation for the latest CamBam release is available here...

Post Processor System

The format of generated gcode files can be controlled using post processor definitions. These definitions can be created, copied and modified within the Post Processors section of the System tab.

The post processor used for a specific drawing is set under the machining options. Select the machining folder in the drawing tree and look in the Post Processor group of the machining properties. If no post processor is specified, the default post processor will be used.

To set the default post processor, right click the definition in the Post Processors section of the System tab, then select Set As Default. The default definition will be marked with a green arrow.

Machining Properties

Post Processor Management

The list of available post processors is accessed from the Post Processor folder of the system tab. Here, post processor definitions can be created, modified, copied, renamed and deleted.

New post processors can be created via the context menu visible when right clicking the post processor folder. Alternatively, existing definitions can be copied, pasted then modified. This is a good way of creating variations of a working post processor.

If post processor files are modified or new ones created outside of CamBam or in another CamBam instance, the post processor list should be refreshed using the Tools - Reload Post Processors menu option.

Post processors are XML files with a .cbpp file extension, stored in the \post sub folder of the system folder.

Post Processor sections

The post processor definition contains a number of sections. Each section can contain a mixture of literal text, which is output to the destination gcode file directly, and text macros of the format {$macro}. The macro definitions are defined within other sections of the post processor, or by defining user macros in the Post Processor Macros property of drawing's machining options. The macros are evaluated and the resulting text values are written to the gcode output.

(Main) - Post File

This section defines the general structure of the gcode file. It typically includes three macros that are evaluated internally based on rules defined in further sections of the post processor.

{$header} - This macro is evaluated using the Header section described below.
{$mops} - This macro is evaluated to a list of blocks of text, one block per each machining operation. Each block is formatted using the rules in the MOP section.
{$footer} - This macro is evaluated using the Footer section described below.

Example:

%
O{$o}
( MY FANUC POST )
{$header}
G0 X10Y10Z0
{$mops}
{$footer}
%

The % characters are output literally and would be omitted if not using an RS232 file transfer program.

(Main) - Header

Defines the text rules used by the {$header} macro.

Example:

{$comment} {$cbfile.name} {$date} {$endcomment}
{$tooltable}
{$comment} CUTVIEWER {$endcomment}
{$comment} FROM/0,0,5 {$endcomment}
{$comment} TOOL/MILL,1,0,20.0,0 {$endcomment}
{$comment}STOCK/BLOCK,{$stock_width},{$stock_length},
    {$stock_height},{$stock_x},{$stock_y},{$stock_z} {$endcomment}
{$cbfile.header}
{$units} {$distancemode} {$velocitymode} {$cuttercomp(off)}
{$toolchange(first)}
G54 ( Use fixture 1 )
{$clearance}

Once again, the Post Processor Macros property is used to pass the {$stock_...} macros to the post processor, which in this example may contain text such as:

$stock_length=150
$stock_width=150
$stock_height=12.7
$stock_x=75
$stock_y=75
$stock_z=12.7

(Main) - Footer

Defines the text rules used by the {$footer} macro.

Example:

{$clearance}
G28 G91 Z0
G90 G53 X-15.0 Y0.0
M09
{$spindle(off)}
{$endrewind}

(Main) - MOP

Defines how each item of the {$mops} macro is formatted. This information will be repeated in the gcode output for each active machining operation.

Example:

{$comment} {$mop.name} {$endcomment}
{$toolchange}
{$velocitymode} {$workplane}
{$mop.header}
{$spindle} {$s}
{$blocks}
{$mop.footer}

(Main) Start Cut

Macro to use when about to feed cut. This may be used for plasma or laser cutters to power on the cutting tool.

The start of cutting is determined when a feed move is detected where Z is below the stock surface.

(Main) End Cut

Macro to use when finished a feed cut. This may be used for plasma or laser cutters to power off the cutting tool.

The end of cutting is determined when a rapid is detected or a feed move where Z is at or above the stock surface.

For example, to power off a laser to avoid holding tabs, use square holding tabs and set the holding tab height so that the top part of the tab move is above the stock surface. The Start Cut macro will then be invoked when the feed move resumes below the stock surface.

(Main) Post Processor Macros

This property can be used to set default values for any custom macros used in the post processor.

Custom macro values will be overridden by the values set in the Post Processor Macros property of the machining options.

Tools - Tool Table Item

Defines how each item of the {$tooltable} macro is produced. Tool tables are typically inserted in the header of a file and contain commented text describing the list of tools that will be used in the gcode file.

Example:

{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}

Tools - Tool Change

Defines how the {$toolchange} macro is formatted.

