-----------------[ A Linux "driver" for the MDX-540 CNC mill: ]-----------------
Publication date: 2025-06-29
 

Roland's CNC machines can't naively run G-code. Instead, they ship a Windows
printer driver that converts G-code into a binary format before it gets
sent to the machine. 

For 90% of people, this is fine, but makes them impossible to use from Linux.
(and could be a problem under Windows in the future, given that my machine
is long discontinued.) 

As a workaround, I wrote a standalone program to convert G-code into the
text-based but naively supported RML format: gcode2rml.c 

Compilation: 

    gcc -lm gcode2rml.c -o gcode2rml
    

Usage: 

    ./gcode2rml [input file.nc] [output file.rml] [nc]
    

If a file is not specified, standard input and standard output is used instead.
Pass "nc" if the mill is set to "NC" mode, omit if it's set to "RML" mode.


The generated RML code should be "printed" to run it on the machine: 

    tee /dev/usb/lp0 < file.rml
     


The mill's starting position will be used as the origin. If you want to
use the coordinate system origin, prepend this sequence to the generated
files: 

    !MC0;
    ^PA;
    !ZEZ0;
    !ZEX0Y0;
    ^PR;
    

This will move to the origin: Z axis first, then X&Y. Make sure this won't
cause any problems. 

If it does, modify the highlighted coordinates: Units are microns in "NC"
mode and 10s of microns in "RML" mode. This will offset both the initial
move and the origin of the coordinate system. 

Supported G-code commands:
##########################
 


Commands                 Function 
G00, G01                 Linear movement (Same feed rate used for both) 
G02, G03                 Circular movement (Only with I,J,K) 
G17, G18, G19            Set circular movement plane 
G10                      Set offset (tool radius offset is not supported) 
G20, G21                 Set units (mm/in) 
G90, G91                 Relative/absolute positioning 
G49, G40                 Clear tool length offset, ignored 
S                        Set spindle speed (approximate) 
F                        Set feed rate 
M00, M01, M02, M30       Stop program, ignored 
M03, M04                 Start spindle (Always clockwise) 
M05                      Stop spindle 
M06                      Tool change, ignored 

Notes:
######
 

I've done a good bit of milling, but there may still be some bugs. I recommend
testing in air to make sure the toolpath is sane. 

Because it uses the text-based format, resolution is limited to 10 microns
(even in NC mode). This is somewhat annoying as the machine is capable of
micron scale movements, and has a backlash of around 3 microns. 

4-axis machining is supported, although 4-axis polar interpolation is not.
The automatic tool changer is not supported because I don't have one. 

It should work on other Roland machines, but I don't have any to test it
on. 

Update: Plotter mode [2025-07-03]
#################################
 

For 2d machines like the "Camm-1" vinyl cutter, compile the program with
this command: 

    gcc gcode2rml.c -lm -o gcode2rml -Dplotter
    

Movement in +Z will be converted into a pen up and -Z into a pen down command.
It's not perfect, and the machine will occasionally give errors, but it
seems to work.