Am I correct in thinking that your Z height switch is the microswitch here, and that it is actuated by the grey block below it? If so, it appears from the second video that the probe cycles complete without this switch making contact with anything. This is almost certainly due to electrical noise/interference on the probe input (not necessarily from the plasma). Also, although I can't see from the video, your initial Z probe seems to happen very quickly, with little movement, so I suspect that the same thing is happening there. Is your probing switch 'normally open'? You could improve things massively by changing it to 'normally closed' (different connections to the switch, connect switch between A5 and ground, resistor between probe input and +5V & change $6 to 1). Also, add a small filter capacitor (as for the 'NC limit switches with improved filtering' here ) and use a separate screened cable for the probe switch connections. [Note from the video: You shouldn't need to zero the Z coordinate after probing (I saw you pressing Set XYZ zero button after probing) - just zero X and Y if needed]
hmmm. It should be moving far enough down to press the nozzle against the metal and compressing the spring until the switch is pressed. Then it should raise the nozzle a little (if you got your offset correct) before starting to cut. Since it is never probing the actual surface I believe MisterG got it right, you have EMI triggering the probe. translated using ChatGPT "Hmmm. Il devrait descendre suffisamment pour presser la buse contre le métal et comprimer le ressort jusqu'à ce que l'interrupteur soit enclenché. Ensuite, il devrait soulever légèrement la buse (si vous avez correctement défini votre décalage) avant de commencer à couper. Étant donné qu'il ne sonde jamais la surface réelle, je crois que MisterG a raison, vous avez des interférences électromagnétiques déclenchant la sonde."
Hello, Here is a small summary of what I accomplished, I installed a 4.7kohm resistor with a capacitor of 0.1uf. i did remouve the keep nozzle down off for this test in fusion 360 Yes de limite switch is on NO for the probing The z-axis does its probing sequence but after a few holes cutted it gives me this alarm here. It's a good start now why do i have this alarme ? I did this test whit no plasma cutter on it is still turn off.
it is time to swap out the USB cable for a shorter, good quality one. that looks like USB corruption, because my previous check showed no radius errors in the arc make sure the USB cable is seperated from all power cables (mains power and cables to the motors)
Hello i did try it direct usb and a still get the error 33 is it normal that if you whant hole .25 in it dosent work ?
When I run your Gcode through my controller I do not get an error, there is nothing wrong with the Gcode. So, There must be something wrong with your machine, and the causes of this kind of error are 1 - EMI 2 - bad USB 3 - non standard settings in GRBL for arcs they should be $11=0.010 ; Junction deviation, millimeters $12=0.002 ; Arc tolerance, millimeters
Rather, post your issue, and screenshots, fusion file, details on which post you are using etc - would be more helpful than a short form follow up question. Include info so we can answer your specific questions (which might seem related but rarely are - a new thread with your specific issue would be better)
New poster here- I've searched for the solution to this Error33 issue to no avail. So: I have this same problem with my JD Garage Arduino Based CNC plasma cutter. I've done the fake home thing, no difference. It's something in Post that is not quite right, but I can't put my finger on it. In my case I'm pretty sure its not EMI or BAD USB I can cause the same error with an Arduino sitting on my desk with a brand new USB cable, and no plasma cutter or Steppermotors within 100 feet of the Arduino. (and it's not even the same Arduino that is on the actual machine) I've even tried different computers ( Mac vs PC) no difference. It also must not be the grbl arc commands either, I've experimented with all sorts of extremes and the error is exactly the same Error 33 right after a Z axis probe. FWIW- JD's recommendation for the grbl settings for those 2 arc commands are are $11=0.020 $12=0.002 I've worked around it, but it's painful. The only fix I have found so far is to do a G0 with X and Y at the last known position after the probe, but before the Z moves to the Pierce height. {Code Snippet } G0 X0.2292 Y5.6942 Z0.725 (move to XYZ as commanded) G38.2 Z-3.937 F6 (Probe for Z touch switch) G10 L20 Z-0.787 (Once Z touch found, move Z off of switch) (Add x,y command to fix error 33) G0 X0.2292 Y5.6942 (This is what I added) G0 Z0.185 (Go to Pierce Height) M3 S1000 (Turn on Torch) G4 P1. (Pierce delay) G1 Z0.125 F1016 (Move to cutting Height) {End Code Snippet} Seems like the post processor looses its location during probe or something is not stacking up correctly inside the Arduino during probe. Interestingly, while not exclusive to small hole sizes, it seems to happen more frequently with small holes. I am not sure what else to try - and editing the gcode for more than a few pierces is not something I look forward to I'm stumped for sure.
