So I’ve been running into an issue I think is caused by some type of EMI. At least that’s what I’ve been reading based on other posts. I’ve been getting weird stops during probing, running a job, and occasionally during jogging/ homing. No way to replicate it but it seems to do it mostly while running a job. It does it when it’s controlled by pc Control software and the Interface controller. So my question is, how do you track it down or figure out where it’s coming from? I ordered some emi snap on barrel style filters, I just need figure out where to put them. thanks.
Is the power cable running in the same drag chain as your stepper motors and limit switch wires? If so, separate them. Do you run dust collection in plastic ungrounded pipes? The static can cause problems.
The power cord is in the same drag chain for the router, z axis and Z endstop yes. I tested it with the router unplugged. And it still did it. I forgot to mention I do have my chassis directly grounded to the ground on the 24v power supply. Tested it with a multimeter. The ground is continuous throughout the entire machine. All the way to the router collet. Not sure if that makes a difference. No dust collection being used.
I am using homing limit switches. But just ones I ordered from Amazon. They don’t have any filtering. What type of filter, and can I add filtering to those?
Easy way is get the Xtension switches. For a fun project using your existing CNC, order the parts from the parts list and machine your own board. I did one years ago before there was a Blackbox or Xtension switches. But, I bet the individual components would cost more. Or just use resistors and capacitors. Wiring Limit Switches · gnea/grbl Wiki
You could also disable your homing switches and disconnect them from your controller. Then you can fake your home position. How to 'Fake the home' If you have no issues cutting the same project, I would guess your switches are the problem.
See our comprehensive guide here: docs:blackbox:faq-emi [OpenBuilds Documentation] Also personal opinion is the low quality amazon switches. Might not be EMI, might just be switches so bad that they make contact from slight vibration - seen that before
Thanks guys! I tried it again today. After homing, I disconnected the endstops and tried running a program with the router turned off and unplugged. I’m still getting freezes. It seems to be roughly around the same spot though. I checked the code and I don’t see any errors. The code was generated from fusion 360 using the grbl format. I tried again with the interface controller and pc. On the pc I got this error.
I did some more testing with some of the grbl settings. If I disable soft limits, it runs the program just fine! It finishes with no errors. But when I go to home, it tries to go past and crashes. I verified my travel limits and they are correct. I am able to manually jog down past where It is erroring. So this all leads me to believe it’s not an EMI issu. Instead it’s something with the software or configuration.
The error states the issue. Your Job is larger than what you configured Grbl to tell it how large your machine is. Either reCAM so the job fits on your machine, or make sure you properly configured Max Travel in Grbl Settings Crashing into the limit switch during homing = wiring. Use the Troubleshooting tab to test each switch, make sure you didn't cross any axes either (Z switch plugged into X?)
Thanks Peter. Actually in grbl, my limits are very large. The machine is 33”x14”x10”. Approx. I have the correct settings in grbl, as I am able to jog the machine to the full limits. The code I’m testing with is a simple 1/2” diameter bore 1/2” deep. as for the wiring on the limit switch’s. It will home perfectly with soft limits set. It also homes with hard limits set. It only crashes when using hard limits after the job is done. I know. It makes no sense. I’m pulling my hair out here.
Soft Limits is a well working principle. You home to set the machine coordinates. Your Max Travel values tells Grbl the safe envelope inside those coordinates. Soft limits stops any move that wants to violate that safe space by exceeding max travel on either end. If it "gets in the way" you either didn't home, have homing setup incorrectly, have incorrect values in Max Travel, or really did CAM up a job larger than that safe movable envelope. No other options exist
Lol, What you said makes complete sense! Except it’s not working…. I have had this machine for years. The limits are set correctly as I am able to jog the entire machine size after I home. I can’t jog without homing first. When homing, it does the z axis first then the other two at the same time. Then does a re-home to validate its position. As part of my cam job, I had to drill 6 holes around the center bore. That worked perfectly at the correct scale, and in the correct position. These holes are spaced outside the center bore so I know for a fact, it will travel that far. My second operation Involved a tool change and then a z probe. Then it ran an adaptive circular path and that’s where I started to have it freeze approx 90% through the job. I tested this several times. And it seemed to stop in the same spot. I proceeded to the next job which is the 1/2” bore. I get the same thing. Freezing toward then end. I’ve gone back into fusion and made a new path from scratch. Exported a new file, and I get the same thing. like I said, it makes no sense! It’s not like it’s a brand new machine, nor am I a rookie when it comes to cnc jobs. I’ve been doing this for a while now so I know what to look for. I just can’t figure this one out.
I just ran it again with the interface controller. Here is a screen shot of the work, You can see the 1/2” bore in the middle. I ran the job and it stopped before it got to the bottom. I took another image with the interface error. It says press ok or cancel, but the ok button does not work.
