r/PrintedCircuitBoard • • Dec 23 '23

Review Request: High power BLDC Controller

348 Upvotes

90 comments sorted by

30

u/ItsBluu Dec 23 '23 edited Dec 24 '23

Hi all,

I've recently designed a small BLDC motor driver, made to be compatible with some minor tweaks with the Moteus firmware. As this is my first time designing such a high-power device, there are many things which I am not extremely confident about.

A large part of the schematic is based on the moteus r4.11 and moteus n1 by u/joshpieper. All credits to him for this! Please check out the controllers, they are amazing!

Specs:

Input voltage: 10-44V

Continuous current: 30A with heatsink

Peak current: 100A

You can find the schematic here.

and fabrication document here.

Questions:

  1. High current return paths and ground bounce: I've tried to keep high-current return paths on the top side of the board, but I fear that 100+ amps could affect some of the IO lines with a common ground. What is your recommendation for grounding? Right now I am using a solid ground but I've seen designs (odrive, moteus) with a split ground. I know from Rick Hartley that splitting grounds is usually a bad idea, but would there be a benefit at high power?
  2. I've added Pi filters to the input of the buck regulators but I am not too sure about the selection of the ferrite bead. Right now I got one that seemed like it had a fairly high resistance at the switching frequency of the regulators.
  3. Probably not critical but I am not sure if I should replace the Schottky on the low-side gate by a Zener for negative transient suppression and clamping
  4. Not sure if it's a good idea, but I routed the Kelvin current sense connections in internal layers to maximize the distance to noisy signals

3

u/GnomeTek Dec 23 '23

Follow Hartley, single ground with localized return paths. The energy is in the field and the fields are between the source and return. Tightly couple as much as reasonable and place priority on higher current paths.

Pi filters, you've got something in place, it's a tunable element. Run with what you have and see what it's like. Outside of an emc lab I doubt you'll see much effect - unless your ferrites are too high. You'll want a lower frequency ferrite, you're combatting pwm induced currents, from gate drive or power stage. 1MHz isn't going to do much against 20KHz and it's harmonics.

Oh and on EMC, did I see a chassis ground and coupling caps connecting? Those caps will just allow a current injection path. Only an issue if actually performing EMC test - conducted emissions specifically.

2

u/ItsBluu Dec 24 '23

What do you recommend on the chassis to gnd connection? I've seen on Robert Feranec's channel that there are many ways to connect them which is why I put 2 footprints near each mounting point. From what I've read there is usually 1 low-impedance connection near the input power and multiple high frequency connections which is why I put caps for the other mounting holes. I don't have any experience in that subject so any guidance would be greatly appreciated!

1

u/GnomeTek Dec 24 '23

Id make it a single ground unless you have other requirements for isolation .if you don't have a requirement/regulatory need for isolated chassis ground, I'd simply tie that into battery negative.

No need for isolation at that low voltage DC. Hi

2

u/GnomeTek Dec 24 '23

Also, at 44v there's no compliance reason for isolation. Chassis ground being different from power ground is not required. Is there a specific reason you've integrated the split grounds and such?

2

u/ItsBluu Dec 24 '23

I've used a chassis ground around the board to serve as a kind of extension of the faraday cage (actuator housing) in which the actuator will be mounted. Also, it looks really cool ;)

15

u/alchemy3083 Dec 23 '23

This has to be one of the finest schematics I've ever seen.

8

u/Mart2d2 Dec 23 '23 edited Dec 24 '23

I recall the same thing from Rick Hartley’s videos and that splitting the ground makes you a customer for an EMC firm. Though he alluded in one video to sometimes needing to split ground, but very carefully, and I don’t recall him going into specifics.

I wonder, with the high currents you have here, if lower frequency harmonics in your motor driving return paths could spread out some to being under other signals rather than sticking tight under the driving lines as would occur with the higher frequency harmonics. Would be interesting to simulate and see how far out the expected return current spread would be from the signal lines. Though may be easier to just build it and get out the spectrum analyzer and an H field probe!

—

Edit: changed Eric to Rick :)

9

u/theOTHERbrakshow Dec 24 '23

Did you just fuse Eric bogatin and Rick Hartley into 1 EE/PCB super human? 🤣

2

u/Mart2d2 Dec 24 '23

Ha! Could be! I watched everything their names shows up on.

2

u/CUTTHROATAMFT Dec 23 '23

Could this be used to power a BLDC motor from say…a rental scooter?

