OMIO spindle issue

New OMIO X8 user and I am struggling with an issue that recently started to appear. The machine has been working great for a couple weeks but recently the spindle shuts down part way through a routine for no known reason. The motion controllers continue to operate but the spindle just winds down and stops, its weird. There is an error message on the controller spindle LED of E02.

Sadly, the kids were counting on my cutting gear plates for them this weekend. Any advice welcome.

Hey Mike, we were facing a similar issue. The E002 error you are seeing is caused by the spindle stalling out. We started seeing the issue during drilling operations.

If you watch the controller during the cut you’ll see the “fault” light illuminate which again we’ve learned is the Spindle is being over loaded and close to stalling. When you “fault” too long the spindle shuts down.

Without more data from your cut, I’ll say make sure your Spindle Speed is 19,000 or higher. If you go too much lower you are out of the power band of the spindle and it stalls easier. Try ramping into your cuts using a helix lead in for an adaptive. Most of the bits we use are not designed for plunging. This is when the Spindle is most likely to stall. Also make sure you are using a quality endmill. The sharper the endmill the easier time the Spindle has turning it.

If you can post what material you were cutting, the bit you were using and your speeds and feeds others might be able to help more. Also, what program you are using for CAM? That would be helpful too.

Lastly, when the Spindle stops the bit is likely breaking. If you feel like you lost your “zero” I can help you get it back so your part isn’t ruined as long as you have at least one hole to reference from.

1 Like

Yes, this sounds exactly like my problem…
here are the specs of my routine:

Solidworks with HSMworks for CAM
I have been using 2 deg ramp and helix for all my 2d pocket routines and profile cuts. I haven’t been plunging the tool on the routines that spindle stalled.

Mach 3 controller (omio software)

Cutting 6061 or 7075 (not sure) 1/4" sheet. I had spindle at 18600 with feed rate of 40 in/min and 0.025in depth of cut.
The bit is new set of 6mm carbides from amazon, it’s a Huaoa type single flute. Not the best but it gives a clean cut when new and sharp.

The last bit chipped at the tip when the spindle stalled so I tossed it out.

I’ve gotten improved at salvaging parts and in the habit of touching off the end mill at zero to leave a scribe mark to reference if I lose home.

Upate: I’ve just started a new routine and it stalled after it reached ramp depth. I rechecked the program and doc was 0.050" with feed of 65in/min cutting speed at 21000rpm.

Maybe take off the control box cover and check the spindle connections. One leg of mine wasn’t soldered correctly at the connector on the back, and caused so much electrical noise that it would stop the program.

1 Like

What is your plunge feedrate? Were you able to look at the controller while it was running? Was it giving you a “fault” light?

plunge was 15 in/min

I heard the spindle load up as it was cutting too deep and the E002 flashed on the controller as spindle stalled and slowed to a stop.

I have noticed the stalling happens towards the back end of the machine and it appears the bed slants upward from front to back such that a 0.025" depth of cut measured at 0.055" the last time it stalled. I think I need to zero my tool further back to prevent deeper cuts and or spend the time to level the bed.

@domtech, I gave the electronics a once over when I removed the cover to perform the grounding modification but didn’t give the other connections a proper vetting. Will check out and report back.

After changing my gear box toolpath to a 0.020" depth of cut, the program finished without issues, so my fingers are crossed that solves the spindle stall error.

Yeah the table level issue will definitely cause a problem. Are you using a waste board?

We laminate up two pieces of half inch PVC sheet from Home Depot and then run a .040 pass using a 1.5” surfacing bit. That way the table will be level to the machine.