Yes firmware is up to date. When I started it up two days ago it automatically did a firmware update. Unless it has changed since then? I'm wondering if my controller (Arduino Uno) has finally bit the dust? I'm currently using Stepper drivers TB6600 (Amazon) rated at 4 amps to control Nema 23 motors. If I ordered a Black Box controller, Would that be comparable to the individual stepper drivers? I noticed the 4 wire conductors you sell are not shielded. Do you sell a shielded version? Also, I might as well order some of the endstops while I'm at it. especially if I have to do a complete rewire. Lastly, are the black box controllers shipping right away? Thanks!
It would be better than TB6600s No need for shielded stepper motor wiring, see docs:blackbox:faq-emi [OpenBuilds Documentation] - stepper motors generate a lot less interference than mains cables and spindles Yes, proper filtered switches makes a huge difference to false endstop alarms. Pretty sure they do, but as always, store questions are better directed at the Store team directly via Support - forum is a different team Looking at your error again, the Soft limit was triggered just before an M30 - make sure your Post Options are correct as well, typing positive values into start/end positions for example would also violate soft limits (Machine coordinates is entirely negative quadrant) - the closeness of an M30 makes it seem like this is near the end just before a Z-safe move
Interesting! I was using the standard GRBL Post processor in Fusion 360. Can I use the Black box version on an Arduino Uno controller? I setup Fusion like the instructions said. I get an error now though. It seems it defaulted the Machine WCS offset to 0. If I change it to 1, it seems to post process ok. I will have to try out the new code when I get home tonight. I'll let you know if this fixes it. THANKS!
Yes, we fixed the "bugs" fusion doesn't care to fix - superior post all round Remember to set your WCS Offset in the Setup tab: How to define Work Coordinate Systems in Fusion 360 Manufacture | Fusion 360 | Autodesk Knowledge Network - to tell the post in which coordinate system to work Make sure those start/end positions are NEGATIVE numbers - no G53GxZ+ moves, only G53GxZ-
Yes you can - the "error" message you were getting was just telling you that you hadn't selected a wcs in Fusion cam, and it was going to use the first one (G54). The Openbuilds post processor allows you to select the wcs of your choice - useful if you have fixed positions for certain jobs. Alex.
It looks like the Black box processor did produce negative Z number for G53. Below is the gcode for the 1/2" bore operation. Do you see anything that looks incorrect? -ignore spindle speed. I use a router. I'll have a look at the pervious Code when I get home to compare. Its on the USB in the interface, so I can't look at it right now. Thanks again! (Made in : Autodesk CAM Post Processor) (G-Code optimized for Grbl 1.1 / BlackBox controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.28) (Units = inch) (Drawing name : Sprockets v33) (Program Name : Bore 1-2) (1 Operation in 1 files.) (File List ( Bore 1-2.gcode) (This is file: 1 of 1) (This file contains the following operations: ) (1 : Bore3 3) ( Work Coordinate System : G54) ( Tool 1: Flat End Mill 4 Flutes, Diam = 0.25inch, Len = 0.75inch) ( Spindle : RPM = 5000) ( Machining time : 13 sec) G90 G94 G17 G20 (Operation 1 of 1 : Bore3 3) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-0.3937 G0 X5.9587 Y9.553 S5000 M3 G4 P1.8 G0 