Hi Peter,
Thank you for posting the link your free online CAD/CAM software which looks most interesting.
Hi Tweakie. Nice to meet you and your interest is most welcome.
I think there are perhaps one or two changes which may need to be made to make it more Mach3 / Mach4 friendly and I will post more details once I have tested the generated code on my machine.
Tweakie.
Definitely changes are needed to offer full compatibility with Mach controllers but your helpful reply has sparked off some interest in me in developing such a compatibility.
Couldn’t resist trying this before meeting friends for lunch.
Friends in real life? Lucky you! Mine seem to be all on line. Otherwise I suppose I might be spending Christmas day with them instead of with my PC, wishing everyone on the internet "Happy Christmas"!
I had to make a few changes (some essential & some desirable) to the generated Gcode file to make it compatible with Mach3 Laser use and these were as follows:-
M00 deleted (it cannot share the same line as another command in the same modal group (M23) and it is not really necessary).
I've made that change to my webpage - to the BASIC code option only - the MACRO is a whole other can of worms to fix which I will need to take time over.
There was no particular reason to put both M commands on the same line but CNC Simulator Pro didn't seem to mind.
G4 P100 deleted (a plasma start delay is not necessary for CO2 laser).
I've left that in for now. Are you sure that even for thick sheets the CO2 laser doesn't ever need some dwell time to get a cut started?
G91.1 added (to ensure Incremental Arcs mode).
I've put that in. Incremental IJ values for arcs seems to be the default on CNC Simulator Pro.
G21 added (to ensure operation in metric units).
I've added that.
F600 added at start of file (a feed-rate must be specified for feed-rate moves).
I've not done that yet on the webpage. It is easy enough to add manually meanwhile. Since feed-rate could be different for different jobs, it probably warrants an input option for feed-rate on my webpage.
M22 replaced with M11P1 (laser on).
M23 deleted (laser off must be followed by an axis movement).
G00 replaced with G00 M10P1 (turns laser off prior to rapid moves).
% added at end of file (all files must end with a Carriage Return and a null character forces the CR).
Not done any of those yet. I was happy enough for this initial reply to you just to get the toolpath displaying correctly when I load up the gcode, see attached image.
I was pleased to get it working at all because I am running windows 8.1 - on a 64-bit machine and Mach3 is not supposed to work here. There is a windows version compatibility troubleshooter which I used and maybe that made all the difference?
Haven’t actually cut any yet but this was laser drawn at low power on a spoil board just to verify the code.
Very nice. I'd like to post your laser drawing elsewhere as proof of concept of my webpage if that's OK?
You have indeed produced an excellent piece of software my friend.
Tweakie.
That's kind of you to say so Tweakie, especially after all the tedious editing to my code you must have had to do to allow it to draw 29 tiles. Ideally, I'd like to develop the software so that it generates code that can work without (a lot of) additional editing.