Layout review for buck-converter power supply - Page 1
Forum section: electronics / projects

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 28, 2020, 08:58:41 pm
content: I mentioned in previous posts that I'm building a positive and negative power supply, and the fruits of my labour are almost at hand. After going through the circuit again, I ran some more simulations and (hopefully) things look pretty good. I managed to get a layout going, but I wanted to ask if I could get a roasting (feedback) on my layout.I started out with just a 4 inch by 4 inch plane, and then I thought to move things in closer as I worked on the design. This is the result for now. It's a 2-layer board with ground planes on the top and bottom. I was thinking of just having bottom layer be ground, but since the positive regulator has its tab to ground, I thought it would be better for overall performance if the top was ground as well. I tried following TI's guide about laying out buck converters, so I kept the catch diodes, inductor, and capacitor close together, but I'm a bit worried about the feedback trace length for the positive regulator. For the input power, I plan to use posts so I can just stick some banana plug cables into it and power it from a bench supply. I haven't got to the output connectors yet, but how does it look so far?

author: thm_w
author_rank: Super Contributor
timestamp: May 28, 2020, 11:42:41 pm
content: Positive supply:Put some ground vias on the left and right of U2 and near D2.C11, C12 position could be optimized possibly. Feedback path can be optimized: take from C13, thin trace running back to R4/Rv2.But generally it looks good and you don't have to mess with those last two if you don't want to. Stitch vias are easy to add.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 04:29:42 pm
content: Thanks for your reply. Yeah, I really should put come ground vias to connect the two planes together. Thanks for reminding me of that.There's so much empty space, so I'm trying to move some small stuff around in order to reduce the space, and therefore the cost of the PCB boards.Regarding the feedback path, the issue I have right now is that it starts at one end of the inductor, PCSP, and it has to connect to pin 6 of the IC. The pin placements are rather difficult to route without putting the components closer. How would you recommend routing it from C13? I'd have to move it around, but right now, it's still hanging at the top left unless I re-orient the inductor.Regarding C12, I can move it , but as long as it's connected properly, the sense resistor can just connect to C10 instead of C12, correct? The two caps are parallel, so as long as they are connected at the same node, I can put C12 across from C10 and move the components closer together to save space.

author: free_electron
author_rank: Super Contributor
timestamp: May 29, 2020, 04:41:44 pm
content: ehh . where is the current regulation loop ? you have a limit detector , but you don't use it to fold back the output voltage...

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: May 29, 2020, 05:17:36 pm
content: Further to the comment from free_electron.The way the circuit is drawn, you have LEDs that come on if a current threshold, set by a potentiometer is exceeded. The circuit does not limit the current.In addition the threshold for the negative circuit is proportional to the negative voltage. The higher the negative output voltage the higher the current limit.Regards,Jay_Diddy_B

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 06:06:21 pm
content: The LM2673 and LM2679 have a pin for a current limiting feature, Pin 5. According to the datasheet, it limits the peak switch current through the inductor (and therefore, to the output) when you place a resistor in between that pin and ground:QuoteI was going to place a potentiometer there, but for this first draft, it became too cumbersome, so I settled for a fixed resistor value: 7.8k for the positive regulator and 5.7k for the negative regulator, limiting it to 4.76 amps and 6.51 amps respectively. This is within the current rating of my inductors.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 06:24:53 pm
content: Thanks for your comments. I explained it to free_electron, but the LM2673/LM2679 has a current limiting feature. I'm limiting it through that pin and resistor combo. I initially had a potentiometer there, but I had to use a fixed resistor in order to save space. Perhaps in the future, I'll use one there, but this is what I have for now.Regarding the negative current comparator, since I'm reading in the negative voltages via R7 as my sense resistor, I have to reference the op-amps to the lower voltage in order for it to be within the ranges of the acceptable input voltages. Otherwise, it would be out of range if U4 and U6 had -Vs at ground since I'm measuring a lower potential than ground. As long as both the op-amps and the inputs are referenced to the same low potential, wouldn't that keep the current limit the same? I'm a little confused by what you said.

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: May 29, 2020, 06:31:27 pm
content: Hi,RV6 is connected between Nout and GND, so as the negative output voltage changes, the voltage on the wiper of RV6 also changes.Jay_Diddy_B

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 06:54:37 pm
content: Thanks. I see what you mean, but assuming that the wiper remains untouched at a specific ratio, the ratio would remain the same, so wouldn't that still be okay? The comparator circuit only looks at the difference of the inputs and outputs a high or low voltage depending on whether the difference is positive or negative. If the power supplies just limit the min/max output, isn't that okay?

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 07:01:36 pm
content: Sorry, but if you don't mind having another look, what do you think of this revised positive layout? I tried to take into consideration what you said by first rethinking some placements. I saw on other buck converter modules that input to output was going from left to right. Following that flow, I've managed to move parts around which resulted in a smaller feedback loop as well as shortening the trace of the feedback pin. I had to make the trace to the input capacitors slightly longer with a via, but I used thick traces where I could to make up for that. I also added some square through holes, TP1 and TP2 as places to probe with my multimeter when adjusting the voltage to make my life easier. Hopefully, they shouldn't be an issue.I'm still working on putting ground vias down but what do you think so far?

author: thm_w
author_rank: Super Contributor
timestamp: May 29, 2020, 08:36:45 pm
content: I think you missed uploading the new photos?Quote from: LoveLaika on May 29, 2020, 04:29:42 pmIf its under 10x10cm then the cost will basically not change from the proto pcb places.QuoteI would route a ~6mil trace from C13 or C11 somewhere, back to the potentiometer. Its not critical, but something you may consider in the future:https://techweb.rohm.com/knowledge/dcdc/dcdc_pwm/dcdc_pwm03/4682Quotethink so

