Request for Feedback on PCB layout for DC/DC Converter on Budget - Page 1
Forum section: electronics / projects

author: cyrus8052
author_rank: Contributor
timestamp: April 30, 2017, 09:10:56 am
content: Hi,I am trying to build a dc/dc converter based on Richtek RT7297B. This is a 3A, 18V, 1.2MHz Synchronous Step-Down Converter.This is my first attempt to design a PCB. I have tried to follow the manufacturers recommendation for layout. Being my first attempt, I am not sure to what extent I got this right.I request you to give your opinions and feedback to improve myself.

author: Rerouter
author_rank: Super Contributor
timestamp: April 30, 2017, 10:01:53 am
content: You can compact it much more without issue, first off your loop size can be way smaller,Starting with the simple stuff, change cb to a slightly larger package and have it hop over the vin pin to the switching node to completly loose the vias. Its low current but you want that switching node tiny to keep the transistions fast.Next up rotate l1 90 degrees counterclockwise, have his pad almost sitting on the switching pin, then have your 2 capacitors sitting to the right of him with there grounds right next to the package (tiny loop sizes is better) and end the top side ground at there pads.Css rotate 90 degrees counterclockwise and also have his ground pad right next to the switching ic, and reduce your top side ground on that end to just css.Flip your cin caps so they connect to the top side ground right at the switching ic.Now with all that other stuff cleaned up, run ren directly across the top with no vias.Now for r1, with the top side ground out of the way run him directly to vout, but connect after the capacitors, and r2s ground inline with cout, we want our output referenced off these output capacitors.Then for the comp network bring them as close to the pins as possible using the bottom ground right next to the cout pad if you can.And for.good luck via stich your grounds very near the capacitor padsTry that, your loop size will be way smaller.

author: sokoloff
author_rank: Super Contributor
timestamp: April 30, 2017, 10:03:58 am
content: Also, consider whether you want to have any mechanical mounting ("screw") hole or holes on the board to help it fit into projects/cases, etc.Then, consider whether you want those screws to be at GND or floating potential (if you can't decide, float them).

author: Rerouter
author_rank: Super Contributor
timestamp: April 30, 2017, 10:10:00 am
content: Because of the switching speed, i would go with grounded screws, otherwise the nearby inductance will likely turn them into antennas.

author: cyrus8052
author_rank: Contributor
timestamp: April 30, 2017, 11:08:15 am
content: @rerouter, Thank you very much for such a detailed reply. I will work on it and share the revised design.@sokoloff Thank you very much for reminding me about mounting holes. I believe this is a classic mistake by newbie's like me. I was focusing on the layout and totally forgot the mounting holes. I will add mounting holes with grounded screws as suggested by @rerouterThanks again for both of you.

author: cyrus8052
author_rank: Contributor
timestamp: April 30, 2017, 02:54:49 pm
content: @rerouter, You have an amazing eye for details. Here is the revised layout with mounting holes as suggested by @sokoloff. The mounting holes are grounded too.I can't thank you enough for helping me out.

author: cyrus8052
author_rank: Contributor
timestamp: April 30, 2017, 03:05:29 pm
content: @rerouter, I forgot the via stitching near capacitor grounds. I have revised the layout, but not uploading it.Thanks again,

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: April 30, 2017, 06:41:50 pm
content: The net names in your holes are GND but I'm seeing enough copper clearance that the screw head may not make contact. Is this your intension?

author: cyrus8052
author_rank: Contributor
timestamp: May 01, 2017, 12:58:56 am
content: Quote from: pixulator on April 30, 2017, 06:41:50 pmNot really. This is my first ever attempt to design a PCB. I have a lot to learn.I will revise the mounting holes to have more copper clearance.Thank you very much.

author: pigrew
author_rank: Frequent Contributor
timestamp: May 01, 2017, 03:43:07 am
content: I'm not sure if it's a good or a bad idea to tent the bottom of the vias of the controller's exposed pad. I just did a design where a fair bit of solder wicked through vias. On the other hand, it may trap moisture in the via, leading to corrosion.

author: cyrus8052
author_rank: Contributor
timestamp: May 01, 2017, 04:33:18 am
content: Quote from: pigrew on May 01, 2017, 03:43:07 amI thought about it too. I am not sure which way to go. Probably I may have to move them away from exposed pad to the other parts of ground pane.

author: pigrew
author_rank: Frequent Contributor
timestamp: May 01, 2017, 04:41:34 am
content: Quote from: cyrus8052 on May 01, 2017, 04:33:18 amI'd leave them where they are. They cool the chip better when placed underneath it.

