I have been playing around with the my newly built cnc router (I built it based on Sam Kellers design) quite a bit. I am using Fusion 360 to design and generate gcode. and then open build controller. I am having an issue with many of my cuts. After I set my zero point at the top of my board and click run on the open build controller, the very first movement the machine makes is straight down. This isn't good because it cuts into my board. I have found in the gcode editor portion of the open build software that "g28 g91 z0" is what is causing this. If I remove that line, the design cuts as it should. Any idea why it is doing this and/or how to fix it? Also, inside of fusion, when I choose my tool etc. there is numerous stock materials to choose from (aluminum, titanium etc.) is there no choice to choose different species of wood? Thanks for any and all help!
Sounds like you are using the wrong Post Processor. Use the OpenBuilds Grbl Post: (no G28) docs:software:fusion360 [OpenBuilds Documentation]
Hey Peter! Thanks! I went through the steps and am now using the correct post processor, but it is still going straight down when I click run.
Make sure you are homing after first startup. Mine shows a G54 Z -.397 (inches or something close) at the start of the code which I figured out will dive into the work piece if you don't home. If you home after startup it will go that far below the limit switch. If you have that line of code you can test if that is it by deleting the G54 Z-.397 line. Found this out the hard way
G54 is Work Coordinates. Do not delete! You forgot to Setzero (homing sets machine coordinates (where is the machine) . Setzero sets work coordinates (where is the stock). Work Coordinates are saved offsets from Machine zero, and thus why rehoming sometimes fixed your issue. But more importantly, is to properly Setzero before every run. Homing to rezero work coordinates only really comes into play with mass production (stock repeatedly located in the same place)
Click Home. Z should raise upward. Refer to the Grbl Wiki > Configuration and Grbl Wiki > Frequently Asked Questions sections for a lot more discussion on this
Please NB note, with a machine and Grbl config properly set up, and using our corrected Grbl Post. You would NEVER need to delete lines from Gcode. Doing so is just wrong. Fix the root issues instead please
Peter, I know this is a very stupid question, but how do I access the wiki page you are referring to (Grbl Wiki > Configuration and Grbl Wiki > Frequently Asked Questions)? Is this it? gnea/grbl Thanks!
I had the same issue with the first move. There is a tab in create nc screen in fusion360 that says "g28" that needs to be changed to "safe retracts." Worked for me.
Yes, the reason is that your machine does not have home switches (not a problem) and you have not set machine home correctly (the problem). All you have to do is turn on (or reset) the controller with Z as high as it will go, every time. This sets a safe Z position that can be counted on by the assumption made by all the Gcode generating software that Z home is high and safe. just put Z as high as it will go and turn on or reset the controller. This sets machine home to a safe height (as far from the work as possible) and also GRBL (the software in the controller) will set the G28 position to 0,0,0 which is the same as home. Now when the Gcode issues a G28 safe move it will go up instead of down, as intended. More information here and you should also switch to the OpenBuilds Fusion post, it is just much better then the stock one google 'feedrate for routing wood' and you will find answers. you can also just start with aluminum settings which will be good for most hardwoods (except the insanely hard like ironwood) and you can speed it up for softer woods (but not so much for pine, the grain is as hard as a hardwood so set rates for that, the soft parts will get cut just fine)
Indeed that does work but it does not address the fundamental elephant, the machine does not have a safe home position that is the basis for industry safety and basic assumptions made by the Gcode generators on the back of those industry standards (generated from a couple of generations of machinists losing fingers/hands/arms to non standard machine setups). I did illustrate the correct settings for the stock post in this thread but the OB post is much better so I do recommend that (-: I use the G28 position for tool changes which does imply that Z is high and safe, but I do prefer to use G53 moves for safety (used in the OB post). G28 is a set position, the user can set it anywhere (though GRBL defaults to machine home 0,0,0) G53 moves in absolute machine coordinates which removes that one element of randomness but does mean that a minimum of 'Z high home' is needed for proper functioning. I created a macro to send the machine home, which I use before I turn off. Available in the thread linked above.