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 09:50:16 pm
content: Sorry about that. I thought I attached it. My bad. Here's the new layout. Hopefully it worked this time. To recap:QuoteWhy is it necessary to route from the capacitor instead of the inductor if they're at the same node? Is it because of filtering done by the capacitors? I used 100 mil traces for the inductor and capacitors, but with this new layout, it shouldn't be a problem. I was more worried about the feedback trace between the pot and the IC (Pin 6, that long bottom layer trace).Also, thanks for the link. I'll have a look at it and see what I can incorporate

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 29, 2020, 10:09:32 pm
content: Sorry, I'm an idiot. After reading the link you sent, I see why you said what you said. I'll definitely have to avoid the diode and inductor when routing.

author: thm_w
author_rank: Super Contributor
timestamp: May 29, 2020, 10:17:17 pm
content: Quote from: LoveLaika on May 29, 2020, 10:09:32 pmIts alright, was referring to this part: "The place for detecting the output voltage should be either across the terminals of the output capacitor, or past the output capacitor"Inductor is probably shielded so not sure if that would be much of an issue, as long as you don't go right under it.Depending on current you are outputting (chip says 3A capable), you may want a few thicker traces and a extra via on U2-pin 2.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: May 30, 2020, 04:17:13 am
content: I followed the guide layout from your link. If you don't mind again, what do you think of it now? As you suggested, I took the feedback from the capacitors instead of the inductor, and I went around the inductor on the bottom layer to the feedback pot RV2 which shortened the loop significantly.One thing that kind of worries me is the negative feedback loop. Following TI's app note about using the LM267x family for an inverting buck-boost converter, the output is connected to ground while the 'ground' is now the negative output. In terms of the feedback loop in my layout, RV1 connects to ground at one end. It feels kind of strange just connecting it to the ground plane like that, though I did try to add a trace between the output capacitors to it, and it avoids the inductor.If it makes any difference, I'm using one of these plug and play 5-V modules from MPS, the MEZD71201A-G at U5 on the far right. All things considering, since that source is just powering the op-amps, I didn't consider it to be as critical as the switching components, so I kind of haphazardly routed it. I figured the bypass caps will take care of the resthttps://www.digikey.com/product-detail/en/monolithic-power-systems-inc/MEZD71201A-G/1589-1458-ND/6823821

author: thm_w
author_rank: Super Contributor
timestamp: June 01, 2020, 09:27:41 pm
content: Looks good to me.The feedback trace doesn't have to be thick, as it carries little current, but if its thin or thick it doesn't change anything.Yeah with the planes you can sometimes have a cutout to pass a trace through, but with such a large plane and not too high density, wouldn't worry much.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: June 02, 2020, 03:07:27 pm
content: Thanks for your reply. I had to redo some parts due to my rookie mistake of incorrectly using the wrong op-amp pin out, but that didn't change my overall design. Thanks for your guidelines. They've helped a lot.What you said about cutouts, that brought to mind another question I had. I saw some other posts that people did with their power supplies as well as TI's LM2673 datasheet that for the top layer, I guess they kept it a signal plane and had their bottom plane to be ground. This appears to lead to 'segmented' copper areas on the top plane. They also kept some copper from going under components, so we have 'islands' of copper dedicated to one trace. Why is this done, and is it recommended I do the same? I've mentioned before that both top and bottom planes are ground planes, but if I put some no fill zones, perhaps it may help?For example, thinking of the negative regulator feedback, if I put no-fill zones at the output capacitor grounds and the two pins on RV1 (trimmer) connected to ground, I can put a trace that routes from the ground of the capacitors to RV1 so there will be a big trace that connects them together (and some small traces that connect them to the ground plane on the bottom side).https://electronics.stackexchange.com/questions/493621/pcb-critique-soft-start-power-distribution-from-24v-battery

author: thm_w
author_rank: Super Contributor
timestamp: June 02, 2020, 09:49:09 pm
content: I think they didn't purposefully remove ground fill, they just used those wide islands as high current transfer paths and then didn't bother with a ground fill. Its more work to set up another plane, and make sure they pour in the correct order.In some cases you might want to avoid ground for HF circuitry.https://electronics.stackexchange.com/questions/39239/when-to-use-ground-plane-cutoutsThermal reasons for soldering as well (or can adjust plane connect rules).What you suggest is a good idea, whether it makes a significant difference for the extra layout work, not sure. The hard part is when you move stuff around, you'll often have to redefine these cutouts.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: June 03, 2020, 03:26:32 am
content: Thanks for your reply. I kind of searched around a bit myself, and I found some links that highlighted the issue. It seems that the old practice was to not put copper fills in order to reduce EMI, but since my inductors are shielded, who knows how much it will help.https://e2e.ti.com/support/power-management/f/196/t/538740?-DC-DC-Converter-Ground-plane-cut-below-power-inductorhttp://rohmfs.rohm.com/en/products/databook/applinote/ic/power/switching_regulator/converter_pcb_layout_appli-e.pdfI went ahead and just decided to cut out the top copper pours under the inductor (and the catch diode). I thought that it would be safer to follow this practice than to not follow it. The rest of the circuit seems fine to leave alone (famous last words). I still kept the bottom layer ground pour untouched, so we'll see how that goes.Well, I submitted my board and ordered my parts. Here's hoping for the best once everything arrives. Funny how after I submitted my board that I realized I forgot to add more silkscreen. Not a dealbreaker, but it would've been real nice to have instructions on the back of the board.