So I've been using my recent DIY build inspired off the Sphinx design. Quick recap on that is dual leadscrew Y 23's using quad MGN12's. The X axis is using a belt driven 23 on openbuilds C channel with nylon wheels. The Z is a 23 powered linear rail + ballscrew combo. This moves the 500W brushless 55mm spindle which spins 12K and everything has been working pretty good. I've mainly cut aluminum so far with it and it's doing it fine enough (way better than my previous one built to mainly cut the parts for this machine). I recently tried switching to some wood projects that I wanted to give away to some co-workers. I started with a simple one for a whiskey lover by making a whiskey smoker. Seemed like an easy enough design and cut in Fusion using just 1 bit, a flat 1/4" downcut. Workflow was simple, 3 holes (concentric holes from the top) then the outer contour cut. This was all done in a 26mm white oak stair tread. All 3 holes worked and sounded good using 3mm DOC and 3600mm/min cutting rate (in hindsight this seemed a little aggressive) but they chomped away and made nice holes with clean walls and smooth bottoms. Then the bit pulled out and moved to the contour. The 2D contour on the first path used the same 3mm DOC with a 3600mm/min cutting rate. Yeah. I knew immediately things were not great by the sound. That plunged 3mm and ripped off like a F1 car losing nearly 20mm worth of steps in the middle of the 2nd half circle. This was as far as I got before smashing pause on the X32. Thinking it was to deep of a cut and to fast I ripped off a new contour only cut with 2mm then eventually 1.5mm DOC and 1600mm/min cutting rate. They both really behaved the same but I let the 1.5mm take it home. All toolpaths used left (climb) cutting so everything was moving clockwise around the material. The problem I'm still seeing is the sides (in green from the picture) cut smooth and quiet. The rounded ends in red will howl, moan and seem to chatter pretty hard. Then it hits a short straight and everything quiets down a bunch then it resumes. So my question is what could this be a result of that I should look into first. My first action I intend to look at is the X32 current to the motors. In full transparency I never touched these after setting it up. They seemed fine enough at the time since they cut aluminum OK and did not run hot. I know this would help with my lost steps initially but honestly it might have just snapped that bit in twain if the steppers didn't skip. Could the spindle just not be keeping up or bogging down? It doesn't sound like anything is happening there but it is hard to tell with the noise from the cuts. The bit is a SpeTools bit and has seen little use because it's not a metal cutting bit so it seems sharp enough and plunges and pockets the holes fine. Without going into all my Fusion CAM settings is there something obvious I might be missing here? Am I expecting to much out of this machine in a hardwood and need to treat it more like aluminum? I'm open to some thoughts and suggestions.
The red sections will be when both the Y motors and the X motor are all running together and pushing the bit that is chewing hard into the material. What power supply do you have supplying the X32? Before tweaking the pots on the motor drivers, if you can, put a volt meter across the power supply just to check that it can maintain its output voltage level when suppling enough current for when all the motors are running hard. If it is the power supply fading out, then adjusting the pots will not solve the problem, but may introduce new odd cut behaviours as higher current spikes will be drawn at other times (such as on corners etc.).
After a little extra thought, what acceleration settings do you have? That is, although when cutting the circles, both Y and X motors are also running, if the curve is tight enough, the machine will not get up to 3600mm/min as the acceleration limit will be hit at some point. If the circles you cut were smaller than this limit, then the slower forward speed will mean the steppers are running slower, and therefore have more torque available. There is also a secondary effect that with a slower cutting rate, the material removal rate is slower, reducing the cutting force needed and hence motor torque. If it is the power supply, as the circles and straight section cut ok, then the machine may be just on a 'limit' point, and a digtal multimeter may not quite capture the power fluctuations to confirm the problem. I ran into a similar issue and thought as my power supply measured ok, I went looking elsewere, only to find it was a power issue! One set of tests that may be worht a try is to rotate the piece (and gcode) by 90 degrees so that the straight section is cut when only the two Y motors are moving. The grain of the wood will also change the load on the cutter too, so by turning the wood around, there may be other changes that can highlight when the motors start to skip steps. Evan
Wow Wow thank you for the detailed responses, you have me some great points to look into. Regarding the power supply, I'm using a Meanwell 24v 360W unit so I need to test that and see if it is dropping at all. As luck would have it I snagged a deal on a 24v 600W off brand unit not to long ago in the event that is the problem. So I started playing with some settings in Fusion this weekend and found some more breadcrumbs. Using the same design I cleared 15mm of material from the top using a 2D adaptive tool path with the 3mm DOC and it did it with no fussing at all. Because this clears with concentric arcs it engaged both motors but the amount of tool head engagement would be certainly less. I'm not engineer for sure but the contour path would seem to have more cutter engagement especially in the corners. I tried to find a way to make the contour cut with that small semi circular pattern like adaptive but my several attempts in simulation didn't do what I wanted. I've got some aluminum stock setup for cuts this evening but when I switch back to wood I'll start with measuring for any voltage drop then hook my meter up in line to measure what kind of amp draw it's pulling. Again thank you for taking the time to weigh in and offer up help. My thought process hadn't gone to the PSU tapping out under the load. In hindsight it kinda makes a lot of sense since three Nema 23's are all asking for juice at that point.
