I believe I have discovered a small bug in the BlackBox post for Fusion360. The post is inserting G53 after G54, rendering the WCS useless. Or is this user error somewhere? Admittedly this is my first time setting up a Blackbox and I have never used Fusion for CAM before. Awesome little controller, by the way. Below is the beginning to one of my Gcode files: Made in : Autodesk CAM Post Processor) (G Code optimized for Openbuilds blackbox controller) (OpenBuilds CNC : GRBL BlackBox) (Post Processor : OpenbuildsFusion360PostGrbl.cps V1.0.21) (Units = mm) (Drawing name : Untitled) (Program Name : 1001) (Program Comments : Facemilling) (1 Operation in 1 files.) (File List: ) ( facemilling.gcode) (This is file: 1 of 1) (This file contains the following operations: ) (1 : Face2) ( Work Coordinate System : G54) ( Tool 1: Flat End Mill 2 Flutes, Diam = 19.05mm, Len = 19.05mm) ( Spindle : RPM = 16000.000000000002, set router dial to 1.0) ( Machining time : 32 sec) G90 G94 G17 G21 (When using Fusion 360 for Personal Use, the feedrate of ) (rapid moves is reduced to match the feedrate of cutting ) (moves, which can increase machining time. Unrestricted ) (rapid moves are available with a Fusion 360 Subscription. ) (Operation 1 of 1 : Face2) G54 G53 G0 Z10
G53 ONLY applies on lines it contains (See G Codes). the set coordinate system is G54, then just the Z safe move is in G53, after it everything else is understood to be G54 again until a G54-G59 is encountered. G53 is never modal. Your crash is rather you set your start and end of job Z position positive (past the switch) - try [-10]
This doesn't seem to be the behavior I am experiencing. During earlier troubleshooting I already offset the "safe" Z, and it no longer goes past my switch. Here is my workflow using Openbuilds Control. Home machine on all axis. Jog machine to set WCS Zero on X and Y. Use probe (puck style) to set WCS on Z. Confirm WCS are correct. Load up Gcode file, review, and run. Z moves up via G53 Z moves back down some amount, and begins cutting in the air. My Z WCS shows it has been reset in Openbuilds Control. Edit: should also add that I have calibrated my steps.
In most cases it will cut air before it reaches your stock unless you are doing something like a plunge. That distance is determined in your toolpath settings. Does the Fusion simulation mimic what you are seeing on the machine?
When you say "confirm wcs are correct" how do you do that? Does the dro say XYZ are all zero in the wcs when the bit is actually at workplace zero? As @Peter Van Der Walt said G53 definitely only applies to the line of code it is on, and doesn't over-ride any wcs settings (which, unlike G53, are modal - they stay set until you change them in g-code). Post a bit more of a troublesome g-code file so we can see what the next few lines are saying. Alex.
The simulation looks good. Z starts cutting in the air and then moves into the work piece as intended during simulation. During live however, the Z is still like, 20+mm in the air cutting. Here are my settings from the "heights" tab in fusion 360: Clearance: 10mm from retract. Retract: 5mm from stock top Feed: 5mm from Top height Top height: 0mm from stock top. Bottom height: 0mm from stock bottom. Removing G53, from any position my machine will go to WCS zero on X, Y, and Z (with safe height) and perform as expected. I haven't tried reversing the order of the commands yet.
Are you sure that your Z0 origin is the same in fusion that it is on your machine. Certainly sounds like maybe you have your origin set to the bottom of your stock in fusion but set it to the top of the stock on your machine. Otherwise, post your fusion file and your gcode file.
Correct- I am confirming WCS all read zero via the Openbuilds control software while the axis are positioned as I want. Well, technically the Z reads 25mm, as the spindle is roughly that amount away from the work piece after using the probe. I can confirm if I tell the machine to move to WCS zero on Z, the spindle moves to the stock piece as expected. Included is a full Gcode file.
I can confirm that the Z steps are properly calibrated. Here is my initial test file in fusion I was using.
I just post processed your file, using the default G53 setting of -10. Ran it on my machine and it did exactly what it was supposed to do. So its not a bug with the post processor. For the heck of it, I'll go test the gcode file you posted.
Hello, I think I may be experiencing something similar Jonathan. I run the maker's space at our high school and we recently received our openbuilds cnc and it is great! I should also add that I am relatively new to using the CNC. I am running a lead 1010 machine with the blackbox controller. I am using the post processing add-on for fusion 360 to generate my gcode. I think I may be experiencing some disconnect during the post processing. When I run the job, the router plunges into the workpiece at least 1.5" before coming back to the WCS and beginning the first facing operation. I have set my coordinate system to be at the bottom right of the workpiece in fusion 360 and then manually set the same coordinate plane on the lead 1010. I have tried setting the "Start and End of job z position" setting to 0 and -10 without any change in the initial plunge. This behavior is not seen in the fusion 360 simulation, so I am assuming something is happening in the post processing. Can anyone see where I am going wrong or provide some advice on making the machine not plunge at the beginning of the run? I have attached some photos of my WCS in fusion 360, my beginning gcode, and my post processor settings. Thank you very much for the feedback!
Did you remember to HOME to establish Machine Coordinates? Most often people forget to home, machine doesn't know where G53 coodinate set is, resulting in weird moves
Oh man that was it! Thank you so much. I will make sure to remember to home the machine at the beginning of EACH job from now on
PS: 0 will still hit the switch (0 was where the switch triggered during homing) so ALWAYS set that to "less than 0" - can be -1, -5, -10, but never 0 or more
Oh I may have misunderstood the offset then! So, for example, if I were to set the offset to 5, it would go up to 5mm below the z home switch rather than 5mm below the WCS? Thanks a bunch for the PS!
-5 would be 5 mm below the switch 5 would be 5 mm ABOVE it. Jobend start and end Z position. The Z home position (MACHINE co-ordinates) is set to zero where the switch is triggered, but that is also the MAXIMUM for the Z axis, so all the co-ordinates below that have to be less than zero - negative values in other words. Alex.
