peter i have the opposite issue, the torch probes, makes the first cut, but doesn't turn off between separate cuts. any suggestions
Need additional info. What CAM? Sample gcode file? Does tool on/off menu work? Is it a Blowback/LF plasma or a HF (EMI preventing proper functioning)
using open builds/fusion360 cam, run through open build control, to black box 32. plasma is cut master 52 with a floating head sensor on z axis. I home the machine then set torch to work zero. torch moves to first cut position, probes appriately, pierces then makes its first cut. I expected torch to shut off after completing first cut but doesn't. it does retract, some while traveling to cut #2 but torch doesn't turn off. at second cut point it probes again with torch burning then make the second cut. is the retraction of the torch after each cut what breaks the arc and turn off the torch? I'll make a new pass and get some code to look at.
hey Peter, code as promised. simple tab with a hole. code is followed as I expect except for the no m5 after cutting out the center circle . I'm struggling with the fusion post inputs little I don't have a great example from the same post processor as the current fusion360/open builds post. Not completely clear where Im entering pierce hieght, or cut height. I'm trying to follow the instruction from README-plasma .md. I've included pic of my 2d cut set up and settings on post page.
pierce height is part of the tool setup, ie it is defined for the tool itself. but that makes it hard to change so we added the pierce height override in the post . if your tool has it defined correctly, then do not override it, not needed. cut height is set as for all tools in the heights tab. in one of your images we see a M5 which is the 'tool off' instruction. as peter said, if the tool does not turn off with the 'tool on/off' controls on the CONTROL screen, then there can be little expectation that the gcode will do it. You should see two M5's in your Gcode. 1 after it cuts the inner circle and 1 after it cuts the outside. If you export your Fusion drawing to an .f3d file and upload it here I will have a look for any problems.
below I've downloaded the fusion file for this set up tab that lacks the m5 code after the first cut. appreciate your input and help
Hi peter, wanted to give an update. I've figured it out, and the table is working ancutting as desired. I thought I'd include some of the hurdles I faced and overcome specific to my build that may be useful to others with similar circumstances. My first challenge was I'm a mac guy. Mac doesn't play well with open build. Getting a mac to speak to the black box was cumbersome at best. Updating firmware was almost impossible with a MAC. I have an interface but was never able to update firmware with it. I was able to connect, jog, and connect wifi but could never get it to update firmware. Updating firmware with mac directly with the wizard was impossible. I spent days investigating python path and watched countless hours of tube without any success. I finally brokedown and borrowed a window pc and was easily able to update firmware. This made connecting by mac possible, and reliable. I was able to creat a firmware thumb drive and update via the interface also . This wasn't difficult but wasn't intuitive, and not a great long term solution for keeping firmware up to date. Conclusion: Learn window, or deal with cumbersome. Hopefully, in the future open builds con address this for MAC users. next hurdle was knowing what I needed to do for parameters, ie probe offset, material height, cutting height, piecing height, and safe travel height, but having to translate these definition into fusion 360 setup, tool path set up and code creator, as these terms didn't jive. There was not one condensed forum entry, tube video, etc that defined these completely. Many good starting points like Dr. D Flo but each used a vastly different post processor than open builds leading some confusion. The best explanation of this process was by JOSH DAVIS and his DIY table. He parted the clouds for me. He had the most complete instructions for posting from fusion that I've found, even though he uses each 3 instead of open builds. I've included a link to his set up page on tube for those interested. He used a floating torch height probe and talked through the process in great detail. I though about making a video, but don't know where to begin,