X5.9587 Y9.553 Z0.6 Z-0.0234 G1 X5.9587 Y9.553 Z-0.0784 F40 X5.9575 Y9.553 Z-0.0861 X5.9539 Y9.553 Z-0.0931 X5.9484 Y9.553 Z-0.0986 X5.9414 Y9.553 Z-0.1022 X5.9337 Y9.553 Z-0.1034 X5.9212 Y9.553 X5.9135 Y9.5518 X5.9065 Y9.5482 X5.901 Y9.5427 X5.8974 Y9.5357 X5.8962 Y9.528 G3 X6.1462 Y9.528 Z-0.1231 I0.125 J0 X5.8962 Y9.528 Z-0.1428 I-0.125 J0 X6.1462 Y9.528 Z-0.1625 I0.125 J0 X5.8962 Y9.528 Z-0.1822 I-0.125 J0 X6.1462 Y9.528 Z-0.2018 I0.125 J0 X5.8962 Y9.528 Z-0.2215 I-0.125 J0 X6.1462 Y9.528 Z-0.2412 I0.125 J0 X5.8962 Y9.528 Z-0.2609 I-0.125 J0 X6.1462 Y9.528 Z-0.2806 I0.125 J0 X5.8962 Y9.528 Z-0.3003 I-0.125 J0 X6.1462 Y9.528 Z-0.32 I0.125 J0 X5.8962 Y9.528 Z-0.3396 I-0.125 J0 X6.1462 Y9.528 Z-0.3593 I0.125 J0 X5.8962 Y9.528 Z-0.379 I-0.125 J0 X6.1462 Y9.528 Z-0.3987 I0.125 J0 X5.8962 Y9.528 Z-0.4184 I-0.125 J0 X6.1462 Y9.528 Z-0.4381 I0.125 J0 X5.8962 Y9.528 Z-0.4578 I-0.125 J0 X6.1462 Y9.528 Z-0.4774 I0.125 J0 X5.8962 Y9.528 Z-0.4971 I-0.125 J0 X5.9091 Y9.4726 Z-0.5 I0.125 J0 X6.1332 Y9.5834 I0.112 J0.0554 X5.9091 Y9.4726 I-0.112 J-0.0554 G1 X5.9137 Y9.4662 X5.9199 Y9.4615 X5.9274 Y9.459 X5.9352 Y9.4589 X5.9426 Y9.4613 X5.9538 Y9.4668 X5.9608 Y9.4702 Z-0.4988 X5.967 Y9.4733 Z-0.4952 X5.972 Y9.4758 Z-0.4897 X5.9752 Y9.4773 Z-0.4827 X5.9763 Y9.4779 Z-0.475 G0 Z0.6 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-0.3937 M5 G0 X-0.3937 Y-0.3937 M30
True, the default post also uses G28 just to further confuse you - despite homing you also would've had to check where G28 is. No worries, our post does it better and just uses G53 and G54-59 depending on which WCS you setup of course)
I have some good news!!!! it seems to be working now. At least it is finishing the jobs like it supposed to. I did have a problem with probing all three axis at once. It would only allow me to do one at a time. Not sure if that's EMI or not. But at least its a step in the right direction. Really glad I didn't have to buy a new controller. Thanks for the awesome help you guys!!!! Much appreciated! Just for reference, here is the Gcode from Yesterday where it locked up on me using the grbl post processor from Fusion 360. It uses G28 but also Z0. (1001) (T1 D=0.25 CR=0 - ZMIN=-0.5 - flat end mill) G90 G94 G17 G20 G28 G91 Z0 G90 (Bore3) T1 S5000 M3 G54 G0 X2.5341 Y9.6431 Z0.6 Z-0.0234 G1 Z-0.0784 F40 G18 G3 X2.5091 Z-0.1034 I-0.025 K0 G1 X2.4966 G17 G3 X2.4716 Y9.6181 I0 J-0.025 X2.7216 Y9.6181 Z-0.1231 I0.125 J0 X2.4716 Y9.6181 Z-0.1428 I-0.125 J0 X2.7216 Y9.6181 Z-0.1625 I0.125 J0 X2.4716 Y9.6181 Z-0.1822 I-0.125 J0 X2.7216 Y9.6181 Z-0.2018 I0.125 J0 X2.4716 Y9.6181 Z-0.2215 I-0.125 J0 X2.7216 Y9.6181 Z-0.2412 I0.125 J0 X2.4716 Y9.6181 Z-0.2609 I-0.125 J0 X2.7216 Y9.6181 Z-0.2806 I0.125 J0 X2.4716 Y9.6181 Z-0.3003 I-0.125 J0 X2.7216 Y9.6181 Z-0.32 I0.125 J0 X2.4716 Y9.6181 Z-0.3396 I-0.125 J0 X2.7216 Y9.6181 Z-0.3593 I0.125 J0 X2.4716 Y9.6181 Z-0.379 I-0.125 J0 X2.7216 Y9.6181 Z-0.3987 I0.125 J0 X2.4716 Y9.6181 Z-0.4184 I-0.125 J0 X2.7216 Y9.6181 Z-0.4381 I0.125 J0 X2.4716 Y9.6181 Z-0.4578 I-0.125 J0 X2.7216 Y9.6181 Z-0.4774 I0.125 J0 X2.4716 Y9.6181 Z-0.4971 I-0.125 J0 X2.4845 Y9.5627 Z-0.5 I0.125 J0 X2.7086 Y9.6735 I0.112 J0.0554 X2.4845 Y9.5627 I-0.112 J-0.0554 X2.518 Y9.5514 I0.0224 J0.0111 G1 X2.5292 Y9.5569 X2.5328 Y9.5586 Z-0.4997 X2.5362 Y9.5603 Z-0.4988 X2.5394 Y9.5619 Z-0.4973 X2.5424 Y9.5634 Z-0.4952 X2.5451 Y9.5648 Z-0.4927 X2.5474 Y9.5659 Z-0.4897 X2.5492 Y9.5668 Z-0.4863 X2.5506 Y9.5675 Z-0.4827 X2.5514 Y9.5679 Z-0.4789 X2.5517 Y9.568 Z-0.475 G0 Z0.6 G28 G91 Z0 G90 G28 G91 X0 Y0 G90 M5 M30