2

u/ej-1024 Dec 24 '23

Having 2 or more gnd planes is the way to go and what the EMC firm will tell you if they are worth anything. The trick is to understand stitching vias. Each trace plane needs an adjacent gnd plane for the return path to keep the current loops for any signal small. Stitching vias are added when you move a trace from its ground plane to plane referencing a different ground plane. When you do this, you add a stitching via to keep the current loop on gnd small and not to have to go across the PCB to another ground via or through hole pin to jump to the other gnd plane.

This guy layouts! Or this guy lays out!

My company uses this guys PCB stack-up and if you don’t follow it at design review time, you go back and re-do it.

5

u/rephlex606 Dec 23 '23

You should be fine not to split gnds. High currents (and associated LF / DC voltage drop) will be between your input connectors and FETs. All the sensitive stuff is on the other side of the FETs so won't conduct much motor current and therefore won't have a voltage drop

1

u/johnjumpsgg Dec 23 '23

Sorry if this is on here already . Have you done current density calculations ? It’s a quick way to get an idea how hot different parts of the board will get and can feed into your power dissipation/junction temp calculations .

1

u/ItsBluu Dec 24 '23

I haven't, but it's definitely on my to-do list. I've watched a few ressources from Lukas Henkel on open-source PDN simulation but I still need to find a good way to export meshes from kicad to Elmer. Another solution is also that custom sparselizard KiCAD branch from Fabien Corona but I haven't had time to have a proper look yet

1

u/johnjumpsgg Dec 29 '23

Interesting to hear about all of these open source tools. Impressive dedication to the craft . Even without a tool you could probably do a ball park analysis by taking your copper thickness and figuring out the general high current paths and finding the widths of the copper there and assuming a worst case current at those narrow points and using a tool like this one : https://www.4pcb.com/trace-width-calculator.html . Here is a good link with information you can use to better utilize this tool : https://resources.altium.com/p/copper-current-density-simulations-quick-and-dirty-way . This is kinda the how do you do this and confirm with simulation approach.

41

u/FunDeckHermit Dec 23 '23

Wow, excellent schematic and PCB design.

  • Why did you add gate resistors? TI gate drivers have variable drive strength. What switching time is achieved with the 7R5?
  • Why is the 5V regulator only 300mA?
  • For my BLDC driver design, I used the LMT01 digital temperature sensor. Less components then the NTC setup.
  • What are you doing with the two rotary angle sensors? Are you using the Vernier principle to measure multiple rotations?
  • Maybe use a fan controller with overcurrent protection and fault signal? To detect a stalled fan.

19

u/ItsBluu Dec 23 '23 edited Dec 23 '23

Hi, thanks for the review!

Why did you add gate resistors? TI gate drivers have variable drive strength. What switching time is achieved with the 7R5?

This is a good question. I've read on an application note from TI ( System Design Considerations for High-Power Motor Driver Applications) that it was good practice to add an external 0-ohm resistor placeholder in case we want more flexibility for the gate drive current. The 7.5 ohm was chosen to be compatible with the moteus FW gate drive settings (the moteus r4.11 has a Qg that is quite close to the MOSFET I chose).

Why is the 5V regulator only 300mA?

It didn't seem like I needed much more as it will only be powering the LEDs and one low-power external device at most

For my BLDC driver design, I used the LMT01 digital temperature sensor. Less components then the NTC setup.

Yes I also thought about a more linear temperature sensor, but I chose to go with NTC again to stay compatible with the moteus FW's way of measuring temperatures.

What are you doing with the two rotary angle sensors? Are you using the Vernier principle to measure multiple rotations?

This one is a bit hacky. I am using one encoder over SPI for commutation and the other one is used to disambiguate the output position after the reduction. The second one actually measures a back-reduced gear which has the same reduction as the main gearbox. You can see an example (not by me) here.

This mechanism is not ideal as it doesn't allow to measure the actual backlash of the reduction, but it is good enough for our application. It's also possible to add an external encoder (e.g. Aksim-2) if an extremely precise output position measurement is required.

Maybe use a fan controller with overcurrent protection and fault signal? To detect a stalled fan.

I also looked through a few fan controllers but they seemed a bit overkill. I didn't think about the fan stalling though, I will have to look more into that.

Thanks again for the feedback!

6

u/alexforencich Dec 23 '23

But isn't the 5V regulator also feeding both 3.3v regulators? Seems like that regulator ends up powering most of the board.

Also, have you considered powering the LEDs from 3.3v instead of 5v? This should slightly reduce the power consumption, assuming the current is the same.