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: May 01, 2017, 06:32:44 pm
content: Regarding the Vias under the pad I agree that's essential. Their are three things to consider first is thermal performance, the second is noise and the third is grounding.If your wanting to drive this to the max then your 3.3 volt output ( as I see you have configured it) @ 3 Amps is as good as 10 Watts !! So your wanting to pull the heat away in an efficient manor to achieve that without things melting (I know it has thermal shutdown but still). Also depending on how accurate you need the output voltage note the chart page 6 shows output voltage drops off with temperature and load. The datasheet gives the shutdown at 150°C but recommends not exceeding 125°C (section "Over Temperature Protection" page 10) for continuous operation. On the next page they give the formula to workout the max power dissipation required for a given junction temperature. Basically the power you can sink must be more then what the chip generates or the temperature will just keep going up.The TDK inductor series mentioned I could not find a 3.6uH version at least on Digikey (typical) but the Tayio one is available (NR8040T3R6N) and is rated up to 4.9 Amps so more then enough. Anyway the max DC resistance is 19.5 m? so we have about 60mW power in that little thing.The power dissipated in your RT7297 is given by its efficiency at the output less the power though the inductor. Worst case that's 80% (Vin=17V Iout=3A). If the power to the load is 10 Watts then the total dissipated power is 10/0.8 - 10 = 2.5 Watts. So in this case the power dissipated by the inductor is negligible but either-way our total dissipation in the chip is 2.5 - 0.0195 = 2.48 W.The reference PCB layout does assume the best case copper as shown in Figure 7.e and as your own design seems to match that then your looking at no worse than 49°C/W. The previous formula then gives you about 2.04 Watts max output at 25°C ambient room temperature.So you do want the vias. I would also recommend doing a coper poor on the bottom layer for the vias to connect to. How you go about calculating the actual heat dissipation of a PCB layout I'm not sure but your close already. Just need to find another 440mW in copper. As I said your design may already achieve that I'm not sure, and also this only maters if your pulling the max current out of it. [http://www.ti.com/lit/an/slva462/slva462.pdf]Regarding noise, switch mode supplies frequency has a nasty hait of ending up on the supply rails at every conceivable point including grounds, behind your ears and so on. So that's another good reason to do copper pour top and bottom with plenty of stitching with a liberal sprinkling of ferrite beads. Depending on your application you may not care about it but it's something to consider.

author: james_s
author_rank: Super Contributor
timestamp: May 01, 2017, 07:22:15 pm
content: That's quite an ambitious undertaking for a first attempt at PCB design, switchmode regulators are not trivial and that's a particularly high frequency unit. I'll be interested to hear if it works when you're finished.

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: May 01, 2017, 11:22:22 pm
content: @james_sAmbition is never illfounded. Having a false expectation of a devices performance characteristics is a different question. OP has not really mentioned any tolerances so we can only presume they are not particularly critical at this stage.In a hobbyist context I subscribe to the 'suck it and see' approach towards prototyping. That does not mean you have not put your all in to a design or layout but at some point you need to set a deadline where the pcb goes to fab. Without a deadline you'll go crazy down the rabbit hole worrying about via placement and so on.I raised some points regarding thermal considerations but that was not meant to demotivate OP from pressing a board but more thoughts for future revisions or other designs.OP Your board looks ok, it's based of the reference design so no doubt it will work. Will it be 3.3V +- 0.00000001V probably not but who cares.. you built it and learning will come from it.GO FOR IT.

author: rx8pilot
author_rank: Super Contributor
timestamp: May 01, 2017, 11:26:44 pm
content: Quote from: james_s on May 01, 2017, 07:22:15 pmThis is very true. SMPS is an interesting and difficult challenge. One major 'gotcha' is just taking accurate measurements which can have you chasing your tail til the end of time. I did not have the time to examine your design, but just wanted to chime in and suggest you prepare yourself for some unexpected tangents. It looks easy until you dive in.

author: james_s
author_rank: Super Contributor
timestamp: May 01, 2017, 11:27:40 pm
content: Don't get me wrong, I'm not saying not to try. My only point was that it's quite an accomplishment if it works properly. Don't be deterred if it isn't quite right the first time around, I think with some guidance from here you'll probably pull it off.

author: rx8pilot
author_rank: Super Contributor
timestamp: May 01, 2017, 11:51:27 pm
content: Quote from: james_s on May 01, 2017, 11:27:40 pmTotally - you have to try. There are some lessons that don't make sense until they are right in front of you. If the first one works really well - fantastic. If it crashes and burns - try again. My experience a few years back when I dove into power electronics was that my first designs 'sorta' worked. I continued to read and experiments until I got some really high-performance designs. As nerdy as it sounds - it was a ton of fun tracking down issues, knowledge, and performance. No major damage along the way.