Example:

{$clearance}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
{$comment} Tool Radius and Taper coming soon {$endcomment}
{$comment} TOOL/MILL, {$tool.diameter}, {$tool.radius}, 
    {$tool.length}, 0 {$endcomment}
T{$tool.index} M6

G Codes - G0, G1, G2, G3, G81, G82, G83

These sections define how the commonly used gcode operators are output.

G Codes - Arc Center Absolute

Used in the {$mop.header} macro to specify that ArcCenterMode is set to Absolute. Mach3 recognizes G90.1

G Codes - Arc Center Incremental

Used in the {$mop.header} macro to specify that ArcCenterMode is set to Absolute. Mach3 recognizes G91.1

G Codes - Canned Cycle Start

Code sequence used at the start of a group of canned cycle blocks. Typically G98 for initial level return after canned cycles.

G Codes - Canned Cycle End

Code sequence used at the end of a group of canned cycle blocks. Typically G80.

G Codes - Cutter Comp Off, Cutter Comp Left, Cutter Comp Right

Used in the {$cuttercomp(off|L|R)} macros. Typically Off=G40, Left=G41, Right=G42.

G Codes - Distance Absolute, Distance Incremental

Typically absolute=G90, incremental=G91. NOTE! Incremental distance mode is not currently supported.

G Codes - Units (Inches), Units (Metric)

Typically inches=G20, millimeters=G21.

G Codes - Velocity Mode - ExactStop, Velocity Mode - Constant Velocity

Typically exact stop=G61, constant velocity=G64.

G Codes - Workplane XY, Workplane XZ, Workplane YZ

Typically XY=G17, XZ=G18, YZ=G19.

G Codes - X Mode Diameter

Used in the {$lathexmode} macro to specify that X values are in diameter mode. For example; EMC2 recognizes G7.

G Codes - X Mode Radius

Used in the {$lathexmode} macro to specify that X values are in radius mode. For example; EMC2 recognizes G8.

M Codes - End Rewind

Typically M30.

M Codes - Repeat

Typically M47.

M Codes - Spindle CW, Spindle CCW, Spindle Off

Typically CW=M3, CCW=M4, Off=M5.

M Codes - Stop

Typically M0.

Moves - Rapid, Feed Move, Arc CW, Arc CCW

These sections define how the commonly used gcode move instructions are formatted.

Example:

{$g0} {$_f} {$_x} {$_y} {$_z} {$_a} {$_b} {$_c}

{$_g1} {$_f} {$_x} {$_y} {$_z} {$_a} {$_b} {$_c}

{$g2} {$_f} {$_x} {$_y} {$_z} {$i} {$j}

{$g3} {$_f} {$_x} {$_y} {$_z} {$i} {$j}

Canned Cycles - Drill, Drill Dwell, Drill Peck

These sections define how the commonly used canned cycle instructions are formatted.

{$g81} {$_x} {$_y} {$_z} {$_r} {$_f}

{$g82} {$_x} {$_y} {$_z} {$p} {$_r} {$_f}

{$g83} {$_x} {$_y} {$_z} {$p} {$_q} {$_r} {$_f}

Lathe - Lathe Tool Radius Offset

If False, the toolpath at the center of the tool radius is output.

If True, an appropriate tool radius offset is applied. The toolpath will be offset by a negative tool radius in the lathe X axis. The direction of the Z tool radius offset is determined by the cut direction. For right hand cuts the toolpath Z will be offset by a negative tool radius. For left hand cuts, a positive tool radius Z offset is used.

In the diagram above, the red cross represents the toolpath reference point when Lathe Tool Radius Offset is set True. If False, the dot at the tool radius center will be the reference point. The reference point is sometimes referred to as the 'Imaginary' or 'Virtual' tool point.

Lathe - Lathe X Mode

For lathe operations, specifies whether X values are radius or diameter mode.

Line Numbering

Line Numbering - Add Line Numbers

If True then line numbers will be inserted at the begining of g-code lines.

Line Numbering - Line Number Format

Controls how the line number values are presented. '0' characters denote a place holder that will contain either a significant digit or a 0. A '#' character will output a significant digit or space character where there is no significant digit at that position.

Line Numbering - Line Number Increment

Line numbers will be incremented by this amount each time a line number is added.

Line Numbering - Line Number Prefix

This text (typically an 'N' character) will be written before the line number value.

Line Numbering - Line Number Skip

Lines where the first non space character is in this list will not receive a line number.

Line Numbering - Line Number Space After

If True then a space character will be inserted after the line number value.

