Difficulty Soldering Discrete SMD's Connected with Copper Ground Pours

JRetSapDoog

Greetings. I recently soldered up the components for a Propeller-based PCB fabricated with (warning: plug) Seeed Fusion's PCB prototyping service. The board came back in just 8 days and I'm quite pleased with the quality (though I didn't come close to bumping up against the limits of their design rules and only used DIP chips). The board is a mixed/hybrid SMD and through-hole design, with the SMD components all being capacitors and resistors that are only on the bottom side of the board.

When designing the board, I used copper pours on both sides, wherein such pours were connected to the ground network. This means that most pads (both SMD and through-hole ones) that are connected to ground ended up having their pad geometries at least partially "merged" with the ground plane, as expected. My problem is that I had some difficulty soldering these because the copper ground pours have the effect of sinking the heat of the iron. I had to turn up the temperature quite a bit to get the solder to flow. I also applied more pressure and increased the contact time. I used flux, but, surprisingly, it didn't seem to help that much, perhaps because the liquid flux that I used was a so-called "no-clean" flux. And while I did manage to eventually get the solder to flow, my confidence in these joints is less than for others, especially for the grounded through-hole dip pads. Incidentally, the solder was leaded and the PCB had a shiny leaded HASL coating over the pads (as well as solder mask coating for both sides of the board).

So, although the soldering of the pads NOT connected to the ground pours went smoothly, I found soldering the ones connected to the ground pours to be frustrating. I'm sure that part of that is just my inexperience (much of my soldering experience is on home-brew boards that either didn't have ground pours or where the ground pours didn't "subsume" any pads). But be that as it may, I think that, in future designs, I will avoid having pads that touch ground pours by using keep-outs or whatever it takes. I also wonder what difficulty a board assembly house would have soldering such components (larger 1206 parts, not the tiny stuff). I presume that they would end up heating the whole board after P&P, so maybe heat sinking wouldn't be a problem. I did recently purchase an oven and might try this at home (though I don't have a stencil for the current board).

So, the reason I'm writing is that I'm curious as to whether anyone else has experienced this "problem" (quoted since maybe I'm the problem) or if others also avoid having pads "merge" into their ground pours (yes, I should check some designs, though the answer may depend on how one solders the board, by hand or wave/oven). By the way, I used DipTrace to design the board. I guess I'll use a combination of keep-outs or maybe a separate "ground" network somehow (even if I have to trick the software or manually bridge it to ground) if redesigning the current board. Or perhaps I'll hold off on connecting pads to ground until after I've done the pours and then not update the pours (though that seems risky as I might forget to update a pour that needs updating). Maybe DT has a way of taking care of this or I just need to adjust my design steps. But if anyone has any tips, I'd be happy to hear them, as this was my first experience outsourcing board fabrication. Also, if anyone has soldering suggestions for pads connected to ground pours, I'm all ears. But I'm thinking I'll avoid them because they really slowed me down while soldering this go around. Thanks. --Jim

Leon

You need good quality soldering equipment. I don't have any problems with the Metcal system that I use.

Heater.

I think you might have to post some images of how the connections from ground pins to ground planes actually looks. Then I'm sure people around here with experience of PCB layout can comment on it.

I can see the problem though. Copper is a great conductor of electricity, which is perhaps what you need on a ground pin. But it's also a great conductor of heat. Which may mean that a ground pin needs a lot more heat input to solder nicely than all the others.

I'm sure there are solutions regarding PCB layout for this issue.

Domanik

No-Clean is harder to use than the older types of fluxes but it does clean up well with alcohol. I never leave the flux on. The older organic used water as a cleaner and if you mix the two types then try to clean it makes a hard to clean mess. That said, a no-clean solder flux pen is very helpful to make the solder flow easier on pins that have substantial heat sinking.

Another thought is that a flash of gold is harder to solder to than tin-lead finish. This is because the solder-gold area forms an alloy and there is more mixing needed with the gold molecules and the solder. Using a few micro inches of gold plating minimizes this affect while maintaining a non-oxidizing finish for increased shelf life.

