Boost converter and PCB design - Page 1
Forum section: electronics / beginners

author: John80
author_rank: Contributor
timestamp: June 14, 2011, 03:06:43 pm
content: Hello to everyone!I am designing a new PCB these days and I have a few questions. I am going to use a boost converter (Microchip MCP1640) in order to increase the voltage of two AA batteries at the level of 3.3V. The converter works at 500KHz.My PCB will have two layers and since I have too many power lines (GND and V+) I was thinking to create a ground plane at the top and a power plane at the bottom. The power plane will carry the 3.3V output of the boost converter. With this technique I can use small vias to power my ICs (microcontroller, external EEPROM and a few SPI / I2C sensors) but the problem is the noise.Is that a good way to design my PCB or I must have two ground planes (top and bottom) and something like a star routing for the V+?

author: Neilm
author_rank: Super Contributor
timestamp: June 14, 2011, 08:32:56 pm
content: You can't do proper planes on a 2 layer board. The closest you can do are copper pours which may cause you problems at this frequency. A proper plane is an unbroken layer.If you can't make the PCB 4 layers I would suggest having one side as 0V and try to route all the tracks on the top layer. With the converter, keep all the switching tracks as short and as wide as possible. It might be possible to put in local planes around the converter to help - I would definitely put an unbroken 0V fill under the converter circuit.The reason for keeping a plane unbroken is to do with the return currents. Current flows in loops. The return current path for a current flowing through a track is as close to that track as possible. If there is an unbroken 0V later it will naturally return directly under that track. This is because it is the path of least resistance (ideally). Tracks and breaks in it will lead to the return current taking a longer path and therefore be more susceptible to EMC / generate more EMI.For more information I would suggest reading articles by Keith Armstrong. They are available athttp://www.compliance-club.com/. I find his articles easy to understand - they are not physics heavy but explain in reasonably simple terms what is happening. i have found them very useful in my work.I read through these articles (and the book he has produced) a few years ago when I had to retest all the products my company makes due to regulatory changes. Most of the products that failed were older designs using 2 layers. In all but 2 instances the problems were fixed by adding power and 0V layers and having only one 0V throughout the board.Neil

author: John80
author_rank: Contributor
timestamp: June 14, 2011, 10:04:28 pm
content: Thanks for your answer Neilm! It was very helpful!It will be good to have four layers design but this is impossible because of the cost constrains.I must designed the system using only two layers, so I must find a solution...Any other suggestions?

author: Zero999
author_rank: Super Contributor
timestamp: June 14, 2011, 10:41:43 pm
content: Is it possible to put two planes on the bottom layer?You could then have make the power tracks as thick as possible on the component side, using multiple vias for the same track if needs be.

author: John80
author_rank: Contributor
timestamp: June 15, 2011, 09:42:10 am
content: Yes I can use two copper pours at the bottom.It is not possible to have a top and bottom GND copper pour for the switching power supply and a separate top and bottom ground copper pour for the digital part? After that I can connect the two ground copper pours together with ferrite beads...

author: Neilm
author_rank: Super Contributor
timestamp: June 15, 2011, 08:06:23 pm
content: Quote from: John80 on June 14, 2011, 10:04:28 pmHave a look around that site for an article from Keith Armstrong called "BOM cost vs profitability" The gist of the article is that the delays and subsequent fixes costs a lot more than spending a bit more at the start. It was in issue 82.A case in point was on the retest work I mentioned earlier. The instrument was a reasonably new one that had beendelayed for some time due to EMC issues. In order to get it to pass the original EMC requirements, the designers had to add a ferrite to a wire in the instrument. There was no way of fixing it as it was very large so it was just stuck down. As it got banged around the glue came loose and the ferrite ended up shattering and the users complained it rattled. Also, a large external ferrite was required on an external lead. Total cost of the ferrites - £3 in round figures. After I revisited the 0V I was able to replace both of these ferrites with a very much smaller one that could be secured. Cost of replacement ferrite £0.62. I don't know how many we shipped during the years but the money wasted adds up very quickly.Eventually you might have to put this to whoever is saying "no 4 layer PCB". If you need tips on how to phrase it for a manager who does not understand good practice I would suggest you read "Getting what you want" on page 19 of issue 77. You might be able to get away with only two layers (in which case well done) but if you have to go and do a redesign / respin and retest you will hold up the project.You might be interested to know that the fallout from the re-test work I did now means the PCBs now designed are 4 layer minimum, unless there is a pressing reason to make it dual layer.Neil

author: ejeffrey
author_rank: Super Contributor
timestamp: June 16, 2011, 10:52:13 am
content: I would recommend no ground plane / copper pour around the converter. It isn't needed, adds unhelpful parasitic capacitance, and can lead to lots of switching hash entering your ground and possibly causing problems with the rest of your circuit. The extra trace inductance should be negligible in a boost converter as long as you provide a reasonable return path from the ground side of the switch back to your input cap. It might make radiated EMI slightly worse, but the main source of EMI from a SMPS is magnetic fields from the inductor which is not shielded at all by a copper pour. As long as your device goes in a metal enclosure you will be fine.Keep all the switch-mode converter stuff in its own section of the PCB separated from the digital circuitry. If the converter is really noisy, you may have to replace the output capacitor with a capacitor-inductor-capacitor "pi" filter where the supply goes to the MCU section. On the MCU side you ideally want a 4-layer board with complete power and ground planes on the inside and signals on the outside. Failing that, try a complete ground plane on the bottom and all your traces on the top. Unfortunately, this is rarely possible for digital applications. Almost always at least a few traces need to cross, and you can't do that without cutting into your ground plane -- at which point it is not really a ground plane any more. What to do then depends on your speed, your noise immunity requirements, and what EMC requirements you have to meet. Options include wire links to jumper traces, getting rid of the ground plane and using a ground pour in unused space, close your eyes and pay for 4 layers, or abandoning the project. Jumper wires deserve special mention: they are usually considered unacceptable in a production product, but it is perfectly acceptable to have a few in a prototype or one-off, especially if you know you are willing to pay for 4 layers when you go to production.