Please keep the Meanwell, its appropriately spec'ed for the controller with plenty of headroom. A "bargain" 600w sounds like a cheap LED PSU with not enough filtering, ugly power up surges, and all kinds of other BlackBox damaging and warranty voiding consequences Undervoltage situations would dumped the drivers into Protection mode (See 1(g) of docs:blackbox-x32:layout [OpenBuilds Documentation]) so anyway not whats happening. Slotting always works the spindle and tool harder, and HSM strategies optimise engagement Those 500w spindles are rarely a a good choice, the armature diameter inside is far too small, and the DC magnets not strong enough. They bog down for nothing. Replacing with a RoutER11 will probably resolve all the issues: RoutER11 CNC Kit The chattering, stalls, etc are all just symptoms of the fact that the 'spindle' is a small DC motor with a collet on it
The Meanwell is a fantastic power supply, but if you have large Nema23's, or if the Nema's have a high inductance, then 360W and 24v could indeed be a factor. Yes a trochoidal milling path / Fusion adaptive clearing is much more forgiving than a simpler path that can dive full tool-width into a corner. I am not fully familiar with the BlackBox internal drivers and what they can handle, so checking the voltage on the Meanwell supply is worth doing as the first check. EDIT: Peter replied while I was typing: it looks like brownouts should be trapped, although I had an issue with a PSU (not a Meanwell) dropping out only for breif spikes, which read fine on my DVM, but was actually the problem (I am lucky enough to have an oscilloscope so could see them). As Peter says, the Meanwell is well built and is unlikely to present 'spiky' dropouts, but the voltage check is still worth a try.
I agree with peter, the combination of hardwood, 3mm doc, slotting and a downcut bit at 1/4 inch is going to be working everything hard, spindle, bit, steppers and lastly ears.. 3600mm is also quick, id be worried id break something at those speeds. vary rarley will i use a 6mm bit in my spindle, i tend to find a 4mm takes less of a toll especially on contour cuts in oak. do smokers not just catch fire?
I assumed that the straight section cut that cuts smoothly was in the X-axis that is belt driven, or is the straight cut along the Y direction where it is the leadscrews as the driving force? It is possible that one axis can handle the cut forces (as in the good straight section cuts), but the other is struggling. Both belt and screw driven axes can give excellent performance, but all drive mechanisms have their sweet-spots and limits. Is the 12k rpm the maximum speed of your spindle so that you are getting the maximum power handling? As Peter noted, you will need to squeeze it to get all it can give. Spinning a 1/4" downcut at 12k rpm and feed of 3600mm/min for a 2-tooth bit the chipload is 0.15mm/min, is within the recommended range for most 1/4" downcuts, so the feed is ok (and is a pretty similar chip load to what I use for the same scenario: my oak go-to with a 1/4" is 5000mm/min at 18krpm and 2-flute), but it then all comes down to how that translates into material removal rate with the depth of cut, and therefore forces on the machine. As the others have said, slotting with a downcut will push the machine hard, but as the machine is handling the straight cut section ok where it should have accelerated to at least as fast as when it hits the curve region, it suggests that only part of the machine is running at the limit. The cut of the straight section may only just be cutting nicely though, and could be close to getting gnarly like on the the curve if the cut was pushed only a little harder. The wood grain direction can play a big factor, especially with woods like oak. With the downcut, it is also common for the the first pass in slotting to be ok, but later passes can get tricky unless you can clear out the shavings from the slot, and when slotting down to 26mm, it is not trivial to clear out the shavings from a 1/4" slot (well, I struggle!). Going to a smaller diameter bit will reduce the material removal rate and machine load, but it can make it even harder to get the debris out of a deep slot. For a 26mm slot, the stick-out of the bit will not be short, and a thinnner bit will deflect more than the 1/4", so slower running and thinner bits usually go hand-in-hand. A strategy I have used before that may work for you is to do a first pass of all the cuts with a 1/4" downcut so that the edges of the cuts are clean, and then switch to a 1/4" upcut spiral and continue all the cuts to get to the material full depth. The upcut can handle the deep slot far more easily and also has the advantage of when it breaks through to the bottom, the lower surface fibres are also cut cleanly. It is a bit like using a compression bit, but in two passes. For the first down-cut pass, the depth of cut needs to be deep enough to make sure there is a clean-strong edge, but I suspect that trying a 1mm pass may be deep enough, and allow you to run the machine at a useful chipload and feed rate. It is usually possible to run the up-cut harder than the down-cut, but your 3600mm/min and 3mm depth may still be a too much for the corners.
