My first PCB design - E3610A power supply

[just_fib_it]

I've been working on creating my own version of the HP E3610A power supply. I've basically copied the schematic from the service manual, only adding some connectors and a few decoupling caps.

Attached is my first attempt at laying out a PCB (which doesn't contain the the +/- 12V bias supplies, those will be on a separate board).
The goal is to have one PCB supporting all three models of this supply (10A, 11A and 12A), so I've tried to design the power section such that it can handle the 3 amp of the 10A as well as the 120V of the 12A.
BTW, it's a 10x10cm board, most resistors/caps are 0805, the ICs are SOIC.

A few questions:

• The original design is all through-hole, I've replaced most components with SMD equivalents. Are there any traps for young players with this approach? In particular, will this affect the stability of the control loops?
• Currently the ground plane is only below the analog circuitry, would it be better to extend the ground plane over the entire board? Should I add a copper pour to the top layer as well?
• The big tracks are 150mil (@ probably only 1oz), is that enough for 3A?
• Any other feedback? Please don't spare my feelings, I'm here to learn 

Thanks in advance,
just_fib_it

[DanielS]

In principle, upgrading a layout from through-hole to SMD should improve performance by cramming all the components closer together so current loops can be made smaller and have fewer opportunities to pick up noise. MLCC capacitors have lower

Bringing everything closer together does increase the possibility of crosstalk though so if you use higher-performance equivalents of the original parts, you need to be extra careful with the layout so your higher-performance parts do not end up amplifying noise.

[just_fib_it]

That sounds promising; there are SMD versions available of the opamps and v-ref used by HP, so I'll start out with those. The only obsolete parts I ran into are the 2N6056 power transistors used in the 10A and 11A variants (the 12A uses MOSFETs instead). I think I'll first give it a try with some darlington BJTs and if/when that works switch to a MOSFET. I've been eyeballing the MJH11022G, the power specs (voltage, current, SOA, gain) are fine, but it has twice the output capacitance (200 vs 100 pF), I have no idea if that will be an issue, but I guess I'll found out...

BTW, what were you going to say about MLCC caps, lower ESR? Your sentence was cut off:

MLCC capacitors have lower

[DanielS]

BTW, what were you going to say about MLCC caps, lower ESR? Your sentence was cut off:

I have been bouncing between a ton of things and apparently posted something incomplete along the way.

Anyway, I meant to say lower ESL/ESR so for (de-)coupling applications, they should fare better than most of the through-hole stuff. This can be both a curse and a blessing since it also means they will have less dampening effect if something ends up resonating.

And then there is the voltage-dependent characteristic which might be bothersome - Dave did a video on that a few months ago. You need to pick your MLCC caps carefully if the in-circuit value is critical.

[mrkev]

Hi, not bad at all for a first PCB design. Just few recomendations:
- If you are building relliable device, size shouldn't matter. Don't beat yourself to get it on 10x10cm board, while you may miss some important things. 
- You should never route capacitors on separate route from where the main current flows. F.e. the route from rectifier to C2 is added serial resistor (and inductor), which is actively increasing your ESR. The same thing for C3 (even worse case). For some bigger current impuls, its like if it's not there at all.
- Make sure that you know which part of design does what. You've done quitte a good job with that sensing (R27 and R34) and connection of grounds.
- Keep feedback loops as short as possible (f.e. R6, C6 is IMHO OK).
- Make sure that you block the supply voltage for OAMPS. Blocking caps are often not in the schematic (!), I see that you've added C40-43. One cap between U1 and U3 (on +12V and -12V) shouldn't hurt . You can also add some caps at those power lines (f.e. near R3, R43), same thing
- It usually looks better if you use like 3 or 4 different widths of routes only (you've done that).
- Even tho devices like MOS-Fets have (in stable mode) no current flowing into gate, keep in mind that you have to charge/discharge the cappacity of that gate. I would personaly use wider routes from R39, R38, R45/C22, R44/c23 and Q2, R3. You have a lot of space there, so why not use it. Btw placing R3 is good solution since it has current path to Q2 and voltage path to the resistors at gates. I would maybe took the -12V for Q2 from a separated route than from OAMPS, but i don't think it's critical.
- Voltage sources are usually made in line, I get that you wanted to have J4 and J1 on the same side and to save space, but if you think where the main current flows,  there is one big open loop (rectifier, fets, R35/36, R2). Those power routes should be close together (essentially the same way you've done +12V and -12V).

[Phaedrus]

Those tracks are more than enough for 3A. I can't shake the feeling that some of those power traces could be a bit shorter. Like mrkev said, you want those to be as short as possible to reduce parasitic RL components in the main loop.

Overall not too bad though! It'd probably work as is, but reorganizing the power traces would make it more optimal.

[TheRuler8510]

just_fib_it,

Just a heads up...I did troubleshooting & repair of a 3610 and I suspect the schematic is not 100% correct.  I could never put my finger on it exactly, but something is not right in the error amp area and (maybe) the connection to the series pass transistor. Maybe it is related to the fact that it is the same schematic for three different models--I don't know.

But then again--maybe I didn't have enough sleep that day. Anyhow, I'd be real interested how your project comes out and if you made any mods to the original schematic.

Regards,

[just_fib_it]

Thanks all for the detailed feedback, it's much appreciated 

I've reworked the layout of the power section a bit, will try to incorporate the rest of your comments next.

[c4757p]

Those tracks are more than enough for 3A. I can't shake the feeling that some of those power traces could be a bit shorter.

Or wider, same effect

[just_fib_it]

Just a heads up...I did troubleshooting & repair of a 3610 and I suspect the schematic is not 100% correct.  I could never put my finger on it exactly, but something is not right in the error amp area and (maybe) the connection to the series pass transistor. Maybe it is related to the fact that it is the same schematic for three different models--I don't know.

Thanks for the warning; I thought I had tried the circuit in LTspice, but just realized that that was the 3614 
Well, I can't really be bothered to redraw another circuit in LTspice now, so I guess I'll see what happens. Maybe I'll learn something about troubleshooting and bodge wires (or magic smoke...)

[matkar]

Nice first PCB design. Most of us probably started with something simpler
Just an observation; have you verified the footprint of C2? Those holes seem very small  for a capacitor that size. It wouldn't hurt to increase pad size as well. Spacing between pads seems odd too. Usually the leads are closer together.

[just_fib_it]

Nice first PCB design. Most of us probably started with something simpler
Just an observation; have you verified the footprint of C2? Those holes seem very small  for a capacitor that size. It wouldn't hurt to increase pad size as well. Spacing between pads seems odd too. Usually the leads are closer together.

Nice catch, the C2 footprint was indeed way off: the caps I intend to use - and have already bought - have 10mm spacing, the footprint I was using had 22mm spacing