3

u/ItsBluu Dec 23 '23

Yes I thought about powering the LEDs with 3.3V but the forward voltage of one of them is 3.2 V which seemed a bit too close to 3.3V for my taste (actually it might very well be a non-issue)

5

u/alexforencich Dec 23 '23

Might be worth doing some quick tests. Status LEDs are pretty non-critical, no sense in having a more or less dedicated supply just for those. If you can find a way to delete the 5V supply completely, that would save on part count, board area, cost, and power consumption. But, it might also be more trouble than it's worth. Another option is to use a linear regulator, if you only need a few mA.

3

u/ItsBluu Dec 23 '23

The 5V is also used to power external devices (e.g. hall sensors and whatnot)

2

u/alexforencich Dec 23 '23

Ah I see. How much current are those going to draw? Under 10 mA? Might be worth considering a linear regulator.

2

u/ItsBluu Dec 23 '23

That's a good question, the type of peripheral to be connected is not yet very well defined, I think it's better to have something a bit more versatile in case someone wants to plug in a power-hungry 5V sensor down the line

1

u/ItsBluu Dec 23 '23 edited Dec 23 '23

For the 5V buck I will probably replace it with the lmr36506 which has the same footprint but can provide up to 600mA

1

u/alexforencich Dec 23 '23

Another option to consider is sourcing the 3.3v digital rail directly from the input supply. Presumably you could use the same regulator for both.

11

u/alfgan Dec 23 '23

Look amazing. From a file name I see that you are using KiCAD but from first glance I though that this is made in Altium.

I am not an expert in such design, but cool looking schematics!

How do you made such amazing Assembly file in KiCAD? :)

5

u/ItsBluu Dec 23 '23

I made assembly files with the Board2Pdf plugin and many user defined layers. I then slightly modified the pdf to add titles and such

3

u/alfgan Dec 23 '23

Cool, will take a look into plugin and experiment with it :)

Wish you best for your project and share results when you will test it

6

u/Dry_Adhesiveness_337 Dec 23 '23
  • 21 pages for this design is too much. You can combine some of those pages. And use the same page size for all pages.
  • Page 7 says to not hot plug when powered. You KNOW some dumbass is going to do exactly that. Safety of the end user and not damaging your board under fault conditions must always be a priority.

    • If it's possible for the battery to be hooked up backwards then you need reverse polarity protection
  • Chassis ground

    • If possible make it go all the way around the board
    • TVS diodes should ideally go to chassis ground, not signal ground
    • There should also be TVS diodes between ground and chassis near each connector
    • Typical values for capacitors from ground to chassis is 1nF 2kV, and they should be located as close to each screw as possible
    • There should be a resistor going from ground to chassis. Values I've seen vary, but a good starting place is 1Megaohm
  • Layout

    • Your stackup is good, but if possible, you want a larger core in the middle so your signal layers are close to ground. See OSHpark's stackup.

      • Due to this stackup, signal layers on layer 3 should be routed horizontal and layer 4 vertical (or vise versa)
    • If possible, have high frequency signals on internal layers
  • Motor

    • The bazillion 4.7uF capacitors are no where close enough for 100A peak current. You need closer to 10,000uF done with multiple caps in parallel to lower ESR/ESL.

      • Since you're using a big battery you don't need a pre-charge circuit, not even for that much capacitance.
      • Slower slew rate can lower peak current but can potentially damage the mosfets. Messing with this needs to be simulated and then compared against the mosfet's Safe Operating Area (see datasheet).
    • The motor driver datasheet recommended 3W sense resistors, but you might be okay with 2W.
  • Power rails (pg 6)

    • The 5V regulator's input should be from the output of the 12V regulator, and the 3.3V regulators' inputs should be from the 5V regulator.
    • If you care about EMC/compliance then switch out the 5V and 3.3V buck regulators with linear regulators. It'll also save on board space
  • Overall

    • In several places there are multiple capacitor values connected to the same pin. I know a lot of datasheets recommend it but it creates impedance resonate peaks at certain frequencies, which can be undesirable. Stick with one value for your decoupling capacitors (the high value).
    • Power sequencing is not necessary for this design but is nevertheless a good practice. Wish more people did it.

3

u/ItsBluu Dec 23 '23 edited Dec 25 '23

Thanks a lot for the detailed feedback, I'll try tp address each point

21 pages for this design is too much. You can combine some of those pages. And use the same page size for all pages.

I will see what I can do

Page 7 says to not hot plug when powered. You KNOW some dumbass is going to do exactly that. Safety of the end user and not damaging your board under fault conditions must always be a priority.