I'm pretty sure you will get an error due to not having a 'P' parameter in the G10 L20 command (not sure what error number it will give, as I haven't tried it). Also, the G10 L20 command doesn't move anything; it resets the current position to the coordinate(s) given in the WCS specified by the P parameter. G-Codes I would *expect* to see something like G10 L20 P1 Z-0.787 which would set the Z coordinate in G54 WCS to -0.787 at the current position. Since you haven't posted the complete gcode file, I can't tell whether you're working in inches or metric. It's possible that the controller is ignoring the malformed G10 command and interpreting the Z-0.787 as a continuation of the G0 move above which may be (trying to) send the torch beyond the travel limit and giving error 33. (Note that you need 4 decimal places in the coordinates to avoid Error 33 if you use arc commands in inch mode)
I can post the whole code, but it's what is generated by Fusion, if it's missing a command, it's a problem with the post processor - But that makes no sense either. since I'm sure many are successfully using the combination of Fusion, the open builds post processor and the Arduino This is a simple rectangular plate with 4 holes cut in it. I've made no changes to the file as generated by Fusion My Grbl settings that affect Arc are $11 0.020 and $12 0.002 Code is imperial units and in this example Pierce height and cut height are equal. but it doesn't matter, the error is always the same even if I change the relationship between the pierce height and cut height The post processor is version 1.0.38
It's probably just the G38.2 Z-3.937 F6 taking the travel out of range - have you got ~4" of travel below your probing height? ETA: You might need to reduce your probing distance as described in the last paragraph here: OpenBuilds-Fusion360-Postprocessor/README-plasma.md at master · OpenBuilds/OpenBuilds-Fusion360-Postprocessor
Thanks, I'll adjust it to something smaller, however, I have 100mm (3.937") of Z axis travel available, It should only take a few minutes to get an answer if that fixes it. Opening Fusion now I'll report back with the results from my desktop setup ( Arduino, microswitch, Laptop) If I can get it to work there it will most likely work on the actual CNC machine
FWIW- I set the Z to 2.95 " ( 75mm) Same result.. Made the change to the .cps file under user adjustments hmm...
Hopefully, this worked. I closed Openbuilds, reopened it, loaded one of the failing files zeroed x,y & z then hit run. Here's the console data Thanks for your help! [17:25:37] [ 3D Viewer ] WebGL Support found! success: this application will work optimally on this device! [17:25:37] [ websocket ] Bidirectional Websocket Interface Started Succesfully [17:25:47] [ connect ] PORT INFO: Port is now open: /dev/tty.usbmodem1401 - Attempting to detect Firmware [17:25:47] [ connect ] Checking for firmware on /dev/tty.usbmodem1401 [17:25:47] [ connect ] Detecting Firmware: Method 1 (Autoreset) [17:25:48] [ connect ] Detecting Firmware: Method 2 (Ctrl+X) [17:25:48] [ connect ] Detecting Firmware: Method 3 (others that are not supported) [17:25:48] [ ] Grbl 1.1h ['$' for help] [17:25:50] [ $$ ] $0=10 ;Step pulse time, microseconds [17:25:50] [ $$ ] $1=255 ;Step idle delay, milliseconds [17:25:50] [ $$ ] $2=0 ;Step pulse invert, mask [17:25:50] [ $$ ] $3=5 ;Step direction invert, mask [17:25:50] [ $$ ] $4=1 ;Invert step enable pin, boolean [17:25:50] [ $$ ] $5=0 ;Invert limit pins, boolean/mask [17:25:50] [ $$ ] $6=0 ;Invert probe pin, boolean [17:25:50] [ $$ ] $10=1 ;Status report options, mask [17:25:50] [ $$ ] $11=0.020 ;Junction deviation, millimeters [17:25:50] [ $$ ] $12=0.002 ;Arc tolerance, millimeters [17:25:50] [ $$ ] $13=0 ;Report in inches, boolean [17:25:50] [ $$ ] $20=0 ;Soft limits enable, boolean [17:25:50] [ $$ ] $21=0 ;Hard limits enable, boolean [17:25:50] [ $$ ] $22=0 ;Homing cycle enable, boolean (Grbl) / mask (GrblHAL) [17:25:50] [ $$ ] $23=0 ;Homing direction invert, mask [17:25:50] [ $$ ] $24=25.000 ;Homing locate feed rate, mm/min [17:25:50] [ $$ ] $25=1000.000 ;Homing search seek rate, mm/min [17:25:50] [ $$ ] $26=250 ;Homing switch debounce delay, milliseconds [17:25:50] [ $$ ] $27=2.000 ;Homing switch