Standby PSU

[zoidbergslo]

Hey forum.

First post here so please be gentle

Ok so here we go. I am working on standby PSU that will control relay to switch mains on or off. It will have few possible I/O for control (button, led, IR, additional offboard relay, serial com with optoisolation). Mainly I am making this for my amplifier and preamp but essentially it could be used in other applications.

I have built one prototype but i was not really happy how it came out. No fuse onboard, hard to get ATTiny out of it, no heatsink on regulator. And since I built it I added second relay into specification so pinout on connectors needed to be changed as well.Prototype can be seen in attachments under name avr_v09 I have attached schematic, pcb, and finished product.


Now for second iteration I have changed few things around and added few things to PCB. And I have some questions if I am going to right direction or should i change more stuff. Ill go through list of things that I want second opinion on. See attachment under v01f.

1. I have added two separate fuses onboard one for psu and one for load controlled by relay. Fuses are Littelfuse TE5 369. Rating on fuses should be fine but I am bit concerned since most other product usually use standard 20x5mm but space is a bit of a premium.
2. Changed bjt to mosfet for relay control. And added another mosfet for controlling offboard relay. Now the question is is it better to put mosfet close to relay or leave it on this board. I know I need to put flyback diode as close as possible to relay but I could not find any good information on mosfet placement.
3. Changed relay from Omron G2R-1A to TE RYA31005 since it is a bit smaller and uses less power. Also added snubber to relay contacts (0.1uf and 100ohm). For my application I will be switching on and off 20VA transformer in one application and 300W SMPS in another. I am guessing that relay is still overspecced for my application for not to worry about inductive load.(I hope).
4. Is psu layout good enough or should I change some things around. (transformer is 2VAC 2VA, filtering cap is 1200uF Panasonic FR, regulator is TI LM2940c but I will probably change that because of high Iq, cap behind regulator is 47uF that satisfies regulator ESR.)

Other things changed
5. ATtiny85 moved to different position for easier extraction.
6. Regulator position changed so I can add heatsink on it.
7. Rearranged connectors and changed pinouts. Led and button connector were moved together on single 3pin connector. Serial communication was moved to 3pin connector.
8. Added optoisolation for serial communication. Board can be used as master or slave so one sends and the other receives  serial data It just depends on what parts are populated.
9. Changed mains connection to screw terminals.

Any other suggestions are also welcome.

I will put everything to github when it is finished. Also don't mind the versioning of this thing but prototype was named AVR switch and version v09 was actually build. Since then I changed name to Standby psu and version started with v01

[wraper]

You made clearance between primary and secondary lower than one should feel comfortable with non grounded device. And that without any reason ar actual design constrain.

[wraper]

1st iteration: Also unsafe distance to mounting holes. You should inform any makers or customers that it's safe to use plastic standoffs only. And again, distance to live is lower than it could be without any reason. Just moving one track would increase it significantly, yet not sufficiently.

2nd iteration: When connecting it to mains, voltage on R7 will exceed is maximum voltage rating. Check the datasheet, such size SMT resistor unlikely to be rated for 350V+. Situation with mounting hole - live distance is much worse than with first. Components near left lower hole will experience mechanical stress and are just asking to be ripped off while mounting the PCB. All in all PCB design is unsafe crap.

[zoidbergslo]

You made clearance between primary and secondary lower than one should feel comfortable with non grounded device. And that without any reason ar actual design constrain.

I made sure that pads are far apart (relay position) but I will change position of track going from fuse to relay as well. Thank you for this.

Also unsafe distance to mounting holes. You should inform customers that it's safe to use plastic standoffs only. And again, distance to live is lower than it could be without any reason. Just moving one track would increase it significantly, yet not sufficiently.
During connecting device to to mains, voltage on R7 will exceed is maximum voltage rating. Check the datasheet, such size SMT resistor unlikely to be rated for 350V+.

I was planing on using plastic standoffs with plastic screws yes. R7 footprint is 2010 size and i was planing on using farnell link but I could change it to THT footprint.

[zoidbergslo]

OK I rearranged few things around and removed separate fuse for psu and kept on just one fuse for the whole system. Spacing between primary and secondary is at lest 10mm now. Spacing between L and N is 3mm. I also changed R7 (which is R11 now) to THT part. Also shuffled around bottom left corner. I hope this is better.

Oh i didn't write in previous post first iteration was 55x47mm big board and this new iteration is 70x55mm.

[wraper]

That's much better, still I cannot say that I like live proximity to the mounting holes. You could safely move C5 closer to the secondary side and move R11 further from the mounting hole. Also you could move fuse closer to the secondary side and use both layers of the PCB, therefore removing track away from top right mounting hole. Something like on the pic.

[wraper]

BTW I think it's a good idea to move electrolytic cap and free up space to move Vreg away from mounting hole. Also 5V relays consume a lot of current, therefore vreg will heat up a lot. You could power relay from say unregulated 12V. Current consumed by the rest of the circuit will be tiny.

[zoidbergslo]

Ok I changed things around as you said. Also had to put in pullup resistor on reset pin since I forgot it.
About relay power: I did change relay to less power hungry option compared to my prototype. If I calculated everything correctly continuous power consumption of the board and extra relay on secondary board would be under 120mA. I did some testing on prototype with additional 50ohm dummy load on it and regulator did get pretty hot but it had over 200mA load on it but that was without heatsink. Regulator was dropping around 2V at that point. I am waiting to get my temperature sensor to get better readings of that.

[wraper]

So much better. BTW, you have plenty of space to place all SMT components on top side. Does not matter that much if you hand solder all the parts. But if you decide to run even small series of them, double sided SMT load is a complete showstopper from assembly standpoint. Not only if built at factory but even if built by hand (applying paste with stencil + reflow in oven).

[zoidbergslo]

Ok tried putting all componets on top and had few problems on my implementation of optical isolation of serial so i removed that to small secondary board. I don't know if layout is good enough. Any tips or is it good enough?

[zoidbergslo]

I am guessing you wanted to say AC/DC modules. I will take a look at that but I was just redesigning what I already had. My only concern with those models is if they fail lets say in few years time will it be easy to get pin to pin compatible module?