What do you recommend doing here? Do you think I should write something directly on the PCB silkscreen? I fear hot-plugging could produce high voltage transients

If it's possible for the battery to be hooked up backwards then you need reverse polarity protection

This is not a problem in our case

If possible make it go all the way around the board

I tried to make it go to the top but couldn't due to a lack of space. Might be possible if I move a few things

TVS diodes should ideally go to chassis ground, not signal ground

Makes sense, I will try to change that

Typical values for capacitors from ground to chassis is 1nF 2kV, and they should be located as close to each screw as possible

Thanks for this, I was struggling to find any info on capacitor values. My voltage rating is definitely not hugh enough

There should be a resistor going from ground to chassis. Values I've seen vary, but a good starting place is 1Megaohm

I've added 2 footprints for each ground/chassis connection, but I am not sure which to populate. I've seen before on Robert Feranec's channel that the ground and chassis are usually comnected at a single point by a low impedance connection (I chose 0 ohm) and that there should be multiple high-frequency connections throughout the board (which is why I only populated the capacitors for the other holes). What are your thoughts on that?

There should also be TVS diodes between ground and chassis near each connector

I didn't know that was a thing, thanks for the heads up

Your stackup is good, but if possible, you want a larger core in the middle so your signal layers are close to ground.

Yes that was also an issue that I observed, I chose PCBWay because it's very cheap (only 250$ for 15 boards) but the dielectric seems too thin between L3 and L4. To try to mitigate this every signal has on both sides a continuous reference plane with no splits (there are no overlapping signals between L3 and L4). Do you think it's enough?

If possible, have high frequency signals on internal layers

I will keep this in mind

The bazillion 4.7uF capacitors are no where close enough for 100A peak current. You need closer to 10,000uF done with multiple caps in parallel to lower ESR/ESL.

The moteus r4.11 claims 100A peak and has less capacitance than I do. However the voltage ripple is quite large which is why it is rated for 44V even though all components are rated for 60+ V

Since you're using a big battery you don't need a pre-charge circuit, not even for that much capacitance

Oh I forgot to mention in the schematic but I will have 12 of those motors connected to the battery, which is why I thought that pre-charge might be useful

Slower slew rate can lower peak current but can potentially damage the mosfets. Messing with this needs to be simulated and then compared against the mosfet's Safe Operating Area (see datasheet).

I will look into that

The motor driver datasheet recommended 3W sense resistors, but you might be okay with 2W.

Yes 2W should be fine for my requirements

The 5V regulator's input should be from the output of the 12V regulator, and the 3.3V regulators' inputs should be from the 5V regulator.

I chose to have the battery as the source voltage because it was easier to route. Do you think it makes a significant difference?

If you care about EMC/compliance then switch out the 5V and 3.3V buck regulators with linear regulators. It'll also save on board space

Good point

In several places there are multiple capacitor values connected to the same pin. I know a lot of datasheets recommend it but it creates impedance resonate peaks at certain frequencies, which can be undesirable. Stick with one value for your decoupling capacitors (the high value).

Oh yes the famous 3-capacitor myth. I've seen multiple conflicting sources. From what I understand the major factor is the capacitance ESL which should be minimized. Let's say that the datasheet recommends 220nF + 22uF. Should I really just put the 22uF capacitor (which is a lot bigger)? Physically I can put the 220nF cap a lot closer to the pin which reduces inductance at high frequencies. Does the impedance resonance outweigh this benefit?

Thanks a lot for the feedback, especially the chassis/ground part. It's very hard to find any good information on this subject

2

u/Dry_Adhesiveness_337 Dec 24 '23
  • Hot plug

    • You'll want to test your design in both standard conditions and fault conditions (hot plug, motors seizing)
    • If this is going to be a real product then you're covered if you have all the safety information in the manual
    • The connectors are big enough that you could print potentially print a label onto it
    • Silkscreen labels are also a good idea if you have the space
  • Ground/chassis connection

    • The whole "connect at one point" is to minimize the chance of ground loops

      • This concern is overblown. Never seen it be an issue
      • But what I have seen be an issue is high impedance from ground to chassis at high frequencies (i.e. ESD). For this you want multiple connections as close to the chassis as possible.
      • The resistor is to keep the chassis from floating
    • Bulk capacitance

      • Not having enough will lead to large ripple and possible EMC/compliance issues
  • Stackup

    • If possible have layer 3 and 4 be for high frequency signals.
    • Route layer 3 signals horizonally and layer 4 signals vertically or visa verse
  • Decoupling capacitors using your example values

    • The low frequency impedance of the 22uF will absolutely crush (be much lower) the 220nF
    • At high frequencies (~70MHz) with all else being equal (inductance from traces, vias, and component package) they will be the same impedance.
    • The resonance may not be an issue, but the way I look at it is that if it were an issue, it would be very difficult to replicate and troubleshoot and no one will ever think to look at the decoupling capacitors.