The above are minor concerns compared to directly connecting pads to a large copper area. That's a horrific No-No. There are industry rules / manufactures guidelines for the exit of a pad --- you should always use a short trace to thermo-isolate all pads from copper planes, including copper pours.

Component removal, hand rework may be difficult and the risk of lifting a pad is increased with the application of more heat. You want to get a part off quickly without melting the glue between the pad and the FR4.

Duane Degn

Take a look at other PCBs with ground pours and you'll see the pads aren't completely merged with the pour. The pads are separated with a few traces running out to the pour.

I'll open up DipTrace and let you know which settings you need to adjust to get these traces automatically.

Duane Degn

Here's the dialog box for the copper pour.

I like to keep traces thick. I think my 14 mil settings are probably thicker than many people use.



As Leon implies, a hotter iron would likely make it easier to use the board you have.

If you iron isn't hot enough the heat will flow away faster than it's applied. Make sure the tip of your iron is wet with solder to allow good heat conduction.

Publison

As Duane said , a Thermal Relief should be used on the pours:

Here's what it looks like.

http://en.wikipedia.org/wiki/Thermal_relief

tonyp12

The problem is that have is connectivity set to solid/direct and thermal "theft" is making it hard to solder.
If you have to hand solder something you never used solid but 4 spoke.

Use a (dedicated) toaster oven and solder it like real SMT is suppose to be soldered and you will see that the problem is mostly/all gone.

JRetSapDoog

@All: Thanks for wading through my long-winded description and for your comments. And answer-wise, you folks nailed this one! As always, this forum rocks!

@Leon: Thanks. I'm using a Huakko 936A soldering station, but the iron is due for at least a new tip replacement.

@Heater: Thanks for the pic suggestion (see below). You're right about the pours sinking the heat. And you're right that standard layout methods exist to avoid this problem (see below)

@Domanik: Thanks for the "horrific No-No" warning for this novice. So I won't manually connect pads to pours or otherwise try to twist DT. Also, I'll try to pick up a flux pen.

@Duane: Thanks for taking the time to post that DipTrace pic. Although the tab under connectivity looks a bit different for my version of DT (2.4.0.2), I see that I defaulted to the "direct" setting for thermals instead of using some kind of spoke setting. I won't make that mistake again, especially if I plan on hand-soldering the boards. I had noticed this tab before, but the word "thermals" just didn't resonate with me, as I assumed it had something to do with increasing (not decreasing) heat dissipation, such as under a QFN chip with a thermal pad. Anyway, I played with some spoked thermals to see the difference.Yeah, I guessed I glossed over the manual too much on this one. Thanks for being my "manual" on this one, even if that means that I was too lazy or careless.

@Publison: Thanks for the link! That's an informative article. Here's a quote: " A pad directly connected to the copper pour is difficult to solder since the heat quickly leaks away from the pad into the copper pour due to high thermal conductivity of copper." Yep, that's my problem.

@tonyp12: Yes, my connectivity was set to solid, or what DT apparently calls "direct.". And regarding your comment about always using four-spoke thermals (if that's what they're called) for hand-soldered boards, thanks! I will. And thanks for the comment about the toaster oven resolving most of the problem. By the way, I might not use a "dedicated" oven as I like a little lead in my blood stream to keep my valves clean. J/K.




First image shows the Connectivity tab of the Properties for a copper pour. Sorry, I hadn't clicked the "Separate Thermals for SMD" checkbox when I took the screenshot, but clicking it reveals another thermals setting dropdown along with a spoke width box. I'm guessing that this is if one only wants spokes for SMD pads, not others.

Second image shows how pads were getting "swallowed" by a copper pour. In the pic, there's a DIP8 (for an EEPROM) and you can see how the ground pad of the bypass cap got merged into the copper ground pour (sorry, I should have turned off display of components). And below the DIP8, there's a 4-pin header (for the PropPlug) with a similar "problem" (by design, admittedly) on the grounded pin (square one).