on opening the file I notice that the penetration points are in the material you are keeping. ie the little green lines are in the part not in the waste. i will fix that after i generate gcode with everythgin exactly as it imported.... 2nd thing, you have not set the WCS right click the setup select 'edit' select 'postprocess' tab set 'WCS offset' to 1 right click the edit box select 'save as user default' 3 - you have multiple 'nc program's, looks like you are generating anew one each time you post direct from the 2D profile cut. You should rather use the NC program, it retains all the post settings for you. initial gcode does indeed contain 2 M5 codes, one after the inner circle is cut, and one after the outer profile is cut. I corrected the start pierce positions by deselecting the face and selecting the circle and outer perimeter as cut lines Gcode is good, contains two M5 torch off commands as expected. (actually 3, last one is a safety 'just in case before end of program' turn off) Code: (Made in : Autodesk CAM Post Processor) (G-Code optimized for Grbl 1.1 / BlackBox controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.42) (Units = inch) (Laser UseZ = false) (Laser UsePierce = false) (Arcs are limited to the XY plane: if you want vertical arcs then) (edit allowedCircularPlanes in the CPS file) (Drawing name : set up tab v3 v1) (Program Name : plasma) (1 Operation :) (1 : 2D Profile1) ( Work Coordinate System : G54) ( Tool 1: Plasma Cutter Diam = 1.5inch) ( Machining time : 0h:0m:15s) G90 G94 G17 G20 (Plasma pierce height 0.157) (Plasma topHeight 0.01) (Operation 1 of 1 : 2D Profile1) G54 (Plasma cutting with GRBL.) (Using torch height probe and pierce delay.) (This relies on homing, see https://openbuilds.com/search/127200199/?q=G53+fusion ) G53 G0 Z-0.3937 G0 X1.2829 Y0.7005 F40 G0 X1.2829 Y0.7005 Z0.6 G38.2 Z-1.1811 F4 G10 L20 Z-0.0709 G0 X1.2829 Y0.7005 ; force position after probe Z0.157 M3 S1000 G4 P1.75 G1 Z0.01 F508 G1 X1.3149 Y0.6557 F20 G3 X0.7651 Y1.4243 I-0.2749 J0.3843 F40 X1.3149 Y0.6557 I0.2749 J-0.3843 G1 X1.2829 Y0.7005 M5 G0 Z0.2 X1.4743 Y-0.0425 G38.2 Z-1.1811 F4 G10 L20 Z-0.0709 G0 X1.4743 Y-0.0425 ; force position after probe Z0.157 M3 G4 P1.75 G1 Z0.01 F508 G1 X1.4743 Y0.0125 F20 X0.44 Y0.0125 F40 G2 X0.0125 Y0.44 I0 J0.4275 G1 X0.0125 Y1.54 G2 X0.54 Y2.0675 I0.5275 J0 G1 X1.54 Y2.0675 G2 X2.0675 Y1.54 I0 J-0.5275 G1 X2.0675 Y0.54 G2 X1.54 Y0.0125 I-0.5275 J0 G1 X1.4743 Y0.0125 X1.4743 Y-0.0425 M5 G0 Z0.6 M5 G0 X0 Y0 M30 conclusion: nothing wrong with the Gcode, something wrong with machine in that arc is not turning off when told to turn off.
So back to Wednesday's question If not, does your plasma have a 2T/4T switch on the front (try other position)
Peter got the table up and cutting well but now having a fusion issue when setting up a new piece to cut, i complete the setup, but when setting up the tool path, only the outside cuts are simulated. I've made sure leading and readouts are minimized but still no internal cut tool paths. Not sure where to go?
Include more details? Gcode file, Fusion file etc Otherwise we are a little in the dark. The more info you provide the easier we can see whats going on
I've included my fusion file for cutting out a simple tab. My issue is when creating a 2d tool path, it's not recognizing the 4 holes and only giving instructions to cut out the outline of the tab. also in the geometry setup, selecting the face doesn't select the holes. in this file I tried to select each contour but even then the four holes are not part of the cut path.
Hi - I've looked at your Fusion file: You have the kerf width of the plasma set at 0.55", but the holes are only 0.39" diameter, so Fusion cannot find a way to cut them. If you reduce the kerf width (part of the tool definition) to 0.06", say, the holes cut OK. I'm not sure about nozzle clearance diameter - there are conflicting definitions as to whether it is the actual diameter of the torch head, or the diameter of the pierce hole (even Autodesk info isn't consistent on this). Leaving it as 1" causes odd effects in simulation, but probably OK in real life. I don't do plasma cutting, so haven't really got an answer for that.
