Is this board solderable? - Page 1
Forum section: electronics / projects

author: ivan747
author_rank: Super Contributor
timestamp: November 24, 2014, 06:32:06 pm
content: I've recently designed a board based on this:https://www.eevblog.com/forum/projects/lt-app-note-'high-performance-portable-dc-bench-power-supply'/msg551258/#msg551258My version of the circuit is very compact, mostly because I don't wanna pay too much for the PCB. By pure coincidence, the board is the size of a credit card. Right now it's costing me $70 at OSHpark.Something that worries me is that maybe I have designed a board that cannot be soldered by handIs this board solderable by hand by using a good Hakko soldering iron? It's 4 layers, the smallest SMD passives are 0603, it has one 0.5mm pitch QFN (to my best knowledge, this one has pins that extend to the sides) and large power planes. Listening to myself I'm starting to think the answer is no, can't be soldered.Maybe some board preheating is needed? Maybe I should add more thermal reliefs? (where?) I could invest in some tips for my FX-888 iron if necessary. Or do I need a hot air rework station? (christmas and yearly bonuses are coming!)Thanks guys

author: ivan747
author_rank: Super Contributor
timestamp: November 24, 2014, 06:35:55 pm
content: Some 3D previews, in case that helps you.You can see that I left some soldermask off in some places, like the bottom of the QFN, for solderability.But, I have a question regarding the D2paks, will those vias suck the solder away to the bottom? Should I leave the bottom soldermask on in this case?Also, remember general criticism is welcomeas well as questionsI can upload files in more formats if you need them

author: Richard Crowley
author_rank: Super Contributor
timestamp: November 24, 2014, 06:40:41 pm
content: Why so small? Why 4-layer?It seems to me that you could achieve that triple-play/hat-trick of:EasierCheaperFasterby giving yourself some working space and using larger components and conventional 2-layer PC.

author: Mr.B
author_rank: Unknown
timestamp: November 24, 2014, 06:54:40 pm
content: I think you will find the QFN almost impossible to solder by hand.The rest of the components are doable but some will be a real challenge.I am assuming that the board needs to be that small for some reason...As Richard said, make it bigger and use easier to solder components.If you really want to go there...Get a paste stencil made by someone like Pololu. (Who I use)Get a frypan.Watch the "Reflow soldering using a frypan" tutorial at the Sparkfun site.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: November 24, 2014, 06:59:36 pm
content: Quote from: Mr.B on November 24, 2014, 06:54:40 pmQFNs are easily hand solderableas long asyou leave at least 0.5mm of pad outside the package outline.If the centre pad needs soldering ( can often be omotted unless needed for heat or RF) this can be doen withe paste & conduction heating through vias from the other side

author: Richard Crowley
author_rank: Super Contributor
timestamp: November 24, 2014, 06:59:42 pm
content: Note that OSHpark also make stencils:https://www.oshstencils.com/

author: Yago
author_rank: Frequent Contributor
timestamp: November 24, 2014, 07:19:47 pm
content: Is hot air and paste viable, for the centre pad?Conduction from underneath preferable?

author: Mr.B
author_rank: Unknown
timestamp: November 24, 2014, 07:38:38 pm
content: Quote from: mikeselectricstuff on November 24, 2014, 06:59:36 pmThat was what I was meaning.Problem solved with the frypan method if you do not have a little reflow oven, home made or not.

author: Mr.B
author_rank: Unknown
timestamp: November 24, 2014, 07:54:41 pm
content: Quote from: Richard Crowley on November 24, 2014, 06:59:42 pmThanks Richard!I have just compared pricing and OSHPark are way, way, way cheaper than Pololu.

author: ivan747
author_rank: Super Contributor
timestamp: November 24, 2014, 08:24:00 pm
content: Quote from: Richard Crowley on November 24, 2014, 06:40:41 pmDo you reckon the QFN chip can be done on 2 layers? That was the main reason for a 4 layer board: a solid ground plane and that QFN package.The original solution was 4 layers using 0603, so I went for that as well, and for cost reasons I started to shrink the design. (And getting it so small was a great exercise in layout too!)I'll look into it when I get home.For now, thanks for the feedback to everyone!

