Andrew J said:

I didn't find a way to create a blog in this section.

Fixed Thanks for posting!

And something weird's going on with the images there, they're so wide they're being cut off, I'll check that up with the dev' team, until then you might want to click on them and edit their width/height.

When I click on them, I get the full size.  If I edit them to reduce the size, I presume that is purely within the posting?

Yes, it is!!

Hi Andrew,

Very nice board, it looks well laid out, I've never built a DC load but it looks pretty reasonable to me. I was wondering, are the large resistors required to be 1 ohm, or was that a placeholder value? I was wondering if much lower resistances could be used, especially if all MOSFETs are going to the same heatsink.

It's a challenge to have a short path through the DC load when it has to go through physically large components, I too had this issue, and I'm not sure mine is a good solution, but I'll paste it here in case it gives any ideas for your board, or if mine has glaring errors in it too! My boards have arrived, so it is what it is for my prototype too. Mine was a MOSFET testbed, not a DC load, and was easier since I didn't have 4 MOSFETs to battle with. I used screw stud-type terminals, I think I would use connectors if I could go back in time. Also, my board is 4-layer since it is small compared to yours, and therefore the cost difference was small. I didn't use all 4 layers fully much, but was slightly handy for the high current path, and creating a bit of a shield for induced signals.

Some ideas to rule in/out for your future PCB could be as follows (these are all really minor, and not necessarily better, they are just a bouncing of ideas between engineers : )  

(1) Maybe use SMA connectors for test points related to MOSFET signals, gate voltage, etc., the connectors are cheap from (say) LCSC, it's not affordable to buy them from Farnell unless you need high quality ones for RF purposes. For test signals, any cheap SMA connectors would be fine. They can then be directly screwed into your 'scope via SMA cables and SMA-to-BNC adapters. Maybe not essential, but if you have the SMA footprints, they can be left unsoldered and used as testpoints anyway as well.

(2) Holes for mounting, granted you may be using a slide-in case that doesn't require it!

(3) The default TO-92 BJT footprint holes in KiCAD are in-line, which is more awkward to solder, they could be replaced with the triangle layout.

(4) Maybe worth considering to consolidate the connectors to one or two flat flex cables for the processor connections etc, they are probably cheaper than normal sockets/plugs, and less effort than making up crimped cables. It is also easy to solder wires to 1mm pitch footprints, so if worst case you needed to make some unplanned connections for your prototype, then you could omit soldering the flat flex connector and just patching wires to it (or have FFC and 0.1 inch header pins on the board).

(5) I can't tell, are the connectors on your board for directly mounting MOSFETs? If so, are they on round millimetre offsets? Otherwise, it's a pain to drill out a heatsink. When placing off-board parts, or external connectors or controls etc., I've found it convenient to place them on a millimetre grid rather than imperial mil etc.

Anyway, the DC load is an interesting project and a great-looking board from my perspective, and looking forward to hearing how it goes : )

I'm assuming that Q1 and friends are intended to operate as current limiters in case of short term overload.

If so then R11 is the wrong value (typo ?)  - 270k is way too big, but 270R would be OK.

I would normally put a resistor in the base ciruit of Q1 and no resistor in the emitter circuit. You need one or the other (or both) so that Q1 doesn't try to clamp the voltage across R12 with its base/emitter junction.

Your cicruit will suffer from a common problem with DC loads (including mid priced commercial ones.).

If you set it as a current sink with a non zero current and no applied voltage at J11  then U1c will saturate with maximum positive output. All the power MOSFETs will be turned on and their gates fully charged up.

When voltage is applied the initial current spike will be huge. It will go on for some time because the MOSFET drive resistors are so big and because of the10us time constant of C6/R3.

I have a Rigol load which has a similar issue, it is not possible to get an Infineon protected high side switch to apply 24V to the load (set for 1A) because the initial current spike trips the 20A hard limit on the high side switch. I found this to my cost when I designed a multichannel test rig that used the Rigol load for measuring

I've spent some time trying to think round this issue, so far without much success.

You may be able to mitigate it in software.