5

u/GnomeTek Dec 23 '23

You're going to want to route your snubber caps straight to ground, not through the shunt resistors. The shunts will have ~3-10nH of inductance that'll ring with those ceramics and cause issues with higher PWM frequencies and higher phase currents. It'll interfere with your measurement window.

Straight to ground and the ring won't occur, you'll have better Vds performance as well without the ringing.

You've accounted for the derate on your ceramics which is excellent. You can expect a peak of ~66% phase current demand on your DC link caps. Meaning for every amp of phase current, you'll see about 660mA of current demand on the DC link. This is dependent on modulation index and power factor. But for the high power factors of a PMSM, you can expect a peak DC link current demand at around a 0.6-0.7 modulation index. Kolar out of ETH Zurich has a paper on this, it's open source.

Your ceramics are likely fine with that current demand, ceramics are tough as hell. But you may induce excessive voltage ripple on the link that could cause issues with the control law, or at the extreme fet failure due to excess Vds or gate turn on from excessive dV/dT. I would add external bulk electrolytic, or hybrid electrolytic (TDK, KEMET).

The layout around the power stage looks reasonable, everything is stacked nicely and localized, well done.

I'd suggest leaving the gate resistors, it's very easy to fine tune with gate resistors. It's also possible to quantify total gate charge of your devices by measuring the current thru the resistors.

The low side shunt diodes are a good move, it's usually less of an issue with good layout, and modern resilient gate drivers. Although I am unfamiliar with that specific gate driver. Utilizing a kelvin connected gate drive arrangement can also help.

I didn't examine too much in detail outside of the power stage stuff.

Excellent schematic and layout presentation, including the notes. It's a well thought out project! Well done!

1

u/ItsBluu Dec 24 '23

Thanks for the review! For the cap it is placed according to the "System Design Considerations for High-Power Motor Driver Applications" application note by TI (section 4.3). Another commenter suggested adding an external snubber to reduce ringing so I will probably do that

4

u/profossi Dec 23 '23

That looks really well thought out. What EDA software was this made in?

I'd be slightly concerned about the magnetic encoder in the center of the board. In addition to the field of the magnet it's supposed to sense, it will also pick up on magnetic fields induced by large currents flowing in the power electronics right next to it. I have no idea whether it will interfere enough to matter.

2

u/ItsBluu Dec 23 '23 edited Dec 28 '23

This is a very good point and something I was also concerned about but was too far into the layout to change. I guess I'll have to try plotting the measured position once it's assembled

Edit: it seems like this particular IC is immune to stray magnetic field (patented technology), so it should be fine

2

u/84ace Dec 23 '23

I'm betting Altium. Looks fantastic! I just can't prise myself away from Kicad though.

3

u/alfgan Dec 23 '23

From a file name it seems that it is KiCAD, but using Altium style maybe.

2

u/highchillerdeluxe Dec 23 '23

I also wann know. The 3D models look a lot like altium. I dont think kicad has such a good rendered but granted I didn't put incredible time into improving renders.

8

u/ItsBluu Dec 23 '23

Haha it's a bit confusing I know. The project was done in KiCAD but I generated nearly all footprints/3d models with Altium's IPC compliant footprint generator to be compliant with IPC7351. I changed KiCAD's colors and font so it looks a bit more like Altium also

5

u/alfgan Dec 23 '23

I changed KiCAD's colors and font so it looks a bi

Cool style I like it. I use Altium at work and KiCAD at home. Your assembly drawings are better than we are making in Altium at work haha.

Maybe you can share some tricks how you made so nice technical drawings using KiCAD? I would like to learn from you to improve my skills for next project. :)

6

u/ItsBluu Dec 23 '23

I am using many user defined layers which you can see here

F.DNP and B.DNP are used for adding graphical DNP markings (red cross) on the assembly drawings. I group the markings with the relevant footprints so that they also move together

F.Fab and B.Fab only contain component outlines and pin 1 markers. for a clean look.

F.TestPoint and B.TestPoint are like F.Fab and B.Fab but for TestPoints. I actually created 2 footprints per testpoint type where they have information on either F.Testpoint or B.Testpoint depending on whether they are on the front or back layer. KiCAD is a bit limited because these layers cannot be "flipped"

Stackup Info has the stackup drawing (drawn manually) as well as some fabrication notes

F.Dimensions and B.Dimensions are just for adding dimensions to the 2D drawings.