pull-off distance, millimeters [17:25:50] [ $$ ] $30=1000 ;Maximum spindle speed, RPM [17:25:50] [ $$ ] $31=0 ;Minimum spindle speed, RPM [17:25:50] [ $$ ] $32=0 ;Laser-mode enable, boolean [17:25:50] [ $$ ] $100=40.000 ;X-axis steps per millimeter [17:25:50] [ $$ ] $101=10.000 ;Y-axis steps per millimeter [17:25:50] [ $$ ] $102=200.000 ;Z-axis steps per millimeter [17:25:50] [ $$ ] $110=5000.000 ;X-axis maximum rate, mm/min [17:25:50] [ $$ ] $111=5000.000 ;Y-axis maximum rate, mm/min [17:25:50] [ $$ ] $112=1000.000 ;Z-axis maximum rate, mm/min [17:25:50] [ $$ ] $120=1000.000 ;X-axis acceleration, mm/sec^2 [17:25:50] [ $$ ] $121=1000.000 ;Y-axis acceleration, mm/sec^2 [17:25:50] [ $$ ] $122=1000.000 ;Z-axis acceleration, mm/sec^2 [17:25:50] [ $$ ] $130=1000.000 ;X-axis maximum travel, millimeters [17:25:50] [ $$ ] $131=1000.000 ;Y-axis maximum travel, millimeters [17:25:50] [ $$ ] $132=100.000 ;Z-axis maximum travel, millimeters [17:25:50] [ $$ ] ok [17:25:50] [ $I ] [VER:1.1h.20190825:] [17:25:50] [ $I ] [OPT:V,15,128] [17:25:50] [ $I ] ok [17:25:50] [ $G ] [GC:G0 G54 G17 G21 G90 G94 M5 M9 T0 F0 S0] [17:25:50] [ $G ] ok [17:25:51] [ connect ] Firmware Detected: grbl version 1.1h on /dev/tty.usbmodem1401 [17:25:54] [ G10 P0 L20 X0 Y0 Z0 ] ok [17:26:07] [ api ] Received new GCODE from API [17:26:07] [ api ] API called window into focus [17:26:07] [ GCODE Parser ] GCODE Preview Rendered Succesfully: Total lines: 542 / Estimated GCODE Run Time: 00h:02m [17:26:11] [ GCODE Parser ] GCODE File (from gcode editor) sent to backend [17:26:11] [ (Made in : Autodesk CAM Post Processor) ] ok [17:26:11] [ (G-Code optimized for Grbl 1.1 / BlackBox controller) ] ok [17:26:11] [ (OpenBuilds CNC : GRBL/BlackBox) ] ok [17:26:11] [ (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.38) ] ok [17:26:11] [ (Units = inch) ] ok [17:26:11] [ (Laser UseZ = false) ] ok [17:26:11] [ (Laser UsePierce = false) ] ok [17:26:11] [ (Arcs are limited to the XY plane: if you want vertical arcs then) ] ok [17:26:11] [ (edit allowedCircularPlanes in the CPS file) ] ok [17:26:11] [ (Drawing name : Y-Axis Connecting Plate v3) ] ok [17:26:11] [ (Program Name : Yaxis-Plate1) ] ok [17:26:11] [ (1 Operation ] ok [17:26:11] [ (1 : 2D Profile1) ] ok [17:26:11] [ ( Work Coordinate System : G54) ] ok [17:26:11] [ $G ] [GC:G0 G54 G17 G21 G90 G94 M5 M9 T0 F0 S0] [17:26:11] [ $G ] ok [17:26:11] [ ( Tool 3: Plasma Cutter Diam = 1.377inch) ] ok [17:26:11] [ ( Machining time : 0h:0m:40s) ] ok [17:26:11] [ G90 G94 G17 ] ok [17:26:11] [ $G ] [GC:G0 G54 G17 G21 G90 G94 M5 M9 T0 F0 S0] [17:26:11] [ $G ] ok [17:26:11] [ G20 ] ok [17:26:11] [ $G ] [GC:G0 G54 G17 G20 G90 G94 M5 M9 T0 F0 S0] [17:26:11] [ $G ] ok [17:26:11] [ (Plasma pierce height 0.14500000000000002) ] ok [17:26:11] [ (Plasma topHeight 0.06) ] ok [17:26:11] [ (Operation 1 of 1 : 2D Profile1) ] ok [17:26:11] [ G54 ] ok [17:26:11] [ $G ] [GC:G0 G54 G17 G20 G90 G94 M5 M9 T0 F0 S0] [17:26:11] [ $G ] ok [17:26:11] [ (Plasma cutting with GRBL.) ] ok [17:26:11] [ (Using torch height probe and pierce delay.) ] ok [17:26:11] [ G0 X3.9825 Y1.14 F40 ] ok [17:26:11] [ G0 X3.9825 Y1.14 Z0.725 ] ok [17:26:15] [ [ PROBE ] ] Probe Completed. [17:26:15] [ G38.2 Z-3.937 F6 ] [PRB:101.150,29.000,14.340:1] [17:26:15] [ G38.2 Z-3.937 F6 ] ok [17:26:15] [ G10 L20 Z-0.0787 ] ok [17:26:15] [ G0 Z0.15 ] ok [17:26:16] [ M3 S1000 ] ok [17:26:16] [ $G ] [GC:G0 G54 G17 G20 G90 G94 M3 M9 T0 F152 S1000] [17:26:16] [ $G ] ok [17:26:17] [ G4 P1. ] ok [17:26:17] [ G1 Z0.06 F1016 ] ok [17:26:17] [ ] error: 33 - The motion command has an invalid target. G2, G3, and G38.2 generates this error, if the arc is impossible to generate or if the probe target is the current position. [ G3 X3.8825 Y1.04 I0 J-0.1 F40 ] [17:26:17] [ ERROR ] error: 33 - The motion command has an invalid target. G2, G3, and G38.2 generates this error, if the arc is impossible to generate or if the probe target is the current position. [ G3 X3.8825 Y1.04 I0 J-0.1 F40 ] [17:26:17] [ G3 X3.8825 Y1.04 I0 J-0.1 F40 ] error:33 [17:26:21] [ ] Grbl 1.1h ['$' for help] [17:26:22] [ JOB COMPLETE ] Job completed in 00h00m [17:26:22] [ ] ok
It does look like it's the G3 command that's generating the error.... I'll have another look tomorrow.
