Thermals on ceramic caps in SMPS

near's LTC3810, the other using Micrel's MIC28304. The manufacturers' demo boards and recommended layouts for these devices do not have thermals on c eramic caps which handle high rms currents. The pads for these caps are op enings in the solder mask over large, continuous copper planes. The caps a re 1210 size. My assembly house said they had no problem hand soldering th em, and the joints looked nice and shiny. I would always put thermals on s maller parts; but is there any reason to have them on these larger parts wh ich have to handle large rms currents?

Hi Andrew, (I always enjoy your rare posts.) By thermals, do you mean big pours of copper on the ends of the cap? (If so I might worry about stray C. But I'm most clueless about SMPS.)

George H.

Linear's LTC3810, the other using Micrel's MIC28304. The manufacturers' de mo boards and recommended layouts for these devices do not have thermals on ceramic caps which handle high rms currents. The pads for these caps are openings in the solder mask over large, continuous copper planes. The caps are 1210 size. My assembly house said they had no problem hand soldering them, and the joints looked nice and shiny. I would always put thermals on smaller parts; but is there any reason to have them on these larger parts which have to handle large rms currents?

I'd assume he means the "spokes" that makes it easier to solder because of the smaller thermal connection between and a plane

-Lasse

g Linear's LTC3810, the other using Micrel's MIC28304. The manufacturers' demo boards and recommended layouts for these devices do not have thermals on ceramic caps which handle high rms currents. The pads for these caps ar e openings in the solder mask over large, continuous copper planes. The ca ps are 1210 size. My assembly house said they had no problem hand solderin g them, and the joints looked nice and shiny. I would always put thermals on smaller parts; but is there any reason to have them on these larger part s which have to handle large rms currents?

ermals.jpg

Duh, Yeah so how much inductance from the spokes?

George H.

But the spokes reduce the thermal conductivity of the vias to the power planes.

We never do spokes. We "flood over" all plane connections. For parts that have high currents, it's good to put power pours on the topside and use multiple vias down to the planes. Less R, less L, less thermal resistance.

If a capacitor is going to get hot from too much AC current, it is a good idea to add more caps in parallel! The output of a beefy switcher should have multiple output caps anyhow, to keep the ESR and ESL down.

Trivial, compared to what's soldered in there.

Thermal reliefs on ground pads helps a lot with soldering through-hole parts. Otherwise it's easy to get cold joints or even wetting failures.

With reflow soldering, thermal reliefs don't do much except make rework easier, ISTM.

Cheers

Phil Hobbs

That's my understanding too. Thermal reliefs are not necessary for modern production lines (including rework), but make things easier if you have simpler, cheaper or older equipment (or simpler, cheaper or older technicians!).

The spoke lengths are too short to make a measurable difference to the inductance except for the most demanding of high-speed boards, and the increased DC resistance is also seldom relevant. But (fairly obviously) the thermal reliefs reduce heat conductance from the component into the board and its power planes, which might make a difference.

Makes very little difference. If you actually run the numbers.

Main downside is probably that you need to make the polygon extra large to get enough spokes in it (>= 2, say), if you're doing a local blob that is.

Large pours with solid, oversized pads tend to vacuum up parts as the solder melts, leading to incomplete joints and tombstoning.

Pad connects should be similar in width for both pads. So you want to avoid four spokes (or direct, none at all) on one pad and a teeny 10 mil trace on the other pad. Better to have two or three spokes and a 20 mil trace, necking down to 10 mil.

Also better to avoid lateral asymmetry, lengthwise pad exits are better than sideways. And traces exiting through corners are better than sides.

Tim

Our boards go through a 7-zone reflow oven with a carefully controlled profile. By the time the solder melts, the board is basically isothermal. And a Metcal iron has no problem melting solder for rework, even on a solid copper plane.