author: ivan747
author_rank: Super Contributor
timestamp: November 24, 2014, 09:00:17 pm
content: Will the vias on the d2paks suck the solder out of the top side?

author: Howardlong
author_rank: Super Contributor
timestamp: November 24, 2014, 09:00:33 pm
content: Quote from: ivan747 on November 24, 2014, 08:24:00 pmDefinitely QFNs are do-able on two layers. The two possible flies in the ointment are (1) getting a decent flood on your ground plane(s) and (2) that the QFN has castellations on the pins. Make sure you have a number of vias under the power pad to your ground plane.QFNs can be a bitch to solder by hand if they don't nave castellations, most do, but some don't. For hand soldering, tin all the pads including the power pad. Use a bit of flux on the tinned pads and the chip itself. Align the chip with tweezers and use a hot air iron on it, and watch under a microscope. The chip should align itself once _all_ the pads have melted.I made a series of videos on hand soldering QFNs about four years ago, including replacing them, see herehttp://youtu.be/bR35paD0od8. This was on a double sided PCB with a non-castellated 0.5mm pitch QFN.Mike at mikeselectricstuff has a video where hdoes it with just a standard soldering iron, I haven't done this myself.Looking at the video, I'd say it looks like I probably used a bit too much flux on there. These days I can swap at a QFN in about five minutes if I have a number to do production-line style, and the yield rate is pretty close to 100%. Typically any fault has nothing to do with the QFN, it's because very occasionally I've accidentally nudged another part out of view of the mocroscope's field of vision.

author: zapta
author_rank: Super Contributor
timestamp: November 24, 2014, 11:17:34 pm
content: Quote from: Richard Crowley on November 24, 2014, 06:59:42 pmNot related to OSH Park but this is a good source for plastic stencils. For 0.5mm pitch metal stencils (e.g. from Elecrow) work better for me. (the plastic holes are not well defined at that pitch).Soldering QFN 0.5mm by hand should be very doable with a cheap stereo microscope from ebay. Without it it's like shooting in the dark for me.

author: ivan747
author_rank: Super Contributor
timestamp: November 25, 2014, 12:19:51 am
content: I prefer to stay away from stencils for now. For a single unit I'd have to buy the stencil, solder paste that goes bad, a rework station, or a frying pan (no I will not solder where I cook).I guess I'll go 2 layers, from OSHpark (their tolerances are better for something like a 0.5mm pitch QFN) and do magic to get a robust layout for the 700kHz, 3A DC-DC converter.Also that's what I should solder first right? (I can get some cheap QFNs and practice on the spare board perhaps).

author: zapta
author_rank: Super Contributor
timestamp: November 25, 2014, 12:24:32 am
content: Use tacky flex sick as chipquick, it does miracles.

author: ivan747
author_rank: Super Contributor
timestamp: November 25, 2014, 12:31:13 am
content: Quote from: zapta on November 25, 2014, 12:24:32 amDo you mean like soldering the QFN using low melting point solder?

author: zapta
author_rank: Super Contributor
timestamp: November 25, 2014, 12:41:37 am
content: No just tacky flux and normal solder. The flux causes the solder to bead nicely and avoid shorts between pads. Tacky flux stays better in place. You can clean it with IPA.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 25, 2014, 03:38:15 am
content: Meh, you can get that on two layers, and probably 30% or more area savings besides. But I'm a layout whiz, so...Tim

author: coppice
author_rank: Super Contributor
timestamp: November 25, 2014, 05:53:20 am
content: Quote from: Howardlong on November 24, 2014, 09:00:33 pmThey are more than just doable. Most QFNs go onto 2 layer boards, except maybe the RF ones. Even there it could well be that most are still on a 2 layer board.