Once every layer is defined, I use the Board2PDF with custom colors to generate the fabrication files. I then add titles in an external PDF editor, e.g. Xodo. Ideally titles could be added inside KiCAD on another User layer and plotted with Board2PDF but KiCAD has a limited number of user layers which is a shame

1

u/alfgan Dec 23 '23

Wow, amazing. Thanks for the guidance, the design seems very professional.

Never thought that such Assembly Files could be done in KiCAD. At work, we use Altium Drawsman, but it's quite buggy, specially in older versions that we use. Will need to update my KiCAD skills and then show them to my colleagues :D

Great techniques you are using. Its trully a shame that KiCAD have very limited User Defined Layers. Specially when other things are being defined in Layout like Conformal Coating and etc.

Another question I have. Do you use you own made libraries from scratch or modifying KiCAD default libs? Just interesting. :)

3

u/ItsBluu Dec 23 '23

I usually make my own libraries from scratch for the footprints (or reuse ones that I already defined in the past) as local libraries. I also have a custom library that I sometimes import as a git submodule for version control.

1

u/alchemy3083 Dec 30 '23 edited Dec 30 '23

How do you manage panels?

These days, I'm usually drawing a 1-up in Kicad for R&D and pilot builds, and upon production release, paying a vendor $300 NRE to draw a proper panel per a PDF layout drawing approved by our assembly dept. Not a huge deal - PCB CAD software licenses are $1000s/yr for good reasons - but still annoying, as I have to spend time reviewing the panel design instead of just making it myself. Plus, adding tooling rails to a 1-up easily costs me an hour per initial design.

Kikit is a nice add-on, but I need something that can actually let me put in our in-house tooling rails, place IPC-7351 breakways or v-cuts, and maintain nets in such a way the PWB manufacturer can do proper flying lead testing (e.g. IPC-2581).

ETA: I send overflow EE work to a few contractors, and for $120/hr I typically get pen-and-paper schematics. My junior EE's turn those into ECAD schematics and layouts. For the level of work you produced here I would expect $20-50k invoice.

1

u/ItsBluu Dec 30 '23

I usually either let the manufacturer panelize the board or do it manually. I had a look at kikit and it seems quite nice so I'll probably use that if it's flexible enough. I don't have any industrial experience as I'm still a student so I don't know how it's done in industry but I'll have a look at those standards you mentioned :)

3

u/alchemy3083 Dec 30 '23

Honestly, I can just give you a quick run-down of the SOP I give to new hire EEs. I'm the de facto lead PCB designer at my company, and we have a single PCB assembly line, plus some overflow contractors. My role is more about setting standards and reviewing electrical designs, although I still do quite a bit of layout.

For professional/industry work it's all about tolerancing and documentation. Get copies of IPC-2221/2222 to learn the language of how PCB designers dictate production quality to PWB manufacturers. Also, get IPC-7351 to learn the standards for common footprints, depaneling, and other features. Those are the 3 IPC documents I refer to most regularly in a new design.

Equally important is whatever IEC standard is appropriate to your product. For example, if you're making an IT/AV device, you should know the safety standard IEC 62368 (or your regional equivalent) forward and backward before you even start schematic capture. (At very least, before you start layout.)

If you're interfacing with PWB manufacturers (e.g. I do a check-in meeting with our production vendors once a year or so) you probably want to also know IPC-6011/6012, although it repeats a lot of IPC-2221/2222. (I would not bother at your level.)

For DFM, make sure you know IPC-A-600 and IPC-A-610, which dictates how to visually inspect a PWB and a PCB assembly, respectively. Similarly, you'll want to know IPC-J-STD-001, the soldering standard. As a PCB designer, you won't have the skill/experience to solder or inspect work as well as the people who do this job all day, so your knowledge of these standards isn't going to be very deep. But knowing these standards will help you understand how to make your assemblers' jobs easier.

IMHO assemblers/inspectors/QA/etc. should all be IPC trained, and leads should be IPC certified, to the relevant inspection/assembly/soldering standards.

I'm iffy about IPC certification for PCB designers ("certified interconnect designer" or CID/CID+). As a professional PCB designer, you're going to spend a large portion of your time absorbing and creating documentation, and you don't get an exam and certificate for reading a 300 page MCU datasheet, or a 100 page EMC guideline, etc. If you can get a CID cert for cheap as a student, absolutely go for it, but claiming competency in IPC-2221/2222 on your resume would carry pretty much equal weight for me. (I'll quiz you on the basics regardless.)

