Hello all. First time poster and new to the whole CNC party. But very excited about my work-bee 1010. I have weird intermediate glitch with my Z axis. I only happens when i first boot everything up. after I align everything as zero-out my work space and try to run a program the z axis drops about 5 mm, then pulls back the 5 mm and then runs to code. Program runs fine it's just the start. I can disconnect everything reboot and then she'll drop 15 mm, pull back and then run the code. I reboot everything and then the same code run's perfect. No initial drop and pull back. After this i can run ad many codes as i want and the is gone. But the minute i power down and restart the issue is back. Tried on another updated windows 10 PC and same issue. Problem is it's digging into my work piece. Any i ideas? Workbee 1015 converted to a 1010 to get the screw drives. Openbuilds Control latest version. Fusion360 to create and post process. Windows 8 laptop. Clean formatted and only runs CNC. Thank you,
So when the machine is idle, it unlocks the motors, and gravity helps it drop? Set $1=255 to keep motors locked (our Grbl profiles sets it too, just good practise) Refer to gnea/grbl
not sure it's just when idle. I can have it on and idled and nothing happens. It's happens immediately after I hit - "Run program." Then the Z goes down, then back up. then program runs. There was one instance that it just went down and proceed to goto the start position. Carved a big trench in the work piece. Thanks for the link.
Are there any G53 Zx moves in the Gcode file near the point it goes funny? Where's the GCODE from? Upload the GCODE?
As @Peter Van Der Walt said, let us have a look at your g-code. Which post processor are you using with Fusion? - it should be this one if you are using a grbl controller ; Fusion 360: grbl post processor install (the easy way) Alex.
I've attached uploaded the Gcode. But here's the begining: (can holder 5) (can holder ) (Machine) ( vendor: Autodesk) ( description: Generic 3-axis) (T1 D=6.35 CR=0 - ZMIN=-19 - flat end mill) G90 G94 G17 G21 G28 G91 Z0 G90 (Contour3) S18001 M3 G54 G0 X-1.305 Y50.928 Z16 Z1.634 G1 Z-0.481 F1016 X-1.298 Y50.925 Z-0.571 X-1.276 Y50.917 Z-0.659 X-1.24 Y50.903 Z-0.741 X-1.192 Y50.884 Z-0.815 X-1.132 Y50.861 Z-0.879 X-1.063 Y50.834 Z-0.93 X-0.987 Y50.804 Z-0.969 X-0.906 Y50.773 Z-0.992 X-0.822 Y50.74 Z-1 G3 X0 Y51.102 I0.23 J0.592 G1 X0.109 Y51.381 F2794 X0.181 Y51.583 X0.463 Y52.389 X0.527 Y52.59 X0.779 Y53.396 X0.805 Y53.484 X1.059 Y54.404 X1.11 Y54.605 X1.304 Y55.411 X1.349 Y55.613 X1.514 Y56.419 X1.554 Y56.62 X1.725 Y57.628 X1.753 Y57.829 X1.862 Y58.635 X1.884 Y58.837 X1.966 Y59.643 X1.983 Y59.844 X2.038 Y60.65 X2.05 Y60.852 X2.084 Y61.859 X2.086 Y62.061 Y62.867 Thanks again for all the help.
I was thinking the same thing, as soon as I saw that "Autodesk" - I'd recently been running into the same problems with G54s from Fusion. I haven't tried his - are the changes substantial beyond that? I just ended up modified their stock grbl post myself and got it working closer to what I wanted, but I'm still not exactly familiar with grbl, so I'm not sure what other pitfalls still lurk in the depths of it. -Bats (hopefully not the kind of pitfalls where you have to use vines to jump over holes with snakes in them. I was never much good at those. I blame the Atari joysticks.)
Here's what i get (Made in : Autodesk CAM Post Processor) (G Code optimized for Autodesk with controller) (Program Name : 1001) (Program Comments : can holder) (1 Operation in 1 files.) (File List ( 1001.nc) (This is file: 1 of 1) (This file contains the following operations: ) (1 : Contour3) ( Tool 1: Flat End Mill 2 Flutes, Diam = 6.35mm, Len = 38.10mm) ( Spindle : RPM = 18001.2) ( Machining time : 9 min 59 sec) G90 G94 G17 G21 (Operation 1 of 1 : Contour3) G90 G53 G0 Z-10 G54 S18001 M3 G4 P1.8 X-1.305 Y50.928 Z16 X-1.305 Y50.928 X-1.305 Y50.928 Z1.634 G1 X-1.305 Y50.928 Z-0.481 F1016 X-1.268 Y50.914 Z-0.68 X-1.164 Y50.873 Z-0.848 X-1.007 Y50.812 Z-0.961 X-0.822 Y50.74 Z-1 G17 G3 X0 Y51.102 Z-1 I0.23 J0.592 G1 X0.109 Y51.381 F2794 X0.181 Y51.583 X0.463 Y52.389 X0.527 Y52.59
Worked like a charm thank you. Except for this line. G53 G0 Z-10 # z drop 10 mm then traveled to start location. changed to G53 G0 Z5 now it pulls 5 mm then travels to start location. Also - What's with the "Z16" I have to manually delete this on every gcode fusion creates or Z hits the limit switch of the bat. ???
The "warning" is simply telling you that you didn't choose a work co-ordinate system in setup in Fusion so it's using the default of G54. Your other points can I believe be changed, but I don't use that post processor myself, so I'll leave that bit to someone who knows more about it, like @David the swarfer. Alex.
You might want to check the Heights tab in the toolpath (in Fusion), and see if any of them are set outside of where your Z is capable of moving, since it (probably - I haven't played with the newer machine definition features yet) doesn't know much about what your particular machine can or can't do. -Bats (my machine has many scars to attest to this fact. oops.)
yeah, the post has options, if your hover your mouse over each one in turn you will get a popup with help that you should read. knowledge is power (-: seems to me your machine home (fake or real) is not at the top of Z travel. it MUST be at the top of Z travel for any of the Fusion posts to work (for any posts really since they all assume the machine adheres to the industry standards for machine home. you will benefit from reading this thread .