author: Dago
author_rank: Frequent Contributor
timestamp: November 25, 2014, 06:34:41 am
content: Huh? QFNs are dead easy to solder.I just dab tiny bit of paste on the center pad, heat with hot air (no reason why not to have a hot air station nowadays, chinese stations that work cost like 50$) and then just put flux and lots of solder on the pads, swipe with soldering iron over the pads (taking away the excess solder) and done. You can also put paste on the pads when hot air soldering but you still need to swipe with a soldering iron unless you use a stencil and are very carefull in aligning it so I don't usually do it.Pretty much my favorite package because how easy and fast they are to solder.

author: ConKbot
author_rank: Super Contributor
timestamp: November 25, 2014, 11:51:03 am
content: Quote from: ivan747 on November 24, 2014, 09:00:17 pmYesQuote from: ivan747 on November 25, 2014, 12:19:51 ambut who care's as you're hand soldering it. Its only an issue for automated assembly. The problem isnt that the holes will pull solder out of the joint and make it dry(as long as the chips down flat enough, anyway), its that in the oven if the board gets to temperature before the package, the solder can melt, not wet the device, wick though the holes, and leave you with not enough solder to attach the tab well. Line up the package, solder your 7 smaller pins, do the rest of the board, etc, and when you change tip to a big one. Then solder the tab down. If your iron cant get done in < 20-30 seconds (already stretching it way past the usual 5 second 'rule' ) then you need a bigger tip, an iron with more wattage, or to preheat the whole thing. Like any other solder joint, it should be a smooth concave fillet.If you only intend on hand assembling stuff, you can do all sorts of 'naughty' stuff when it comes to unfilled vias in pads.

author: ivan747
author_rank: Super Contributor
timestamp: November 25, 2014, 12:07:07 pm
content: Quote from: T3sl4co1l on November 25, 2014, 03:38:15 amWith components on both sides? I think noise an ground loops would take over.2 layers I can do

author: ivan747
author_rank: Super Contributor
timestamp: November 25, 2014, 12:10:46 pm
content: Quote from: Dago on November 25, 2014, 06:34:41 amThe center pad can be soldered with a soldering iron if you make a relatively large via to transfer heat from the bottom. Someone mentioned a Mikesekectricstuff video that shows that, I think that's the method I'm going to use.

author: ivan747
author_rank: Super Contributor
timestamp: November 25, 2014, 12:13:50 pm
content: ConKbor, thanks for that information. If I were to put this into production I would change the thermal vias in all chips, so that the things you describe don't happen on reflow. I'd get soldermask under the thermal vias so that solder doesn't suck through.

author: TiN
author_rank: Super Contributor
timestamp: November 25, 2014, 01:31:23 pm
content: It's well doable, but make sure you have big 4mm+ tip for your iron. Good thermal contact and surface area is a key.Also for QFN - make pads extend outside more, so you can get tip onto pads and solder that chip on.For center pad - I was used to make a single bigger via under it and then just solder it all thru from bottom side.If you have access to hotair station - QFN would be zero problems as well.I'd prefer to make via arrays more spaced between, so copper pour can go thru those via arrays, uninterrupting plane current flow.Currently your vias near electrolyte are breaking ?-shape power shape pretty nicely just in half.Also nothing wrong with using 4L board, it's really nice to layout when you have ability to toss power delivery to dedicated layers.

author: Dago
author_rank: Frequent Contributor
timestamp: November 25, 2014, 02:56:59 pm
content: Quote from: ivan747 on November 25, 2014, 12:10:46 pmYou can do that too but you need to take that in to account when you're making the PCB (put enough thermal vias and leave out the solder mask). You'll also need a proper soldering iron (=JBC or Metcal) with a big tip, otherwise heating it from the bottom side might prove difficult.

author: chickenHeadKnob
author_rank: Super Contributor
timestamp: November 25, 2014, 06:46:50 pm
content: I know one of LT's claims for this circuit with lt3081 D-paks is an "all surface mount" design, and I can see the desirability of that, but I still would use the more expensive 7 lead TO-220 package. Three of them positioned at the edge of the board so they can be bolted to a proper heat-sink and have some hope of supplying 4.5 amps without thermal problems.

