Boost converter not maintaining voltage under load - Page 1
Forum section: electronics / projects

author: Jay1011
author_rank: Contributor
timestamp: December 11, 2016, 10:49:55 pm
content: I've just implemented on a PCB a boost converter based on the Microchip MCP1642. Its input is a single-cell LiPo and it is configured to boost the ~3-4V input to 5.2V.Under no-load (or minimal load of perhaps a few mA), the output voltage is dead on.However, I find that when I draw ~250mA from the converter as ~125mA continuous and another ~125mA switching on and then off every 250ms (blinking LEDs), the output voltage drops to ~4V, the MCP1642's "power good" (PG) output negates, and nothing short of turning off power and then back on again will restore proper voltage regulation.I have several theories as to what might be going wrong, and I'd appreciate any comments:(1) The inductor I've selected is not up to the task. It's a Bourns 4.7uH SRN4018-4R7M, rated at 84mohm DCR and 2.0A saturation current. This seems to be in line with what the MCP1642 datasheet calls for, but perhaps I'm missing something.(2) My PCB layout is inducing oscillation. I'm hand soldering the board, and so I have not placed the inductor, output caps, and MCP1642 itself as close together as might be desirable, but I don't think it's a terrible layout either and I'm not really sure whether this is a real concern at this output current.(3) The LiPo can't supply enough current to the MCP1642. It's a 900mAh LiPo, and for 250mA output at 5.2V with 85% converter efficiency, that's around 400mA from the battery, or about 0.5C. I believe that should be OK, but perhaps not.(4) I have too much output capacitance and/or not enough input capacitance. I've got one 10uF X7R ceramic on the input and three 10uF X7R ceramics paralleled on the output. Again, this is in line with datasheet recommendations.(5) The ~125mA current steps as the LEDs turn on/off cause oscillation or some other problem.Any thoughts are much appreciated. Alas, I am at the moment limited to just a voltage meter for my "lab equipment" -- no scope, etc. -- so my debugging ability is limited.

author: IanB
author_rank: Super Contributor
timestamp: December 11, 2016, 10:58:35 pm
content: If you suspect the LiPo, have you tried testing with an alternate source of power? For example, two D cells in series will give you a voltage similar to the LiPo at the end of its discharge curve and should easily supply 1 A or more without too much voltage sag.

author: trophosphere
author_rank: Frequent Contributor
timestamp: December 11, 2016, 11:23:05 pm
content: Another thing to consider is the current handling capability of your wires/traces. I know it's kind of a "have you tried turning it on?" type of question but just to be complete. It would also be good to have an additional data-point of how much current you are actually drawing from the battery by using a shunt resistor and seeing the voltage drop with your voltmeter. A value that is way out of bounds than what you have calculated could give a hint as to what is going on.

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 12:52:21 am
content: Thanks.Traces are all 0.5mm wide in 1oz copper on a 2-layer board, and no more than 50mm long, which according to the web-based trace width calculators I've found should easily handle up to 1A of current.I will try swapping 2 D cells for the LiPo; good suggestion. I may be able to use a bench power supply at my workplace as well, which should yield a similar experiment.

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 01:38:15 am
content: I just tried powering with 3 AA cells with an open circuit voltage of 3.55V. The result was the same -- the MCP1642's output drops under load, with its power good output negating just as I mentioned in the original post. Hopefully this is roughly the same as trying 2 D cells; a AA cell should be able to supply 500mA of output current, I believe.

author: IanB
author_rank: Super Contributor
timestamp: December 12, 2016, 02:03:27 am
content: What do you see if you measure the voltage at the input of the converter? Is the actual voltage there what you would expect it to be?

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 02:23:36 am
content: @IanB: Well, I can't actually probe the converter's input pin because the MCP1642 is a 0.65mm pitch part and I'll no doubt short several pins together if I try to probe it.That said, I do have a testpoint available at the battery output, with the battery output connected directly via PCB trace to the MCP1642 input pin.Using that testpoint and again using the original LiPo battery, I see 4.06V open-circuit at the battery output (i.e., with the LiPo connected to the boost converter but the converter powered off).When I turn on the circuit in the ~250mA mode I described above, I see the battery output varying from 3.98V to 4.02V as the LEDs blink on and off. All of this seems reasonable to me.

author: georges80
author_rank: Frequent Contributor
timestamp: December 12, 2016, 05:27:01 am
content: 1MHz switching speed needs good layout. Inductor to switcher needs to be large flooded copper right to the pins. Ditto for the input/output caps.Let's see the actual layout - pics of your board...cheers,george.

