Connecting GND Pads on PCB - are thermal relief necessary?

[Saimoun]

Hi

Quick question: I know it is common practice to add thermal relief on GND pads on PCB (see picture below f.x.), are these only for hand soldering?
Because if the board is going through a reflow oven well then the whole GND plane will get hot, with a without the thermal relief, then it does not matter, correct?



Thank you!
Simon

[Siwastaja]

I use thermal reliefs on MLCCs in such places because MLCCs, especially larger sizes, are prone to cracking if you look at them the wrong way; hence, I have chosen to follow all manufacturer advice, and that includes using thermal reliefs.

(If you ever hand-solder the parts, the more important this becomes.)

You are right though that, especially in the presence of unbroken ground plane just below, the board heats up quite evenly (and cools down evenly as well) regardless of the reliefs, so you may get away with it.

You may also want to reduce that trace width right before entering the pad, creating a thinner "neck" as a relief as well.

The reliefs you show are so thick though they are not doing much.

Definitely avoid extreme differences between pads: this is, one pad in ground plane without reliefs, and another connected to a thin trace; especially if there is no plane right below. Otherwise, it's very likely you'll see tombstoning.

Usually you would want to place ground vias as close as possible, but these are contradicting goals regarding electrical and manufacturing.

[T3sl4co1l]

And you should use much finer spokes than shown -- 10 mil (0.25mm) would be fine for a 0805 chip, unless it's carrying tremendous power (say a current sense resistor, or resonant capacitor).  The thermal resistance is easy enough to calculate: take the thickness of copper, width and number of spokes, their length, and the thermal resistivity of copper.  Mash them all together (use unit analysis) and you'll find it's really quite negligible for most purposes.  (The trick is, soldering delivers much higher heat flux than the components dissipate, hence the temp rise can be useful for soldering, but isn't very important in circuit, most of the time.)

Likewise, trace neckdown can be a good idea.  Again, tombstoning can be a hazard.

Tim

[Saimoun]

Oooh ok, thanks!! I'm happy I asked, I did not think about stuff like that!
Do you mean having pad connections not even would get temperature differences between the two pads during soldering and therefore could get the MLCC to crack? But if it is in a reflow oven the whole board would be more or less at the same temperature, would it not?

Good point about the bottom layer ground plane - in my case it only has very few cuts.

I keep hearing stuff about large (physical) size MLCC cracking easily - in one of my designs my biggest is a 0805 4.7uF, would it be worth it replacing it with a 0604 then? (taking into account the drop of capacitance with a DC offset)

[Siwastaja]

Google "smd tombstoning". The smaller the part, the higher the risk of tombstoning; opposite of cracking.

0805 isn't a high-risk item for cracking. Just follow all advice, i.e., avoid board flex, don't place mounting holes nearby, avoid excessive hand soldering temperatures or slow hand-soldering practices. 1206 and bigger are getting more risky and give less room for forgetting any of said rules. If in doubt and have budget, buy soft termination capacitors but I usually don't care for 0805 and smaller. Cracking is cause by mechanical stress either during use, or during soldering caused by quick temperature change, or spatial temperature difference within the part, which is why hand-soldering one pad at a time is a potential risk.

IMHO, failure to add thermal reliefs in a project to be purely reflowed (not reworked with soldering iron), is very unlikely to cause cracking alone, but given that manufacturer appnotes about avoiding cracking recommend using the reliefs, I like to follow this suggestion.

[T3sl4co1l]

Heh, for that matter, manufacturers usually recommend against soldering iron entirely.  Partly because of the intense heat stress, partly because solder is so much harder to control (my joints almost always end up blobby..).

And you can get away with it a hundred times in a row, sure -- but who knows.  This is the sort of thing that production must know, and know very well: a failure rate less than one in a thousand, or ten thousand, say.  So they'll recommend against using an iron.

All the same, if you're doing it by iron and don't have hot air or preheat or anything, you're going to want thermals just so you can solder the stupid thing.  Especially on heavier copper (>1oz).  Don't forget a generous toe fillet area, too!

BTW, the board may not actually get all that hot -- especially one with internal planes, thermal vias, etc.  Those take a long time to heat up.  You can easily do hot-air reflow without melting anything on the opposite side, for example.  (Oven reflow should tend to melt everything, but the temperature in the middle of the board could still be below melting.)

On a related note... I never did understand how SMT electrolytics are supposed to work.  Utterly huge thermal mass, very little soldering area exposed to the heat.  Can those only be melted by through-heating the board, or what?  I can see vapor-phase might work, but I don't see how hot air or IR would.  I've tried using hot air once or twice, and it looks really sketch...  When I'm building prototypes, I always use an iron on them.

Tim

[Siwastaja]

I think the SMD electrolytics rely on the fact they have fairly long leads so that a significant part of the leg, where it is bent, does not even touch the pads but is hidden inside the black plastic thing. Given relatively thin leads and some distance to the core of the capacitor, the capacitor itself doesn't need to heat up, also protecting the electrolyte from excessive temperatures.

I tend to use SMD electrolytics in a home-brew prototyping reflow process combining preheat from below and local hot air gun from above, and don't have any large issues with SMD electrolytics, but they do require a bit of attention because they seem to reflow a few seconds later than the other parts in the vicinity.

[Saimoun]

Alright I am so happy I asked!! I had never heard about tombstoning before (quite a funny name I gotta say  ). Thanks so much guys.

Just FYI - I am asking for a project that will go to a manufacturer: all SMD parts will be soldered through a reflow oven, most TH parts using wave soldering, and the last few TH will be either hand-soldered or done with a robot. So no hand-soldering of SMD parts.

