Hi all, I hope this is the right place to put my question… Last Saturday I had problems with my CNC Sphinx XL… I’m using an Arduino board with 4 Nema 23 425 Oz motors driven by 4 (Chinese) DM542 drivers, GRBL V1.1 installed on an older laptop. For the first time I was trying to mill a 2.5D part, an eagle. The roughing part was done with a 8mm flat mill with Z steps of 2mm, this without any problems. Then for the finishing part I used a 3mm ball nose bit. After milling several lines I could already see the eagle his feet’s, great it works, but then it was going wrong. The bit was running for a couple of lines strait true the material (eagle his feet’s), then he was going all the way into the right side of the material. This action has broken the bit but also the motor coupling of the X axis. With the emergency button I stopped the CNC. At the moment, I am confused about the cause and how to proceed. Until now I don’t know what exactly causes the problem, was it a failure from the computer or the hardware/software? Attach some pictures for illustration. QUESTION: Has someone had similar problems in the past and what was causes this strange behavior? I will thank you for any comment. Best regards, Benny Rosenwasser Belgium
It's hard to say. It's possible your speeds and feeds were too high and the bit grabbed the material pulling the z out of step. It's also possible your software generated a few bad lines of code or something that the controller didn't like. Or something else. Revisit your feedrates(depth of cut) for the bullnose. Run the code through a toolpath simulator and clean up any funny lines of code. Sorry and good luck. Joe.
I see no errors in the Gcode, but... I see a lot of feedrate settings of F18900 ... can your machine really do 18900mm per minute feedrate? if it cannot, then it is basically feeding at max rapid rate during the cuts, which may not be what you wanted. I cannot see your Arduino in the foto but if the gcode is correct, then we are left with electrical interference (does not look like this) or a failure to communicate all the Gcode, which IS likely with clone Arduino's. This presents sometimes as an error reported by GRBL but it can also just miss out entire lines of Gcode and result in mixing 2 unrelated lines together. The CH340 chip on clone Arduinos is the problem here.
How thick is your material? What post processer are you using? It's plunging to a full 16.7mm, which is an odd number for any material thickness.
Hi again, First of all, thank you all for your effort to look into this and of course your comments. @ David, The Arduino that I use is behind the screw shield that is on top the Arduino Uno. (screw shield only used for easier connecting of the cables) Screw Shield link: Robotale Proto Screw Shield Assembled for Arduino - Red I am pretty sure that I don’t have a Arduino clone, see picture. To avoid noise problems, I have installed opto-couplers between my limit scwitches, this works perfect. Also I has seen that the Gcode has much F18900 code. Fact is that in the X direction, the router moves fast where almost nothing should be cut, then where the Z is going up, the X movement is slowing down and so on. (See Video) I have made this Gcode with the program ArtCam, the Toolpath processor I used called “G-Code (mm)(*.tap)” See also pictures of both Toolpath settings. The material thickness is 28mm. Today I installed my new coupling ordered at Ooznest. To test, I have been running the same Gcode (for 3mm ball nose) in the air, this means without running the router. I have not been able to discover any irregularities. Regards, Benny
From the pictures, I noticed how low you have the router. Raise it up a bit. This way, the end mill can clear the bottom of the gantry. I'd raise it up by at least 2.5 inches. You will also notice how much easier (and safer) it is to change tools. Now for the problem. I think I get it. If your material thickness is 28mm, but you have the depth set to 16mm, I'm assuming that you are using half thickness as z zero. That would be an additional 2mm above and below the stock which is why it's plunging so deep. It may not plunge to full depth on a roughing pass, but a finishing will do it.
indeed, not a clone. (I could see where it was, but i could not see the chips on it!) However, depending on how old it is you may still have a problem since the actual USB firmware was a problem. Known Bugs · grbl/grbl Wiki · GitHub down the bottom of the page.... so is 18900mm/min related to any of your settings? That software appears to use mm/s for the rate settings, and I see 105 for the finishing stuff. That is 6300mm/min (Gcode is in mm/min!) I see F2520.0 which is 42mm/s which is your plunge rate. but no F6300 anywhere what this means is that it is trying to cut at maximum speed, which probably wont hurt in wood but might be a real problem in aluminum. no problem there, plunging to -16.x is quite normal here, since the top of the material is Z=0, right? [/QUOTE] To test, I have been running the same Gcode (for 3mm ball nose) in the air, this means without running the router. I have not been able to discover any irregularities. [/QUOTE] this indicates that the problem was temporary/random, maybe your cellphone rang near the machine? (-:
I have doing home research and have bought the Arduino R3 in 2013 The chip on it is a “atmega16u2” Driver Version 1.2.3.0 VID 2341 PID 0043 R1 To be absolutely sure, after resetting the chip, with the JRE-FLIP installer, I flashed the latest firmware “Arduino-usbserial-uno.hex” on it. (not without any problems, the FLIP program couldn't find the USB port and spoked following Error: "AtLibUsbDfu.dll not found" … to fix this I did what this man said OK, thank you for the explanation, but I cannot find any setting that I have made which is related to the 18900mm/min. In ArtCam you can optimize feed rates of toolpaths, I’m almost sure that this action has written the F18900 in the Gcode See explanation here Right ! I hope this behavior will not come back, it make me a little nervous to work with this machine…. :-( @ Kevon, I understand your concern My CNC has Sphinx-XL side plates which are a little bit taller than the original design of Mr. Kyo. When I do engraving work of thin materials, the router must go down all the way to catch the material. (thickness of 3-4 mm). At the moment, I don’t have problems to safely change the bits. Thanks to all for your input. Regards, Benny
What you should do is make a platform to mount on the table that takes up space when you are doing thin materials. This way the Z does not have to come down so far. This means you can move the router up on the mounting and use 2 mounting rings for a lot more stiffness.
OK Kevon, David, I understand now what you mean, and you’re right, Stiffnes is important, I will see what I can do. Thanks a lot, Benny
This is just to help reinforce the idea. This is with a 2.5" end mill. My bed is raised by 40mm and uses a ~10mm spoiler. In fact, 3/8" (10mm) stock only has less than 10mm clearance to the bottom of the z axis. This is with the short plates. I pretty much only cut aluminum. To be honest, I kind of misinterpreted the actual issue at first. Like was said before, your machine is trying to fun at (probably 5x) it's max speed. It's possible that it is freaking out. Have you trying slowing it down? Try 1500mm/min instead of 19k. Have you tried recreating the gcode?
In fact I did, see file attached. I lowered the feed rate from 105 to 42, the plunge rate from 42 to 10.