author: james_s
author_rank: Super Contributor
timestamp: May 02, 2017, 12:04:56 am
content: The part that gave me the most difficulty in the beginning was layout and grounding. I'd build them on perfboard and sometimes they worked, other times they ran hot, were unstable or didn't work at all. Layout can be critical, proximity between certain components can have large effects on the design. Ground loops, stray capacitance, stray inductance, it can have you ripping your hair out. Now armed with more knowledge, experience, a decent oscilloscope and an LCR meter to measure inductors it's quite a bit easier. It's really quite satisfying to design a switching regulator that just works.

author: cyrus8052
author_rank: Contributor
timestamp: May 02, 2017, 01:57:17 am
content: Quote from: pixulator on May 01, 2017, 06:32:44 pmThank you very much for making me think more on heat dissipation. I will calculate the heat dissipation and will change the layout if necessary.Quote from: pixulator on May 01, 2017, 06:32:44 pmI am using NR8040T3R6N. Further, the load may be around 2 Amps and heat dissipated by inductor may not impact the design.Quote from: pixulator on May 01, 2017, 06:32:44 pmI did give little thought about heat dissipation, but nowhere like you have analyzed. My focus was getting this work on some load, if not full load. The reference layout in datasheet gave me some idea about copper needed to dissipate the heat generated. So, I decided to use the bottom layer as ground and enough vias to bottom layer.Quote from: pixulator on May 01, 2017, 06:32:44 pmI will definitely use ferrite beads in the final application. The final application requires a good quality power supply with low noise. I took upon the challenge of building one on a budget.

author: cyrus8052
author_rank: Contributor
timestamp: May 02, 2017, 01:59:26 am
content: Quote from: james_s on May 01, 2017, 07:22:15 pmYou are absolutely right. I have no illusions about this right from start. I will definitely share the final working design.

author: cyrus8052
author_rank: Contributor
timestamp: May 02, 2017, 02:08:14 am
content: Quote from: pixulator on May 01, 2017, 11:22:22 pmAt this point of time, tolerances are not critical, as long as this design works.Quote from: pixulator on May 01, 2017, 11:22:22 pmThank you very much fo the encouraging words. At this moment, the goal is to make this board work within reasonable tolerances needed for digital electronics, I would be very happy.

author: cyrus8052
author_rank: Contributor
timestamp: May 02, 2017, 02:33:23 am
content: Quote from: rx8pilot on May 01, 2017, 11:26:44 pm@rx8pilot I hear you. I don't know how I will fare with testing, but I have collected information on the subject. One of them is a wonderful guide from TI, called "TI-PMLK Buck-Boost Experiment Book". Though the book is targeting a development board with TI dc/dc converters, it does teach a lot about testing the dc/dc converters in general.One can download it from herehttp://www.ti.com/lit/ug/ssqu009a/ssqu009a.pdf

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: May 02, 2017, 08:16:39 pm
content: Hi OP, here is the power supply part of a layout I just got back. No idea how it performs yet will be loading it this weekend.It's based on the reference layouts for the TPS65130 for +-15 Volts. The companion chip is MAX5496ETE to do calibration. VDD is just 3.3V from a ADP1715ARMZ-3.3. Probably not relevant to your question but thought I would share some hot off the press FR4.

author: james_s
author_rank: Super Contributor
timestamp: May 02, 2017, 10:34:46 pm
content: It looks reasonably good to me, certainly impressive for a first try.One thing I notice though is that it's missing reference designators, you'll want to have those in the future as it makes building and troubleshooting so much easier. When you go back and look at this months from now you'll probably be wondering which part is which on the schematic.

author: cyrus8052
author_rank: Contributor
timestamp: May 03, 2017, 12:38:56 am
content: @pixulator Thanks for sharing the layout. Considering my experience in design and layout, I am certainly not qualified to comment. But, you have inspired me to do more like designing around dc/dc switching controllers for dual outputs.It would be great if you can share how did it go when you assemble the board.

author: Rerouter
author_rank: Super Contributor
timestamp: May 03, 2017, 09:31:03 am
content: The only real negative i can see on pixalators is that below his +15v inductor his capacitor is on a stub and not inline with the power trace, its tiny, and not worth worrying about for suck it and see, but will add a little noiss to his output.