But then I have a following question: when it comes to capacitors between VDD and GND, I often have really large traces for VDD (for example 30 or 40 mil - simply because if there is space then I think why not making the trace bigger?), and then when this trace gets through the MCU supply caps (f.x.) I like to keep it very thick - i.e. it takes the whole width of the pads on a small 0402 cap, and similarly the GND plane I tend to keep thick connections. I do this because I think it will "help" the current to go through (lower impedance) - are you saying I could simply connect all of them using a 10mil VDD trace and 10mil spokes on the GND?

Said in another way, with the attached pictures: I would usually do "1.png", thinking that it will be the best for the electronics, but you're saying I should do "2.png" because it will not impact the electronics (or very very little) but will help manufacturing?

Just FYI:
1) on the pictures: the MCU is at the top left (QFN package), the three bypass caps are 0402, 0402, and 0803. Following the +3V3 there is another 0803 cap and the LDO. On the "2.png" all pads are connected with 12mil traces.
2) in my case I am only dealing will low currents, the +3V3 will have 100-200mA max, and most traces will be under 20mA.

[ogden]

I think the SMD electrolytics rely on the fact they have fairly long leads so that a significant part of the leg, where it is bent, does not even touch the pads but is hidden inside the black plastic thing.

They inevitably heat up-to reflow temperature (that far exceeds electrolyte boiling temp BTW), may bulge. Plain electrolytics in reflow oven is risky pain in the *ss, especially when you have high thermal mass components as well on the board. You have to be really careful about reflow temp profiles, read component reflow soldering specs carefully. If you can afford - get rid of SMT electrolytics, use other caps that don't boil.

[Siwastaja]

10 mil spokes in thermal reliefs are OK because they are so short. Say, the resulting relief is like 10 mil x 10 mil square. It has the same resistance as any other square on the PCB (say 1 inch x 1 inch square for example).

The same applies to the power pin bypass caps: say your 0.5mm QFP pad is just 10 mils wide, you go from there with a 10 mil track directly to the pad of a 0402 capacitor, but the length of that trace is maybe just some 50 mils. There, from the cap, you can start again with 10 mil width for the first say 20 mils creating a neck, then widen the track.

For resistance, it's really the aspect ratio which matters. A 100-mil long 10 mil wide track is equal in resistance to a 1000-mil long 100-mil wide track.

Inductance is a bit trickier, though. I recommend playing around with wire / loop inductance calculators available on the interwebz.


Personally, I try to keep the width of power traces entering the passives some 60-70% max of the pad width. Say the pad is 1.5mm x 1.0 mm; so I use maximum track width of some 1mm or 0.7mm depending on which side I enter. But such rules are not set in stone, but highly personal. The idea is to limit the amount of thermal heatsinking.

For thermals in plane, I normally use 4 spokes 10 mil in width, 8 to 10 mil separation from the plane, but if I feel like this is some super critical super low inductance high current loop I might add a few extra spokes on the direction of the expected current flow, so maybe have 6 such spokes instead of standard 4.

[Siwastaja]

I think the SMD electrolytics rely on the fact they have fairly long leads so that a significant part of the leg, where it is bent, does not even touch the pads but is hidden inside the black plastic thing.

They inevitably heat up-to reflow temperature (that far exceeds electrolyte boiling temp BTW), may bulge. Plain electrolytics in reflow oven is risky pain in the *ss, especially when you have high thermal mass components as well on the board. You have to be really careful about reflow temp profiles, read component reflow soldering specs carefully. If you can afford - get rid of SMT electrolytics, use other caps that don't boil.

I haven't had any such problems. This being said, I'm using leaded paste in prototyping for added process margin, and when I subcontract, the CMs should know how to set up the process. As a result, I haven't seen what you describe at all.

To compare, I have seen problems with some plastic connectors; most are just fine but some specific ones despite being rated for reflow require very careful control of parameters.

[Saimoun]

I think the SMD electrolytics rely on the fact they have fairly long leads so that a significant part of the leg, where it is bent, does not even touch the pads but is hidden inside the black plastic thing.

They inevitably heat up-to reflow temperature (that far exceeds electrolyte boiling temp BTW), may bulge. Plain electrolytics in reflow oven is risky pain in the *ss, especially when you have high thermal mass components as well on the board. You have to be really careful about reflow temp profiles, read component reflow soldering specs carefully. If you can afford - get rid of SMT electrolytics, use other caps that don't boil.

Well that would explain why JLCPCB does not do any SMD electrolytic caps - clearly they do not want to go through the issues of putting them in the reflow oven

And Siwastaja thanks so much, I never thought about it this way - it makes sense now! So it's still a good idea to go very large (40+ mil) on my relatively long traces, but with a thinner "neck" on the pads. And for short traces I can basically keep them thin.

0805 isn't a high-risk item for cracking. Just follow all advice, i.e., avoid board flex, don't place mounting holes nearby [...]

Sorry this is off-topic but I'd like to pick your brains on it: I actually have 2 push buttons about 150mil down of the LDO output cap. I tried to solve that by putting a mounting hole right between the two buttons, thinking the screw will prevent the board from flexing when the push buttons are pressed - I guess I forgot to take into account the small tolerances on the sizes (case+stand off for the screw f.x.) which could make the screw bending the board a little?

[ogden]

Sorry this is off-topic but I'd like to pick your brains on it: I actually have 2 push buttons about 150mil down of the LDO output cap. I tried to solve that by putting a mounting hole right between the two buttons, thinking the screw will prevent the board from flexing when the push buttons are pressed - I guess I forgot to take into account the small tolerances on the sizes (case+stand off for the screw f.x.) which could make the screw bending the board a little?

Mounting hole also can be source of flex. You may consider soft termination MLCC cap. Other way of board flex isolation from sensitive components - slit. Any chances we can see layout pic? Many manufacturers have appnotes about MLCCs. Murata for example. It addresses pad layouts as well.