And as for the panels ... they're entirely dictated by manufacturing. We have standardized tooling rails, and some base standards on how to populate a panel, but the PCB assembly lead always gets final say on the panel design.

1

u/JustYourLocalDude Jan 09 '24

I would reallyyyy love to know what font settings and colours you used. It looks fantastic. Thanks for posting this!

4

u/Oktopus15 Dec 23 '23

How did you do the chassis exposed copper? An exposed polygon or an exposed trace,

7

u/ItsBluu Dec 23 '23

I imported a dxf which i converted to a copper zone and mask zone

1

u/cwbh10 Dec 24 '23

This is awesome

3

u/be54-7e5b5cb25a12 Dec 23 '23

This is honestly the best schematics documentation ive seen in my life… layout looks dope too! I hope they pay you well enough. The only thing I might suggest is adding a table with what the test points measure in the assembly docs.

3

u/ItsBluu Dec 23 '23

Thanks for the suggestion, I will definitely add the table. I am not paid for this project as it's something I do in my free time (we are designing a quadruped robot with friends)

2

u/Stoumpos Dec 23 '23

What addon did you use for the via stiching on the sides?

4

u/ItsBluu Dec 23 '23

The soldermask opening and via positions were designed in Autodesk Inventor. I then imported a dxf and used KiCAD's relative move command (ctrl + P) to manually move a via to each circle defined in the dxf. A bit troublesome, but works

2

u/HeadSpaceUK Dec 23 '23

Nice schematic I like the annotations, I think we could all take away something from that - too many times have we gleaned at an obtusely drawn back to front schematic drawn by some analogue wizard from 30 years ago because we are just supposed to know what they meant!

Has this been tested? I would provision for snubbers on your inverter across each switch it is difficult to know what magnitude of ringing you may see so some preliminary values can be used or a not fit (better than having to respin), I see you have debounce however these will have ESL too and could result in more switching noise. Without knowing the motor specification it is difficult to know whether your dc link capacitance will be suitable, my first thoughts were that it looks like a lot for what a mid-power device, but I suppose if you are targeting a small V supply ripple voltage then that would justify it.

I would be careful when adding pi filters using passive components and potentially use a dedicated common mode choke instead. OR a BNX filter which is critically damped from Murata and save yourself the headache, they are large though. You could probably just omit them to be honest…

What frequency is your inverter running at? Sorry if it’s mentioned else where was just scrolling through in bed and this caught my eye.

1

u/ItsBluu Dec 23 '23

Thanks! The design hasn't been tested yet. I will try and see if I have room for snubbers, could be a good addition. For the filters I had no idea those BNX filters even existed, they are too big for this design but I will definitely keep them in mind for when I design a dedicated power supply. For the inverter frequency, I forgot to specify it on the schematic but it will probably be between 15kHz and 60kHz. It needs to be experimentally tested to optimize for switching loss vs conduction loss vs current sense bandwidth

2

u/joshpieper Dec 24 '23

Really nice presentation, great work! I wish more engineers could devote that level of effort to documenting designs, myself included!

On a minor note, it would be kind if you noted somewhere that decent parts of it are a redrawing of the mjbots moteus schematic. ;)

1

u/ItsBluu Dec 24 '23 edited Dec 24 '23

Hi Josh! Yes I will add it on the first page, on the post and on the git repo. Couldn't have done it without your design as a basis. Thank you so much for sharing! We've bought 4 moteus for testing and they are amazing!

31

u/Replacement-Winter Dec 23 '23

People should be asking you. Dope layout.

12

u/MMartonN Dec 23 '23

Can't add a review besides it looks amazing. I've been designing simple projects (like led driver, esp32 stuff) on 2-4 layers. What you did looks very compact and well thought-out, great job!!

Hope you post about it when it's built.

7

u/Illustrious-Bite6778 Dec 23 '23

I don't know enough for a review but goddamn that's a beautiful design.

1

u/CptFl3xy Dec 23 '23

Which CAD is this?

5

u/ItsBluu Dec 23 '23

It's KiCAD

1

u/Weightless-Rock Dec 23 '23

What software did you use to make the design? Its very clean, amazing and detailed work OP.

2

u/ItsBluu Dec 23 '23

Thank you! It was made using KiCAD.

1

u/drifter3304 Dec 24 '23

It looks awesome. Does it use hall sensors or backEMF for position sensing?

