Configuring post processors

The machines available to your copy of HeeksCNC are defined in "C:\Program Files (x86)\HeeksCNC\HeeksCNC\nc\machines.xml"

You can edit this file.

It contains lines like this:

<Machine post="emc2b" reader="iso_read" suffix=".ngc" description="LinuxCNC"/>

You can add your own machine in here, and it will appear in the Program's "Machine" drop-down.

For example, if you add this line:

<Machine post="iso" reader="iso_read" suffix=".ngc" description="Machine A"/>

to your "machines.xml"

You will see it in the Program dialog, when you edit the Program object.

These parameters are necessary for your machine definition:

post="iso"

This means that the script file used for generating your g-code, will be "iso.py".

Machine script files are to be found in "C:\Program Files (x86)\HeeksCNC\HeeksCNC\nc"

reader="iso_read"

This means that the script file used to read the g-code and create the graphical toolpath, will be "iso_read.py".

Also found in "C:\Program Files (x86)\HeeksCNC\HeeksCNC\nc"

suffix=".ngc"

This sets the default file suffix for your g-code file.

By default, the g-code file will have the same path and name as your ".heeks" file, but with the ".heeks" replaced with this given suffix.

Popular alternatives are ".tap" and ".nc"

description="Machine A"

This is the description that will appear in the program's "Machines" drop-down.

There are many other parameters which can be set here.

These are:

useCrc="True"

This will enable Cutter Radius Compensation output for your machine ( G40 and G42 )

Be aware that the toolpath shown will not necessarily be the same as on your machine, when using CRC.

You can also use the parameter

useCrcCenterline="True"

if you want the offset toolpath output; default is to output the geometry shape.

output_block_numbers="False"

This will turn off the line numbers from the output.

output_tool_definitions="False"

This will turn off the tool definitions from the output.

These are the lines starting G10L1.

output_h_and_d_at_tool_change="True"

This will turn on the output of H and D on the tool change line

output_g43_on_tool_change_line = "True"

Turns on output of G43 on tool change line

output_internal_coolant_commands="True"

Turns on the output of M18 and M28 commands with drilling operations.

drillExpanded="True"

Output drilling operations as rapid and feed commands ( G0 and G1)