Where can I find more information on how make good layouts for boost converters? Is there guide to designing, and sizing trace widths? Where can I find more information component layout? Guide to footprints, and other material?
An old but good AN is “Switching regulators for Poets”.
They must be able to handle the currents.
Trace length and clearance are another issue.
Tracks that radiate noise should short to minimize radiation of noise.
Tracks that are sensitive should be short to minimize noise pickup, and be far away from tracks that radiate noise.
Carefully consider how currents flow through the GND plane. Above a few kHz there is a very strong tendency for return currents to be as close as possible to the “forward” current because loop inductance dominates the impedance and not DC resistance. (Inductance increases with loop area).
Use a search engine with the magic words “hot loop”.
In short: The tracks to the inductor are not the main parts. You have to consider how currents through the PCB change when the SMPS switches. This usually entails the Input filter capacitor, the power switch, and flyback diode. Especially in “continuous mode” the current through the inductor itself and the output filter capacitor does not change very much, and is therefore less important. The power switch and the diode change between zero current and full current on each cycle.
It normally varies but the best source of information it’s normally the datasheet of the part you are planning to use.
I don’t agree with this:
SMPS circuits share the same physics so the same rules apply. A datasheet of a bad SMPS circuit may have a good section with PCB recommendations (Maybe cause it’s mandatory to tame the bad IC?)
I do not have much experience with these IC’s. Apparently there are some quite bad one’s. Maybe because the switch switches a bit too quick, which generates excessive noise, maybe because of bad layout in the IC itself, which may cause internal feedback. For this reason apparently some designers avoid all IC’s with internal power switch.
WRONG WRONG. I do agree that:
See about hot loops. In a boost converter, the output capacitor is part of the hot loop. In a buck converter, the input capacitor is part of the hot loop. There are other important points as well such as gate drive paths. For any low voltage (<50V at least) switching converter, stray inductance is the problem more than anything else, and that the datasheet is usually the best guide for using a given chip.
I like to use track widths which are wide. Generally I use 1 mm tracks for current < 50 mA but of course these need to be narrower in many situations. Copper zones are your friend.
Use generous ground planes. Most switcher IC datasheets will include layout information which illustrates partitioning IC quiet analog ground from noisy power ground. Doing this is often not necessary if your current is not too high, but doing it is better than not doing it and wishing that you had.
Jim Williams is a long revered expert in the world of analog circuit design. But the components have advanced so much since 1987 that I think that much this app note is out of date. Examples of this are many uF of small low ESL inexpensive capacitance in SMT ceramic capacitors, much higher switching frequencies, lower inductance in all sorts of SMT components, lower ESR in polymer capacitors which I think were completely unavailable then. Also a quick scan of the app note showed me no layout examples. Good pcb layout is critical and Ninja_kg0 is correct to be focused on this.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.