Line Numbering - Line Number Start

The initial for the first line number used.

Options - Arc Output

Controls how arcs are output to gcode.
If Convert To Lines, small line moves are used rather than arc commands.
Helix Convert To Lines is similar to Convert To Lines, but only for helical arcs (i.e. arcs with varying Z).

Options - Arc Center Mode

This property controls whether the I and J parameters for arc moves (G2, G3) use absolute coordinates or incremental, relative to the arc end points. If this setting is different to the way the CNC controller interprets arc moves, the resulting toolpath may look a mess of random arcs in the controller.

Default When default is set in the drawing's machining properties, the post processor Arc Center Mode will be used. A default value in the post processor will use Incremental (C-P1).

Absolute I & J are absolute coordinates of the arc center point.

Incremental (C-P1) I & J are coordinates of the arc center, offset from the first arc point. This is the typical incremental mode. In previous versions this option was just called Incremental.

Incremental (P1-C) I & J are offsets of the first arc point from the arc center.

Incremental (C-P2) I & J are arc center offsets from the second arc point.

Incremental (P2-C) I & J are offsets of the second arc point from the arc center.

Options - Arc To Lines Tolerance

If Arc Output=Convert To Lines is used, this value controls the maximum allowed error when converting arcs to lines. Smaller tolerances will result in smoother curves but larger files.

Options - Clearance Plane Axis

Used to specify which direction clearance moves are made. Usually Z, but may be set to X or Z for lathe operations.

Options - Comment, End Comment

Defines the text to be used at the beginning and end of a comment.

Example 1:

Comment: (
End Comment: )

Example 2:

Comment: ;
End Comment:

Options - End Of Line

Character sequence used at the end of a line. Escape code \r and \n can be used.

Options - Invert Arcs

Controls the behaviour od XZ (G18) arcs only.

For milling operations, this should be set False. The direction of the g-code arcs will then be relative to the positive Y axis (using a right hand coordinate system).

For lathe operations, this should usually be set True. Lathe arc directions are typically relative to the 'Up' direction. This would imply a positive Y axis using a left hand coordinate system. CamBam's drawing view is a right hand coordinate system so XZ arcs would need to be inverted when written to g-code.

Note: Coordinate handedness can be determined by pointing your thumb in the direction of positive X, second finger in the postive Y axis and third (middle) finger in the positive Z axis direction.

Options - Minimum Arc Length

A numerical value that controls the precision limits used for outputting arc moves (G2, G3). If the length of an arc is less than the Minimum Arc Length value then a straight move (G1) is used instead. This is useful for TurboCNC users where very small arcs can cause glitches that may appear as dimples in the toolpath.

Example:
Minimum Arc Length=1e-4

Options - Maximum Arc Radius

A numerical value that controls the maximum radius allowed for arc moves. If an arcs radius exceeds this value, a straight line move (G1) is used.

Example:
Maximum Arc Radius=1e6

Options - Number Format

This is a string formatting pattern that controls how floating point numbers are displayed.

A hash character (#) denotes an optional digit place holder and a 0 character denotes a digit that is always displayed, adding padding zeros if required.

It can also change the gcode instructions that are required. For example, if a toolpath contains a move from X=1.234 to X=1.233 and a number format of #.#0 is used, no move instruction will be written to the gcode as the coordinates are identical when formatted to 2 decimal places.

Options - Rapid Down To Clearance

If set True, and Z is above the clearance plane a rapid down to the clearance plane is used.
If False the current Z is maintained.

Options - Suppress Parser Errors

The post processor will parse gcode as it is created to update internal values such as registers. This can produce error messages for post processors that produce non-standard gcode. In many cases the gcode will still be correctly generated and the error messages can be ignored.

Setting Suppress Parser Errors to True will prevent the gcode parsing errors being displayed, which may otherwise hide genuine error messages.

Options - Upper Case

If set to True, the post processor converts all text written to the gcode file to upper case. This is particularly useful for Fanuc posts that do not support lower case characters.

Post Build - Post-Build Command and Post-Build Command Args

Post-Build Command can be used to specify an external application to modify the gcode produced from the post processor.

Post-Build Command Args contains any arguments to pass to the application.
The following macros are recognised:
{$outfile} is the filename of the raw gcode output.
{$cbfile.name} is the short name of the current CamBam document.

Note: Double quotes should be used in command arguments to avoid problems with spaces in filenames.

Example:
Post-Build Command=C:\bin\gcodelinenums.exe
Post-Build Command Args="{$outfile}" "{$outfile}.out"

Post Processor Macros

$set(z,5.5)