I'm seeing inconsistent start Z heights when I begin running a job. I usually start by zeroing the cutter, then moving it up a bit to be sure the bit doesn't catch on the stock when I turn it on. Then I hit the start button. In some cases my bit travels to zero and then goes to the beginning of the tool path. In some cases the bit travels to substantially below zero and then goes to the beginning (I've destroyed two pieces this way). I've seen both behaviors running the same file, and I'm not sure what's causing the difference. I'm running the current version of the control software on OSX. Not sure if this is relevant, but I had to disable the limit switches due to a broken switch.
Are you meticulously hitting SETZERO before running? It has to know where the stock's Origin is, and thats up to the human in the keyboard to tell it where it is by jogging to origin and setting zero See
I mean that I set X Y and Z axes to zero at the same location on my stock piece. Sometimes when I start the run the cutter moves horizontally (staying at Z=0) and sometimes it drops down by about 15mm and then moves horizontally, slicing a groove through my stock. I've verified this path isn't part of my file - it's coming from how the tool moves from where it is when I start the job to the first position defined in the file. As I said, the behavior isn't consistent - I've seen both behaviors with the same file. My assumption is there's some type of persistent state present, either in the software or the controller firmware that's controlling this. How is the cutter _supposed_ to move from it's initial position to the beginning of the first path in the file?
How is the cutter _supposed_ to move from it's initial position to the beginning of the first path in the file? Once you've "set zero" with the tool just touching the top of the work, you would then move the cutter up a few mm (as you've done). The machine then sets the Z position accurately as defined in the G code then proceeds in a straight line to the start position of the job ( which could be anywhere) but is determined by the g code coordinates. I'm beginning to think that the Z stepper is moving in the wrong direction at start up - e.g. wiring fault maybe (if this is your first job attempt) so might be worth investigating.
It's not the Z direction, I've completed a number of jobs with complex engraving successfully. This behavior is intermittent and I haven't found a way to reliably reproduce it. Here's the beginning of one of the jobs I've observed the behavior running, just in case there's something unexpected in the initial commands: (Made in : Autodesk CAM Post Processor) (G Code optimized for OpenBuilds OX,Workbee,Sphinx,Lead with BlackBox GRBL V1.1 controller) (Program Name : 1001) (6 Operations in 2 files.) (File List ( Snowflake6 names.nc) ( Snowflake6 names.02of2.nc) (This is file: 1 of 2) (This file contains the following operations: ) (1 : Registration) ( Tool 3: Flat End Mill 2 Flutes, Diam = 6.35mm, Len = 25.40mm) ( Spindle : RPM = 19700) ( Machining time : 22 sec) (2 : Rough) ( Tool 3: Flat End Mill 2 Flutes, Diam = 6.35mm, Len = 25.40mm) ( Spindle : RPM = 19700) ( Machining time : 9 min 37 sec) (3 : Face) ( Tool 3: Flat End Mill 2 Flutes, Diam = 6.35mm, Len = 25.40mm) ( Spindle : RPM = 19700) ( Machining time : 1 min 0 sec) (Remaining operations located in additional files.) G90 G94 G17 G21 (Operation 1 of 6 : Registration) G90 G53 G0 Z0 G54 S19700 M3 G4 P1.8 X107.786 Y112.264 Z15 X107.786 Y112.264 X107.786 Y112.264 Z2 G1 X107.786 Y112.264 Z0.635 F1651 X107.79 Y112.264 Z0.564 X107.802 Y112.264 Z0.494 X107.822 Y112.264 Z0.425 So I'm pretty new to G-codes, but I think the issue may be related to "G53 G0 Z0" - if I understand correctly G53 is machine coordinates, which isn't related to where I've zeroed the work coordinate system. How is the machine coordinate system defined? Immediately after that instruction the coordinate mode switches to G54 and moves to X107.786 Y112.264.
Correct, G53 is Machine Coordinates, that can ONLY be set by Homing. Having homing limit at Z such that it retracts fully from the bed is a safety thing, G53 Z(low value) is a good move to avoid a crash (move up and out of the way before any XY moves - if its up its unlikely to crash into any stock or clamps or other fixturing) If you machine doesn't have limits, get them, setup homing, and home everytime your power it up
Just to close the loop on this, the problem was that I hadn't been homing the machine consistently, so the machine coordinate system (G53) was set based on the cutter location when the machine was powered on, which wasn't consistent, and occasionally resulted in G53 G0 Z0 being in the middle of my piece. Thanks for the help!