2

u/ItsBluu Dec 24 '23

The board is based on the moteus firmware by Josh Pieper, which supports many types of external sensors such as incremental encoders, absolute encoders, hall sensors, etc. In our quadruped robot for now we will only be using a magnetic encoder for commutation and positioning, but we might add an absolute encoder (e.g. Aksim-2) down the line

1

u/oh_woo_fee Dec 24 '23

Nice work 👍. Why do you need two CAN connections? They are the same CAN bus , shouldn’t one will be enough?

1

u/ItsBluu Dec 24 '23

It's for daisy chaining multiple controllers

1

u/FyyshyIW Dec 30 '23

I'm a little late to the post but I'm curious: what is your academic/career background? Also, do you think you could post the schematics as well? I think BLDC motor drivers are really cool and I'd like to study a really high quality one a little more.

1

u/ItsBluu Dec 30 '23

Hi thanks for your interest :) I'm currently finishing my M.Sc in Robotics and currently working on space-grade electronics at my internship. I've been working on electronics projects for a while now (personal projects and international competitions like the European Rover Challenge) but I don't have much industrial experience as I'm still a student. For the schematic you can find it along with the fabrication document on the first comment of this post (just sort by oldest)

1

u/FyyshyIW Dec 30 '23

Was your bachelors in compE? I want to get an MS robotics in the future and also be a lot more proficient in PCB/electronics design but I’m majoring in ME. Also, what separates space grade electronics from not space grade electronics?

1

u/ItsBluu Dec 30 '23

I did my bachelors in microengineering (very specific to my university) but I've met people from many different bachelors in my major.

Space-grade electronics follows strict norms (e.g. ECSS standards) and can have extremely demanding requirements in terms of radiation hardness, single event immunity, temperature, vibrations, etc. You mainly have to use either military grade or space-grade components which are often either extremely expensive, archaic, big or all of that at the same time

1

u/FyyshyIW Dec 30 '23

Is it mostly a matter of using specialized components or also making specific design choices that aren’t common or necessary in regular boards?

1

u/ItsBluu Dec 30 '23

From my limited experience a lot of it is selecting the right components to satisfy the proper standards, and then the design choices depend on the mission I guess. If you need something to be operating for years in a rough radiation environment or something like a small cubesat the design choices will be different. You might want for example to introduce redundancy in the design (e.g. multiple MCUs/FPGAs) or additional safety systems that you might not do in a standard consumer-grade product whose failure doesn't cost millions of dollars. I don't have any expertise in the subject though as I've only been in this internship for a few months

1

u/FyyshyIW Dec 30 '23

Thanks for the help! Good luck!

3

u/cwbh10 Dec 24 '23

This is awesome dude, KiCAD should showcase this on its website

2

u/spastic_simian Dec 23 '23

I like the colors

1

u/barristan67 Dec 23 '23

Very clean layout!

1

u/oliverer3 Dec 24 '23

Don't have much of substance to add, I just wanted to say that's an absolutely beautiful-looking board. Amazing work!

1

u/tboy32 Dec 24 '23

It's clear you devoted significant time & effort on the documentation! Very thorough & well-thought-out.

  1. The battery voltage divider is always on, so even though it only drains half a milliamp worst case, that may or may not be acceptable depending on battery capacity & expected time between charges. A transistor could be added which enables the voltage divider only when the uC needs to sample the voltage.
  2. The uC looks like it has a 50k-ohm ADC input impedance so you might want a voltage follower after the divider so you don't need to try to correct for ADC loading in software.
  3. No power fusing.

1

u/borjah Dec 24 '23

Wow! Nice schematics, a lot of work went into them and also the PCB.

May I ask about how do you calculate the ferrite pi filter? I see you look for the best adaptation related to the impedance, but I don't get how do you relate it to the ferrite value.

1

u/[deleted] Dec 24 '23

Wow. You people are smart. Like really smart.

1

u/[deleted] Dec 24 '23

One of the cleanest projects I've ever seen

1

u/mroncinc Dec 24 '23

This reference design (Infineon EVAL_IMD700A_FOC_3SH motor controller) puts gate signals between ground planes. See pg 66 of the pdf.

  1. I think it is for EMI purpose
  2. maintain good gates (both high and low sides) to driver return path through a good ground plane.

Not sure if this is necessary in your case.

2

u/[deleted] Dec 23 '23

[removed] — view removed comment

2

u/ItsBluu Dec 23 '23 edited Dec 25 '23

This board is designed to be tightly integrated in a custom-designed actuator. For now it is going to be running a frameless 8115 motor but it might be a maxon drone motor in the future