it has to be, errror 33 only applies to arc and probe commands. please reset your $11 and $12 to the defaults, the defaults work and there is no benefit to changing them, ever. $11=0.010 ;Junction deviation, millimeters $12=0.002 ;Arc tolerance, millimeters (there is, no doubt, other code within GRBL that is tuned to work correctly with these defaults and goes wonky if they are changed, these shoudl actualyl be a compile time constant not a user adjustable value) there is nothing wrong with the gcode, however at this point in the code the plasma has just turned on. a plasma cutter is a big sparc transmitter, thery used to use them to transmit morse code before real radios were figured out (-: so, most lilkely is USB data corruption from EMI easy test is to turn the plasma cutter off at the wall and run the code.
The error occurs even when I' just have an Arduino on my desktop and a manually triggered microswitch connected to it. I eliminated the plasma cutter and stepper motors that way- ( and I did use a different USB cable and tried running it with both a Mac and a PC. Same Results - I tinkered with $11 with no change, but will try resetting $11 to 0.010 I'll also try generating a new gcode file from Fusion with just a rectangle with 3 or 4 different sized holes to see if the hole size is a contributor Thanks again for all the suggestions. If I do get this licked, I'll be sure to post the solution.
OK so this morning, I reset $11 to 0.010 and created a new design file in Fusion a 4" x 6" rectangle with a series of holes from 3/8" to 1/4" plus 1 hole 1 1/2" Set the material thickness to 0.125, Kerf width to 0.10, Pierce height to 0.12, Cut height to 0.06 Post processed the file and at this point it created a working file. So I went into the grbl settings and changed $11 to 0.02 and re ran- the gcode - Still working. Not sure what is different today, but I'll keep these settings and see if they work with other designs. Thanks again for the suggestions. I'll post back if I get another failure with both the file, and the console readings
sicne you did not post the full gcode that was not working, nor the project file from fusion, it is hard to diagnose in more depth. I can say that Fusion has defaults for some things that result in very small arcs that are related to the diameter of the tool. An example is the vertical arc that is used to enter some cuts which is defaulted to diam/10, so for a 1/16" bit that is a very small arc (radius 6 thou) and often results in error 33. While the latest postprocessor includes code to try and fix these small arcs and prevent errors, you may have stumbled on a new situation. I can diagnose it if you send me your fusion file that generates 'bad' gcode.
David, If I understand your explanation then maybe I have found the problem with one file that still was giving me an error33. Here's the file that generated gcode that errors out. And the associated gcode And the console from Open builds control (EDIT This is wrong) :I believe the error might be due to a lack of radius definition at the corner of the rectangle. I'm not actually running this on the machine at the moment, just an Arduino connected to the laptop with a microswitch that I hand actuate when I see Z moving down during probe ( no stepper motors or plasma torch to cause interference) What happens at this moment: The 3 holes are cut, then when moving to (EDIT) the outer edge to start the cut around the permitter of the rectangle I get the error 33. I'm going to try adding a radius to the corners and see if that fixes the error 33 with this design I'm a newbie at Fusion, so there are some tricks and tips I still need to learn of course... Thanks for your help!
Darn, that didn't fix it.. I still got the error33 its occurring when the move to start the outer cut finishes the probe. I have a small 0.1 lead in radius, 0 lead in distance and tolerance set to 0.01" Smoothing turned on.
OK, now I got a file that works without error33 occurring. All I did was set the lead in distance to something greater than 0, re saved the file. Then set lead in distance back to 0 saved the file and then re-ran the post and now the gcode works. There is something I'm still doing wrong, but at least I got this file to work now. I'm sure it's newbie operator error
