For starters, I installed the latest OpenbuildsFusion360PostGrbl.cps post-processor in fusion 360 and have the latest firmware in my interface touch on my LEAD 1515 (which grbl is set to this machine). I have the original Blackbox (whatever that is not the 32). I have homed the machine and used the probe to zero out the starting position of my stock. After finishing the probe sequence, X=0, y=0 and z is at 14mm but will go to the z=0 position if I tell it to. I have a very simple job, go cut 5 - 3/8 inch slots in specific places in 36X4" 1/2" (11.7mm) thick baltic birch. It seems to me that it is instructing the machine to head down -10mm as opposed to moving up relatively -10mm from where it is. Here are the first few commands. It buries the bit into the x,y 0,0, point to about 4mm (thich is 14mm-10mm) then starts running across to the X=506 mark. It's at this point I hit the emergency stop button. I marked in red what I think it's doing that is causing the problems. G90 G94 G17 G21 (Operation 1 of 1 : 2D Contour2) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 G0 X506.083 Y51.202 M3 S18000 G4 P1.8 G0 X506.083 Y51.202 Z50.8 F4572 G1 Z5.08 Z1 F2286 Z-5.715 X506.091 Z-5.814 F4572 X506.114 Z-5.911 X506.152 Z-6.003 X506.204 Z-6.088 .... I am not sure where to look to fix this. Nowhere in my fusion simulation does it do this. The model orientation matches how it would sit on the spoil board. I am not sure if I need to change something in the post-processor. Should I remove the G0 commands and just tell it to go up to Z50.8 X506 Y51?
You don't need to fix this - G53 is a move in the Machine co-ordinate system. G90 has put the controller in ABSOLUTE movement mode - go to the co-ordinates specified. G0 Z-10 is a move to the point 10 mm below the Z0 position (home).. If you have homed your machine (essential with this post processor) that line will move to 10 mm below the Z limit switch. If it's not doing that are you sure that you homed your machine? Your probe sets the WORKPLACE coordinate system (wcs) zero. G53 is "non modal" - it only applies to the line of code it is on. After that move the controller reverts to the current (G54 - the first of six possible) wcs Alex.
Just to make sure I shut everything down and turned it on, Homed it, probed it and ran it. It looked like it was going to work but it only made 2 passes at each hole and then when it finished it is instructed to go back to the Z-10 position and it triggered the limit switch. I changed up the tool path to just a slot and had it create the gcode. I followed the same CNC procedure and it immediately shot over to the left and triggered the x limit switch. Looking at the gcode, the post-processor put in an instruction to send it -400mm which triggers the limit switch immediately. again, not in the simulation at all. My origin point is set to the same stock point at I set my probe but it seems to be taking the origin of the model and ignoring it in post-processing. Toolpath G90 G94 G17 G21 (Operation 1 of 1 : Slot2) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 G0 X-400 Y11.038 M3 S18000 G4 P1.8 G0 X-400 Y11.038 Z36.7 F4572 Z16.7 G1 Z14.2 F2286 Y1.038 Z13.884 Y11.038 Z13.569 Y1.038 Z13.253 Y11.038 Z12.938 I am probably missing some Fusion 360 milling concept here. I'm about to redraw the model and make sure the origin is in the corner I zero it by default to see if that fixes it. The only thing I haven't updated is the probe and machine settings software on my flash drive for the Interface Touch. They are about 2 years old. Does anyone know where to download the most recent .SET profiles?
According to the calculated toolpath you have set your origin in Fusion cam at the XY centre of your stock box - I'm guessing you are probing front, left corner? Alex.
Align your CAM and physical workflows. Probing front left = set origin front left to match You want to set Zero where CAM expects Zero. With probing thats almost always Front Left corner, top of the stock. Particularly with Interface (On a PC you have a couple more probe options)
