Hi there,
So I'm looking at this solid state relay which comes in a through-hole-mounted package, but I'm wondering how I should mount it to my PCB because according to this PCB trace width calculator I need traces 737mil wide with 1oz copper to be able to handle 10A. Currently my traces are 125mil. How are these things supposed to be used if they come in a through-hole package??? Should I just opt for a screw-terminal SSR external to the PCB, and wire the leads separately?
Thanks!
Take a piece of bare copper wire and lay it on top of the PCB track. (Make sure you used the soldermask layer to keep soldermask off the trace.) Puddle solder around the wire until it looks like the example above. Single-core wire like you find in house wiring is good for this and that kind of wire is extremely cheap to buy at the hardware store.
If you're modifying an existing PCB then either scrape the soldermask off with a knife or just run the wire direct across the PCB.
Thanks, that's a great idea! 
Is that what they do on production-quality boards?
On production boards, they very frequently have a thick layer of solder on high current traces (like in that picture). They may also use copper thicker than 1oz.
737mil is for inner tracks of multi-layer boards.
125mil could give a 40C rise above ambient @10A on an outer trace.
For high currents, I add a second trace on the other side of the board.
2*125mil would be enough in your case (+12C).
If that's not enough, then think of messing with traces without solder mask.
Leo..
Really? That's good news, but is there an online calculator or equation where I can verify your numbers?
Thanks!
Hi,
Keep the copper traces as short as possible, that is mount the SSR as close to the power terminals o your PCB.
Tom...
@TomGeorge: Yup, that's what I'm doing. I just don't know if the traces can handle the amps.
If you are concerned about current capacity, solder sweat a 18AWG bare copper wire from one pad to the other along the trace.
.
Yes, but is there a calculator where I can see if i really need it or not? There must be some equation that tells me the trace width I need to handle a certain amount of current.
androidfanboy:
Yes, but is there a calculator where I can see if i really need it or not?
You aready posted the calculator.
But you used the wrong box.
The top green box if for inner layers of multi-layer boards.
The bottom green box is for normal tracks.
Leo..
Ahhh, thanks for pointing that out, I feel like an idiot now! Hahahaha I totally missed that lol.
Could I just make 2 gigantic planes (both top and bottom copper planes), one half for the one output pin, and another plane for the other pin? Or is that not recommended?
I've attached a picture of what I'm talking about.
Full plane with that many vias is a bit silly I think.
Two straight fat tracks, double-sided, is all you need.
No mounting holes? Mechanical safety is also important.
480V AC? relay from the link was only rated for 280AC max.
What is the primary/secondary creepage distance.
Do you know the legally safe distances if the primary side is grounded to mains ground, or not.
And is the creepage distance between the relay 'contacts' large enough?
Do you need a snubber network.
A factory-made solid state relay block with screw terminals could be easier and safer.
Leo..
My design with the large pads and vias was to enhance thermal conductivity between the two planes and act sort of like a secondary heat sink as well as make the pads really wide so that current isn't an issue. Is this bad practice?
The picture doesn't show mounting holes because this is only part of the PCB, but yes, I do have mounting holes on the board.
The relay is indeed rated for 25A/480V AC (max specs with cooling fan), but I would only use it for 120V. Check the very top of the first page of the spec sheet again.
The clearance between the 2 planes is 50mil.
I don't actually know the legal distances. Where can I find these rules for PCB's?
I'm not sure what you mean by "the creepage distance between the relay contacts" since this is an opto-isolated solid state relay without physical contacts. The DC input pins are the two holes at the bottom, in line with the larger ones at the top (the AC out pins).
Do I need a snubber? I wouldn't think so, but I could be wrong.
androidfanboy:
Is this bad practice?The clearance between the 2 planes is 50mil.
I don't actually know the legal distances. Where can I find these rules for PCB's?
I'm not sure what you mean by "the creepage distance between the relay contacts" since this is an opto-isolated solid state relay without physical contacts. The DC input pins are the two holes at the bottom, in line with the larger ones at the top (the AC out pins).Do I need a snubber? I wouldn't think so, but I could be wrong.
Up to you.
Maybe just ok for coated tracks in a clean environment.
Don't know. Google it. Relay contact or triac, there is still full mains there when the relay is off.
Primary/secondary should be much bigger clearance. I use 4mm minimum (230AC).
Snubber or not depends on the load you're switching.
Are you sure you need a zero-crossing type relay.
Leo..
Hi,
What load are you switching with the SSR?
Tom...
Ok thanks, I will increase the spacing.
The relay will be used to switch a toaster oven, so I'm expecting only up to 10A.
And you're right, I probably don't need a zero crossing relay, although the reason I chose it was because it's cheaper and it has that functionality, so I though "why not" lol.
The online calculators are assuming an infinitely long trace. If you have pads or blobs on the trace, then they will act like extra heat-dissipation area. "Heatsink" in other words. The legs of your components may be significant contributors to the heat dissipation if the trace is really short.
"Creepage" is an allowance for dust and moisture deposited on the board, which assists mains voltage to jump gaps that it would not normally jump. The ultimate separation is to route a slot in the board so nothing can stick there and encourage the sparks.