MK

Thanks Shabaz.

Using 0.1Ohm resistors was a start point in dealing with the slight construction differences in the parallel MOSFETS to help balance out the negative Vgsth co-efficient - any MOSFET that was drawing slightly more current would cause a larger voltage drop over the resistor, thus reducing Vgs and the current draw.  In practice, in conjunction with the NPN transistors which provide the active feedback, it seemed to work better with a higher value - 1 ohm - without the (potential) drawback that it has a bigger impact on the circuit because it causes an even bigger voltage drop. I’m benefiting here from the results of experimentation! 

I want to be clear here, again, that I owe John Scully a lot for this parallelisation circuit and real-world observation.  I started off with a bog standard parallel design but from research it was clear that would cause issues, particularly at higher currents.

All the MOSFETS will be mounted on an off-board heatsink and I wanted an easy way to connect them to the board without having to provide soldering holes and then carefully position the PCB/heatsink together to not strain them.  That would of course have the benefit of shorter paths.  My start point is that the active feedback to balance the MOSFETS and short wires from the MOSFET to the board connectors won't have a big impact, or nothing that can't be adjusted from the readings in the Sense circuit - something to look at though.  The connectors I've plumped for are these: Metz Connect spring loaded connectors

The other connectors are ones I had to hand which is why they are a mix.  It's interesting you mention ribbon cable because I did start off with that premise.  However, as I was laying out the board it became much easier to stick to two layers with signals on the top layer if I could distribute the board connectors over the surface - hence why they're sort of all over the place!

The biggest issue I had with connectors, in general, were finding ones that were mountable on a panel.  

(1) I'll check out SMA connectors on my next board.  I went with what I have/used to without giving it much consideration TBH.  It's a good idea.

(2) Very specifically this time I designed the PCB in conjunction with an enclosure - in this case, one that has rails to slot a PCB into, hence the 181mm wide board.  I normally add mounting holes of 3.2mm diameter for an M3 mount.  Pretty much every single time I've built up a PCB, looked for a case only to find if I'd done that first I may have a wider and cheaper choice.  It's also very hard to filter enclosures on retailer websites as they don't seem to use height/width/depth consistently.

(3) Yeh, they were a pain to solder you're right, and I did have to rework one of them.  Worse, I've been bitten before.

(5) The MOSFETS are all heatsink mountable and I don't know if the spacing of the connector footprint would actually allow them to be soldered to the board.  I think I understand your point though - I have seen instances of MOSFETS soldered to the board then attached to the heatsink and I considered that to be difficult to do accurately.  Seems from your experience I was right.

Thanks Michael.

The NPN transistors (Q1 and friends) are a form of current limiting in the sense they are part of an active feedback for a MOSFET that would want to normally draw more current because of its’ construction difference.  They are used to drag down the voltage on the gate (Vgs) to reduce the current through the MOSFET to help keep them in balance. This is all part of dealing with a Rds-on positive temperature impact and a Vgsth negative temperature impact.  It started with a lower valued emitter resistor but changed to 270K as a result of increasing the Source resistor, e.g. R12, to 1Ohm.

As I mention above, I've benefitted a lot from John Scully's work on this particular aspect and his real-life observations.     

The switch on surge is interesting observation and I'll have to watch out for that.  The DAC in the ICB starts up at 0V output, though in theory it can be configured alternately, and the MUX output is also off because the PWRSIG input is low.  So at startup there should be no issue with a non-zero current at U1C, but one to watch out for - I mention it because some DACs power up at midpoint by default.  Dealing with a non-zero current and no voltage after startup, I might be able to handle differently.  To apply current, PWRSIG has to go high: even though there is a physical button and a touch button to do this, it is still software driven.  If through the Sense circuit (which is active even if no sense cables are plugged in) I read zero volts I could prevent PWRSIG from being raised.

I suppose the big question there is: in testing that, is anything likely to blow?  I've tried to put in a fair bit of protection to prevent damage to expensive components but it would be good to understand the risk.

These are a few random thoughts, in random order, from a quick view of the board.