author: ivan747
author_rank: Super Contributor
timestamp: November 26, 2014, 12:34:33 am
content: Quote from: chickenHeadKnob on November 25, 2014, 06:46:50 pmWell, remember it's all preregulated, only 2.5W is dissipated per regulator. I fixed the problem myself with one of these:http://www.digikey.com/product-search/en/fans-thermal-management/thermal-heat-sinks/1179752?k=7106This heatsink heats up 40 degrees above ambient all by itself, at 2.5W. That's a thermal resistance of 16C/W, plus 3C/W on the package means the junction temperature reaches about 48C at maximum power, if we assume a 35C ambient, that'll be 83C, I've seen procesors get warmer than thatIt's not that great, so I added the power planes you see in the layout.

author: ivan747
author_rank: Super Contributor
timestamp: November 26, 2014, 12:53:16 am
content: I'm working on a 2 layer layout, this is what I have so far. It's the DC-DC converter section, 700kHz, must be able to supply 3A, and I'd like it to be as quiet as possible, no conducted or radiated noise (I think it could use a a common mode choke, actually, I'm looking into it).What do you think about the layout? THe thing I like the least is the output capacitors, they need vias in order to make a low impedance ground connection, as you can see.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 26, 2014, 01:35:41 am
content: Looks pretty good. If you still need to cram for space, it seems like there's a bit more pushing you could do, but hey, I'd be happy with that as is.Don't bother with separating grounds, just make sure it's well stitched around all the traces.If you need low noise, you can add extra filtering on the end. That you have input and output nearby is helpful: that limits common mode noise, because you can apply differential filtering to a common ground. Then, your only source of common mode noise is from voltages generated on the rest of the board, which if you surround it with a shield, grounded to the same point as the outermost filters, the current through those capacitances (i.e., voltages on the board --> stray capacitance to shield --> weak noise currents) are also blocked. With a common ground (the shield), wires exiting at one point, and filtered to that point, there's no common mode, only differential. This is the best / gold standard sort of way to go about things.If you had connections exiting opposite ends of the board, even if each signal is perfectly filtered to the ground at that point, you run the risk of the grounds not being equal (due to currents flowing in the ground plane) -- common mode noise proper. Even if you put this example inside a shield box, the common mode noise remains -- you have to pick one ground or the other; even if you short both to the shielding, you've only rerouted the ground current, and the voltage difference remains (somewhat reduced) between input and output lines. You would then need one more (differential) filter stage outside the shield to address the noise.Common mode filtering is tricky on a converter, because for one it's not making much -- it's all common ground, what is the noise supposedly common to? -- and to use a current compensated choke, you need equal DC currents... which means you can't just wire everything together, you need an explicit input +/- that only connects to stuff upstream, and an explicit output +/- that only connects to stuff downstream, with no loop between those two grounds. So your grounding topology has to resemble a tree. Which probably isn't a bad idea anyway, but it's not as simple as chaining devices on a common bus (if you have many boards powered from a common supply) or using chassis ground with a single wire supply routed to the boards (which is also good, but you may want extra inductance where that wire enters the board, to reduce noise coupling from the loop made by that wire to ground).Tim

author: ivan747
author_rank: Super Contributor
timestamp: November 26, 2014, 03:11:59 pm
content: Thanks for the advise, Tim.I just hope that the grounding is alright, as you can see there are vias between the chip and the output capacitors, let's hope they don't add much inductance.I removed the separation between signal and power and now I'm relying on the ground plane made up by the top and bottom layer, joined together with approximately 70 vias.If I got what you said about filtering right, I need something like this:All grounded to the same point in my board, that would be close to the region where the input and output are.And that I could even shield it if I want to make it fancy (I found a place that sells copper clad the other day, so that is a possibility).Maybe it's possible to get rid of all the spikes the original power supply had:I'm really lost at the filtering but I will do my research, don't worryThere are many app notes that deal with this kind of high frequency DC-DC converters and the best of all is that because the frequency is so high, filters are small, the problem is dealing with the little radio transmitter you created along the way