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 02:16:42 pm
content: @georges80 -- Layout (from Eagle) attached, I hope. From your comments, I suspect there is ample room for improvement.U2 is the MCP1642 boost converter. L1 is the inductor. C5 is the 10uF input cap. C6/C7/C8 are 10uF output caps; C9 is a 1uF output cap; C10 is a 0.1uF output cap. RTOP and RBOT are the resistor divider to establish the output voltage.All passives except the inductor are 0805. All the thick traces are 0.5mm wide.

author: georges80
author_rank: Frequent Contributor
timestamp: December 12, 2016, 07:29:27 pm
content: Yeah, that layout is not good (sucks actually). You need to consider the high current switching paths and return paths including feedback sensing if using the adjustable part.Go look at the datasheet ->http://ww1.microchip.com/downloads/en/DeviceDoc/20005253A.pdfPage 19 shows a recommended layout - read/understand that page carefully and implement that routing as much as possible.Switchers require attention to detail in the layout, it's not sufficient to just get continuity between the various nodes... Think of the layout as more an RF project...cheers,george.

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 07:45:36 pm
content: Yes, I saw that suggested layout and did not appreciate that it was actually critical on this part. I will be respinning the board for several bugfixes and will attempt to redo the MCP1642 section to match the suggested layout as closely as I can given that I need to solder the components by hand.Much thanks.

author: suicidaleggroll
author_rank: Super Contributor
timestamp: December 12, 2016, 07:58:40 pm
content: Quote from: Jay1011 on December 12, 2016, 07:45:36 pmI don't understand why that's a hindrance. What about hand soldering keeps you from getting the parts closer together? I build almost all of my boards by hand at least once, anything that's too close for hand soldering would likely be too close for automated placement as well, and you can go MUCH tighter than what's shown on your layout. The recommended layout shouldn't be a problem at all.

author: mariush
author_rank: Super Contributor
timestamp: December 12, 2016, 08:27:06 pm
content: The layout is horrible. Look in datasheet for a start.Also pay attention to the ceramic capacitors you pick, make sure they're rated for 25v or higher, pay attention to how those particular capacitors you choose behave when it comes to voltage ( seehttps://www.maximintegrated.com/en/app-notes/index.mvp/id/5527)

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 08:33:45 pm
content: I certainly can get the parts closer together, but in the end (a) I'm soldering the parts with an iron rather than using paste and a reflow oven/skillet, which means I need room to physically get the iron tip next to all the pins/teminals of each part; and (b) I'm using 0805-sized components because I have a ton of those on hand, and my experience with suggested layouts (though perhaps not this one) is that they assume 0603 and often 0402 components are acceptable. Not great reasons, I'll admit, but in all honestly I tend to do simple boards and -- until now -- have not been burned by layout issues.

author: Jay1011
author_rank: Contributor
timestamp: December 12, 2016, 08:53:21 pm
content: @mariush -- Interesting app note; thanks.

author: KL27x
author_rank: Super Contributor
timestamp: December 13, 2016, 06:47:22 am
content: Heh. I have copied layout exactly from datasheet down to number and placement of vias. Trying 3 different boost IC, and using (sometimes very expensive) recommended parts, I have yet to reach much more than half of max sustained output, yet, on any of em.Fastest solution... use boost IC rated for at least twice what you need.*Curious how bad can my pcb design and part selection be? I asked on forum to see what % of performance other people get out of these things. No one responded.. I have one other data point, now.

author: Jay1011
author_rank: Contributor
timestamp: December 29, 2016, 04:44:54 pm
content: Original poster here. I wanted to follow-up on this in case someone finds it useful in the future.I redid the PCB, taking into account the advice in this thread: (a) I closely followed the suggested PCB layout from the MCP1642 boost converter datasheet (per several comments above); and (b) I switched to 1206 size capacitors for the 10uF input and output caps (per mariush's comment above).Result: the revised board works great -- the boost converter maintains the desired output voltage (5.2V in this case) under loads of up to 400mA, even when ~50% of the total load is switching on and off every 250ms (blinking LEDs).I am attaching screen shots of the relevant area of the revised layout in Eagle and of the board plot generated by OSHPark.Thanks to all for the help. Perhaps my New Year's resolution should be to take suggested PCB layouts in the datasheets more seriously