I'm trying to determine if there is something wrong with my BlackBox controller, or just my understanding of it. I'm working with a LEAD 1515 CNC with a Dewalt spindle and the BlackBox controller. I've been using Fusion360 and became curious about the coordinate systems implementations. I found this YouTube video about understanding coordinate systems in the GRBL controllers. I followed the steps he uses to Home the gantry, and then return it to a stored position on the work surface. I'm on a Mac, so I've been using Candle to send commands directly to the controller. This appears to work well, but please let me know if there are issues with this application. After following his instructions, my gantry does not return to the stored position for the G59 work coordinate system. Here's the video and sequence he describes: The command sequence he describes (with my intended modifications) is: Code: // Home the gantry $H // Set the coordinate system to G59 to create a space where I can move the gantry out of the way. G59 // Move the Y axis back away from the front of the machine G91 X0 Y500 Z0 // Set the current work coordinate system's 0 position. G10 L20 P0 X0 Y0 Z0 // Review the coordinate system configurations. This appears to be correct for the G59 coordinate system in my configuration $# // Home the gantry again $H // Return the gantry to the stored position. // THIS IS WHERE MY FAILURE APPEARS TO OCCUR // My gantry does not move at all after this command, in the video, his gantry returns to the stored position. G0 X0 Y0 Z0 Thoughts on why this is happening. Am I not understanding something about work coordinates? Is my controller not doing something its supposed to? Thanks for any assistance.
Use OpenBuildsCONTROL > OpenBuilds Software - FREE Software for CNC Control: OpenBuilds CONTROL and OpenBuilds CAM - runs on Mac too - easier to understand Use our Post too: docs:software:fusion360 [OpenBuilds Documentation] Using our post and our software its as simple as: 1) Home the machine on power up (or after any abort event like an alarm or a crash where machine position is lost) (Sets machine coordinates) 2) Jog to origin and Zero or Probe to set Zero (Sets Work Coordinates) 3) Run the GCODE Are you in G59 after the homing, may need to go back to G59 first
Thanks for the feedback @Peter Van Der Walt . I'll confirm if the coordinate system needs to be reset after homing. Regarding the application recommendation. I do run the OpenBuilds app when I execute GCode, but the Post Processor for the LEAD 1515 that I have is generating GCode that is crashing the bit into the work piece when it's set to the origin position. I have to manually fix the GCode every time I generate it. I am using the Candle app to send commands to the controller directly, which the OpenBuilds app does not allow me to do (that I can tell). My hope is to find the issue with the PostProcessor and fix it, but before I can do that, I have to get the behaviors to match the expectations. I have tried forking the OpenBuilds app repository to implement a command line in the Application, however, I cannot get the code to build properly in NodeJS. I'm getting a NodeJS versioning error with regard to the SerialPort library. Until I can do that I'm back to the Candle app to try and figure out what GCode needs to be generated by the PostProcessor to get it to behave properly.
@Peter Van Der Walt -- I'm facepalming a bit. I just notices that the Serial Console tab has an input for sending commands to the controller. I will try that and see if I can get better results.
Use our Post. Remember to Home and it will all be great, no need to edit any gcode Provided you are homing correctly (Z to the top) Serial terminal tab > input field and Send button right at the bottom
1 - Candle is ancient and has not been updated in quite some time. 2 - Candle does not support coordinate systems other than G54, ie if you set G56 and then use the setZero buttons, it will actually set G54 offsets (or G92 a hazy memory tells me, which is way worse than simply ignoring the selected system). 3 - it has no way of selecting a coordinate system other than manually entering code, this leads to mistakes, which can be expensive. 4 - Homing resets the controller, which also means that the default G54 system becomes active, and Gcode you produce MUST ALWAYS select the coordinate system it expects,along with any other settings. (which implies that YOU must also set what you expect after a reset, and also after some other file or process has run, never assume the modes are correct) 5 - Are you using the OB post for Fusion? The built in post for GRBL is not good at all, that is why we created our own good one (-: We know exactly what it does and what you need to do to make the system work correctly. 6 - Your Z home position is high up at the Z+ end of travel, right? If not, rewire it now, this is a requirement for every CNC machine everywhere and all the posts assume that this is the situation.
