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"
These parameters are necessary for your machine definition:
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"
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"
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"
This is the description that will appear in the program's "Machines" drop-down.
There are many other parameters which can be set here.
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
if you want the offset toolpath output; default is to output the geometry shape.
This will turn off the line numbers from the output.
This will turn off the tool definitions from the output.
These are the lines starting G10L1.
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
Turns on the output of M18 and M28 commands with drilling operations.
Output drilling operations as rapid and feed commands ( G0 and G1)