I can't see where -5Vgnd joins +5Vgnd. Does that happen off the board? As it stands, -5V doesn't seem like it would have any relationship to the other voltages on the board.

Some of the high current tracking could be a more generous. The track from pin 2 of the fuse to the connector, and the track across the top, 'Net-(D2-Pad1)', in particular. The track you've got is about the minimum you need for 5A (assuming a 20C rise, which is the kind of conservative figure you'd go with for something commercial), but you've got room to make it much better than that.

What kind of 1R resistors are they? Are they wirewound? Inductance? Temperature coefficient?

The transistor footprint looks horrible.

I can't get my head round whether the transistor feedback does what you want or not. Is it possible that it works simply by virtue of the added resistors (in the same way that adding emitter resistors allows BJTs to be paralleled)?

What's the contact resistance of the non-screw terminals? I'd be a bit nervous of using something like that to wire power devices to a pcb. Maybe that's just prejudice and being very old-fashioned on my part.

It feels to me like you're building too much inductance into the high-current output loop, both with the layout (separating load+ and load-, and so forcing the external wiring to be a wide loop to follow suit) and having all these loops off the board to the various power devices, but maybe it will be ok. We'll find out when you try it. 

Thanks John.  

I take note of your comments on layout and trace sizes.  It will be interesting to see how it tests out when I get around to it  If this causes issues, I think I'd go back to the drawing board and relayout those connections and design them to either direct mount the MOSFETs on the board or re-arrange the solder points to allow direct solder wire rather than use connectors.

This is a module for my ICB so is designed to be driven by that: all grounds are tied at one point there.

The 1R resistors are wire-wound: Buy Now .  The connectors are rated to 300V 9A and can take quite a thick wire (up to 16AWG) so should be ok - there's no information on contact resistance though, which I hadn't thought about until you mentioned it!  Datasheet link in a post above.

I'm not sure what you mean by the transistor footprint looks horrible - you mean aesthetically? Functionally?

Personally, I'd common the grounds on the board, not back at the power supply. If this was a commercial product, you'd filter the power coming on to the board, so you want the common point to be the plane immediately after that (and rely on the low inductance and low resistance of the plane to make that the same, as far as possible, over the whole extent of the board). Otherwise you've got the lead inductance and the filters between different points of what you would hope would be a common reference ground.

Two things to think about with the resistors.

A wirewound resistor is a coil of wire that has a dc resistance of the chosen value (in this case 1R). But coils also have inductance, so at a megahertz it's going to be behaving somewhat differently to a pure resistor. Although you've slugged the op amp, so that it doesn't get too frisky above a few tens of kilohertz, the MOSFET and the BJT can probably manage a bit of mischievous behaviour up there AND you've got that gate capacitance that will happily resonate with an inductance if there's a bit of gain to keep everything going. I'm not saying that it will be a problem at all, just that it's an 'amber light' so to speak - something to be aware of and to look at.

The temp coefficient might be as bad as 400ppm/C (according to the datasheet). That's approx 0.4mR/C for a 1R resistor. The temperature rise for 20% of the rated wattage is about 20C (graph on datasheet), so your resistance change from 0 to full current might be 8mR, or so. How does that sit with what your sharing circuit is doing? Not necessarily a problem - might even help you, but again worth a look.

Better resistors are available for power work. Thick film resistors have better temperature specs and can be much lower in inductance.

The connectors might be ok. If they can carry 9A then the contact resistance can't be too high. But with 2 for the diode, 2 for the MOSFET, and 2 for the sense resistor in the high current path, that's getting to be a fair amount of extra resistance.

Don't mind me over the transistor. I'm just old. The TO92 package replaced metal can parts that had the middle pin offset to give a triangle shape to the arrangement. So the TO92 parts would have the pins formed to the same pattern (you could even buy them ready formed). There were plastic supports that you could buy that would form the leads and support the transistor above the board. The reason for the support, though, was more than just shaping the legs. If you have a package like that and solder it hard against a board, which you can do with the footprint you've got, then temperature cycling of the whole thing can damage the transistor - the support acts as a buffer between the two.