DC-DC Converter layout feedback - Page 1
Forum section: electronics / projects

author: Spikee
author_rank: Frequent Contributor
timestamp: March 06, 2013, 09:44:26 am
content: For a new project i want to use a DC-DC converter to get the voltage from 4 18650 lipo's to 5V 1A.I used TI Webench to select the appropriate components and.The input Voltage is 10.0 -> 18V (lipo cutoff is 11V , Full is 16.8V)Output voltage 5V 1ADatasheet:http://www.mouser.com/ds/2/405/slvsa13e-120867.pdfWebench design :https://dl.dropbox.com/u/100819959/DC_DC/webench_DC_DCpdf.pdfSchematic:Recommended layout (datasheet) :Pcb Layout:Did i make any mistakes ?Also if i decided to get another DC-DC Converter for the 3V rail will that cause any issues?It will be connected to the battery.Thanks , Spikee !

author: CarlG
author_rank: Regular Contributor
timestamp: March 06, 2013, 03:26:35 pm
content: The feedback should come directly from the output cap C2, so I would suggest:1) rotate L1 90 deg clockwise2) rotate C4 90 deg clockwise (to reduce the current loop)3) remove the GND vias in the lower right corner and place them below C44) move the +5V vias down (where the GND vias were) and place them below C4, beside the GND vias5) route the feedback wire and the wire to VOUT directly from C2 (give some space to L1)6) place C3 right beside R2Also, I would give priority to the feedback node; minimizing the VFB node. The PGOOD resistor R1 node is not sensitive.

author: Spikee
author_rank: Frequent Contributor
timestamp: March 07, 2013, 01:21:38 pm
content: I did the layout again using your feedback and i come up with this.I took the Feedback and Vout line together because they go to the same place.Is that correct or is it important that they are separate traces ?Top view pcb:3D top view pcb:3D bottom view pcb:The feedback line seems a little bit long if you ask me ...Thanks !Spikee

author: jerry507
author_rank: Regular Contributor
timestamp: March 07, 2013, 04:46:05 pm
content: Rotate your inductor 180 degrees and move the output filter cap with it. It will be fine the way it is, but making this change would improve output voltage accuracy and regulation slightly.

author: Spikee
author_rank: Frequent Contributor
timestamp: March 07, 2013, 06:05:50 pm
content: So i took your feedback in consideration and this is the result:Now i need to get a trace from Vin to a connector and the HIGH pin.Can i run those under the DC/DC converter or will that cause problems ?Thanks!Spikee

author: jerry507
author_rank: Regular Contributor
timestamp: March 07, 2013, 07:43:10 pm
content: If it's more than 2 layers, go ahead. If not, move your connector to the otherside. Your enable line can be pretty long, it's not a particularly important signal.

author: CarlG
author_rank: Regular Contributor
timestamp: March 07, 2013, 10:12:00 pm
content: QuoteSince they've indicated separate traces in the functional diagram as well as in the layout suggestions it sure will make some difference. I haven't read the datasheet to find out what pin 1 actually is for, except that it's used for Ton adjustment, but obviously it seems to interfere with the regulation, or the other way round, that the voltage drop in the FB trace disturbes the Ton adjustment.Naturally, there are at least as many opinions as there are EE, so of course I'm of a different opinion than jerry507 %-BThe last two layouts suffers from the same problem as the first: the FB is not taken directly at Cout, as I pointed out before. With due respect, I would prefer the second layout, but rotate & move Cout so it comes below L1. And place the FB tap right a CoutThen it's also possible to lower L1 and move it a bit closer to the regulator. If you have the possibility to make more than one PCB you could learn some from comparing them (and also tell us the performance of each). Allow as much as possible space between the traces from Vout and L1 & C1 to avoid noise pickup..The last (third) layout has much bigger current loop that the previous ones, resulting in more noise. Think of where the current flows: From Cin via the regulator switch, through L1 and Cout back to GND of Cin (in the ON phase). In the OFF phase from GND of the regulator via the internal switch, L1 and Cout back to GND at the regulator.The least output voltage ripple is at Cout, so that's where you should feed the rest of the circuitry from. And I mean right at Cout, not a few millimeters away from it. There's no gain in separating the GND and +5V vias.Note also Fig 13, and how signal signal GND and power GND are separated. You can move C5 a bit to the left, rotate R3 90 deg CCW, route the trace from pin3 between R3 pads and route a trace from R3 via C6 to signal GND (pin 5). Finally, instead of put a trace directly from pin 5 to the power GND under the IC, I would connect pin 5 to the reference GND plane with a via and tie GND of Cout to that reference plane as well. To minimize IR drop from Cout to pin 5 due to the "external" load you can place a cut in the reference plane. But that all depends how the rest of the circuitry is placed.