Hi David! First and foremost: I am not the creator of this wonderful tool. *The creator, maintainer and lead developer of this tool is Juan Pablo Caram (aka JP). * He is the one that deserves all the credits. We, the rest, are just helping him, doing some features, as he can no longer be as active as some time ago. He is still helping us, those few who are putting some time into this tool. Read about JP here: http://caram.cl/ About the requested features. I will try to give you an short answer as I'm not the lead developer but I've got and idea about how things work. *Wish1* - there is some discussion about this feature but I don't see it coming soon unless someone wants to help. *Wish2 and Wish4* are linked together. In order for this to work you need some kind of feedback from the machine. Please bear in mind that FlatCAM is a tool. There is a good reason why there a re many tools and not a single universal one. There are multifunctional tools but those are not so good as those specialized. FlatCAM is FlatCAM. A nice CAM software. *Wish3* - that , I think, it is doable. To merge the Gcode files in a single file. We will see. *Wish5* - again, I don't see it but who knows ... if JP will get more time for coding he might add some basic features like adding width to the drawn lines, circular polygons so you might draw something in the Geometry editor. There is no Excellon editor yet. You should know, that every feature added, even simplest ones, require a lot of work and documentation and bug fixing and so on. If more peoples come onboard and start developing, some of your wishes might come true after all :)
Hi Marius, Just a quick clarification on Wish2 - Many machines have feedback already - All that is needed is the GCODE for probe, then to set the Z-axis. A final requirement would be to locate a part of the board where copper exists so that a disconnected piece of the board is not probed. Autoleveller software uses this same feature. So all that would be needed here is a tickbox that generates GCODE at the start like; G20 (Inches) G90 (Absolute distance) G92 Z0 (Set Z=0 to whatever height Z is now... We assume it's above the workpiece ) G0 X0 Y0 Z0 (Use the origin perhaps as the probe point? Maybe there's a better one ) G31 Z-2.00 F5 (Probe down to -2 inches slowly. Stop when the probe touches the board ) G92 Z0 (Set this new height as Z=0. Tool is now touching the board surface ) The danger would be that we will crash the tool if the probe isn't attached, but this could be fixed with a pause, and a warning in the GCODE when it's implemented. The G31 Z-2.00 F5 assumes the tool is within 2" of the board surface Sometimes I cut and paste something like this into t he G-code myself before running a drill process. Thanks for the comments about JP - This really is amazing software.
Hi David, Your suggestion is doable. It will require a new postprocessor. But the possible crash part is making me uncertain if this should be implemented ... As for myself I am using a different approach. A manual one. I've included in the Nightly's that I post a postprocessor named "manual_toolchange". It does not use automatic probing but use ones eye and touch. How it is working: Before the GCode is run I mount loosely a drill bit in the spindle (usually the first tool) and move the CNC to a certain X and Y positions that I find to be suitable. After that I lower the spindle slowly until the drill bit is just above the PCB. I let loose the drill bit, it will fall slightly and make contact to the PCB. I tighten the tool loosely, make Z=0 in the CNC sender (be it bCNC or Mach3 etc), raise the spindle, tighten a bit more the drill bit in the chuck. I start the GCode and when a toolchange command is encountered it will go to a "toolchange Z" (I personally use 30mm as a Z to change the tools). Then it will go to X0Y0 and Pause (spindle OFF). In this moment I mou nt the drill bit loosely in the chuck and press Continue. The drill bit will be lowered slowly until Z=0 and then Pause. I let loose the drill bit, it falls a bit and touch the PCB, I tighten just a bit the drill bit, press Continue, the drill bit is raised until Toolchange Z is reached and then Pause. Here I may tighten the drill bit more (without fear that I break small drill bits) and then press Continue, Spindle is ON and then CNC will start the drilling process. And so on until the end when the Spindle will go to the EndZ (FlatCAM parameter) which is the Z park position, stop spindle and then go to X=0, Y=0 where the router is parked. I park the spindle in the X=0, Y=0 due of the fact that my router has unsupported round rails, and it's the best position to avoid "bending" of the rails (although mine are 20mm in diameter).
Errata: the last X=0 Y=0 are actually around the limit switch positions because I choose them around there (suitable for me).