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) |
Help >