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: May 03, 2017, 07:43:52 pm
content: @Rerouter I'm not sure what component you are referring to, I've added some designators the the image below if you don't mind directing me the the component in question.@james_s : Regarding the designators, on larger boards (this one has 350 odd components mostly 0402) it just gets to be a mess so I tend to leave them off just highlighting section blocks as I've done on the power supply. Other projects I work on, in a commercial context, it's a different story where some poor guy who is not me may be expected to service the board in the future. For personal use I have the layout and designators on a PDF drawing or back in KiCad.@cyrus8052 : Yeah just go for it. The only thing I will warn you about is the 'suck it and see' mentality can cost you money for a big fail or it may save you money and time it just depends. The main idea is that worrying about every design aspect to the n'th degree when it is not required is another form of procrastination, and so must die. Dave's recent videohe goes on about 10 different things that are not good or perfect but hey it's just a project for him, not production so who cares.

author: dmills
author_rank: Super Contributor
timestamp: May 03, 2017, 10:59:59 pm
content: One thing I would add to the OPs design is an electrolytic across the input, maybe 100uF or so, the ESR helps to dampen the overshoot that can happen if you connect a stiff power supply on reasonably long leads when a MLCC is used as the main input cap.73 Dan.

author: cyrus8052
author_rank: Contributor
timestamp: May 04, 2017, 12:48:50 am
content: Quote from: pixulator on May 03, 2017, 07:43:52 pmI am going for it. I am hoping this will work, thanks to advice received over here. I will send it out for PCB once I am done with application part of PCB.I will checkout the video today.

author: cyrus8052
author_rank: Contributor
timestamp: May 04, 2017, 12:51:32 am
content: Quote from: dmills on May 03, 2017, 10:59:59 pmThanks for the suggestion. I will make a provision for an electrolytic and populate it if required.

author: Rerouter
author_rank: Super Contributor
timestamp: May 04, 2017, 10:22:25 am
content: Pixalator, c5, rotated 90 degrees clockwise would mean all output current is passed by the capacitors esr rather than directly out to your ciruit.

author: David Chamberlain
author_rank: Frequent Contributor
timestamp: May 04, 2017, 01:38:41 pm
content: I see Rerouter, thanks.

author: alexig
author_rank: Contributor
timestamp: May 06, 2017, 10:51:37 am
content: I used the RT8293A (340KHz) with a similar design as your first PCB (except I had the output caps ground going to the same ground as the input caps). The RT8293A I used also worked on a breadboard, although I didn't try it with much load (something I hear that usually doesn't work with most DC-DCs).I do like the second design PCB better so it does have a very high chance of working.One thing you don't want to do is touch the feedback resistors like I did, it will fluctuate the output voltage and can damage the chip. Also careful about running any cabling near by it too (within ~1cm, pretty rare to do and probably not something that you would do) as that can cause a similar issue.

author: cyrus8052
author_rank: Contributor
timestamp: May 06, 2017, 12:05:29 pm
content: Quote from: alexig on May 06, 2017, 10:51:37 amThanks to wonderful feedback from @rerouter, I could refine the initial design. I too believe it will work.Quote from: alexig on May 06, 2017, 10:51:37 amThank you very much for the tip. I will be careful when I build.

author: Rerouter
author_rank: Super Contributor
timestamp: May 06, 2017, 12:58:52 pm
content: Behold the power of a boring Saturday afternoon and MS Paint, again none of the changes are really required, PCB layout literally is an artwork, and open to interpretation past a certain point. i just wanted to close the loops of current as small as possible, remove all non ground via's, and force all current through the input and output capacitors.the purple and green is just me drawing on the forward and lowest impedance return paths, just to get an idea on loop size, in this case its literally only at the capacitors, which with the vias where they are only leave a very tiny loop open,

author: cyrus8052
author_rank: Contributor
timestamp: May 06, 2017, 01:24:30 pm
content: Quote from: Rerouter on May 06, 2017, 12:58:52 pm@rerouter, you are great! You are a wonderful teacher and mentor. Thanks to you and other members of the forum, this thread is evolving into a very good tutorial on layout for dc/dc converters.I am yet to send the layout to fab as I had not completed the design of the application. I will revise the layout.Thanks again.

author: Rerouter
author_rank: Super Contributor
timestamp: May 06, 2017, 01:28:16 pm
content: just realized i broke ren's trace, just run him around the ground trace to j1

author: MagicSmoker
author_rank: Super Contributor
timestamp: May 06, 2017, 01:32:44 pm
content: Quote from: Rerouter on May 06, 2017, 12:58:52 pmThe OP's layout wasn't bad for a first attempt, but you fixed the two big issues that I saw with it very nicely - the trace from pin 3 to Cboot interrupting the return pathway for the input capacitors (this sin is especially bad in a buck converter due to the square shape current pulses drawn from them) and the trace from Vout to the upper divider resistor (much less of an issue because current in the output capacitors is triangular, and the top layer ground fill provides a solid return pathway).