Third image shows the use of spokes. These are just quick screen grabs taken while playing with the Connectivity settings. I believe that the clearance from the ground pour is greater than normal/needed, but hopefully you (now) get the idea of how my pads were being "eaten" by the ground pours. [If a pic is worth a thousand words, why do I always neglect to use a pic and go for the thousand-word option, huh Heater? Well, better late than never, usually.]

Thanks for your quick and spot-on responses! This is going to help me a lot if/when I do a redesign (and maybe save me from manufacturing errors caused by unorthodox methodology), as Domanik may have hinted at. Thanks again, everyone!

SRLM

I like my grounds filled in, and haven't had any problems. When you cook an SMD board it will heat everything up relatively evenly, and the components will just drop in place.

If you're soldering by hand I think it's easier to avoid the soldering iron, and just use a hot air iron and solder paste. The trick there is to just watch your part, and like magic it will suddenly slide into perfect position.

I use a Breville 1800 watt toaster with quartz heating elements and a convection fan for my oven. I use a Sparkfun branded hot air gut and a Weller digital soldering iron for manual work.

Tracy Allen

Heat the board from below so that all the components and ground plane come up to about 150°C. Then do your soldering to the ground plane using either an iron or a hot air pencil. I have a heat "fountain" for that purpose, a commercial model, but you could probably rig something up with a heat gun that has a temperature control. Soldering is much easier and puts less stress on the components when the board and components are already hot. SMT ovens generally work by bringing the board to a plateau at 150°C and then raising the temperature quickly up and over the reflow point. The soldering iron should have a good size tip matched to the size of the pad.

kwinn

What Tracy said, and you can also do it with a higher wattage iron. I use a Weller WTCP60 (60W) iron for bigger jobs and have no trouble soldering directly to a copper pour, but not so with my 35W iron.

JRetSapDoog

Thanks for the additional soldering tips, folks. I did read an online review of the soldering station that I'm using. The reviewer stated that the supplied small conical tip was basically useless, and recommended going with a chisel-type one. I have one, so, the next time I solder a board (finished the current one), I'll swap that one in and see if it's more effective. Sounds like it will be (once I get used to it). I also have a cheap hot air station, but I've only used it to remove connectors (and I'm not very adept with it yet). I look forward to using an oven (or griddle) some day (I've seen the videos of surface tension or whatever pulling components into place "automagically"). Step by step, though. I'd be more motivated to try that if I were doing some kind of production, but I should probably test it out (even without a stencil, though I hear that manually dispensing paste is for the birds). @ SRLM, that's quite a setup you've got there! I sometimes wonder about how folks arrange their shops or work areas and stay organized. For example, my soldering station doesn't have a dedicated space big enough for soldering, so I always have to drag it over to my general purpose work table where my light/magnifier is. That's inefficient, but I don't solder that often at present.

JRetSapDoog

By way of UPDATE, I soldered up a new board and didn't have any problems this time, despite the grounded pads being partly embedded in heat-sinking copper pours. I changed the tip on my soldering iron, switching from a cone-shaped one to a chisel-shaped one in the process. And that did the trick. This time around, I didn't need to turn up the temp of the iron, nor use much extra time or pressure. I didn't even need extra flux beyond what is in the solder. Those pads in the pours weren't really problematic at all. I guess my old iron tip was shot (and it was conical).

With this good soldering result, I'm no longer sure that I'd need to use spoked connections to grounded pads for hand soldering (though I very well may). However, if I had a pad all by its lonesome, so to speak, such as a ground pin for a scope in the middle of a big copper pour, then I'd definitely prefer the pad to be connected to the pour using spoke connections. So, anyway, it turns out that the problem was me (due to not keeping my iron in good condition). Sorry if I had you folks scratching your heads wondering why this guy couldn't readily solder those pads. The tip I was using just wasn't doing the job. Aside from being conical, it was pretty cruddy (corroded or whatever) and beyond cleaning.

Although a bit of a false alarm, thanks so much for all the tips. They put me back on the straight-and-narrow path. And I learned how to use the spoked connections setting in DipTrace to boot. Thanks, all, for both the soldering tips and the DipTrace assistance. --Jim