PCB Design - Page 1
Forum section: electronics / beginners

author: nuclear213
author_rank: Newbie
timestamp: August 12, 2019, 08:58:43 am
content: Hello everyone,I am currently studying electrical engineering in Germany, sadly we have no course about PCB layout and design and as far as I could find out not even a professor with experience in this field. Since we have semester breaks right now I thought it might be good to idea to try it out a bit. Previously I was just building my circuits on perfboard so I have no idea how to design a good layout especially with SMD components.This design is just a DC-DC converter and a h-bridge with a SM72295 full bridge driver, however at somewhat high currents (7A-10A@40V). Also the switching frequency of the DC-DC converter is quite high with up to 1.5MHz so EMI could become a problem.To adress the problems I filled in most copper parts with areas, split the ground plane and tried to keep the tracks as short as possible but I am sure I violated at least one or two good design practices.So if anyone could see the gerber files and give me a few tips it would be geatly appreciated.Thanks in advancenuclear213Edit:Thanks for the videos DaveThere were a great help and inspiration to me. I have been watching them since I was 14 years old. Keep up the good work

author: teksturi
author_rank: Regular Contributor
timestamp: August 13, 2019, 08:47:50 pm
content: It would be much nicer to people that you submit schematic and board layout top and bottom straight to forum using png's. I atleast think that then you will get responses.Edit: And welcome to forum.

author: homebrew
author_rank: Frequent Contributor
timestamp: August 13, 2019, 09:04:30 pm
content: Quote from: teksturi on August 13, 2019, 08:47:50 pmAnd additionally - especially as this is a KiCAD project, just add the whole thing.Some things in the schematic seem incorrect - like the 39K resistor on the feedback voltage divider ...

author: JustMeHere
author_rank: Frequent Contributor
timestamp: August 14, 2019, 03:40:08 am
content: I'd be wary of a split ground plane. You need to make sure you have a good return path. Read High Speed Digital Design: A Handbook of Black Magic.

author: nuclear213
author_rank: Newbie
timestamp: August 14, 2019, 10:23:52 am
content: First of all thanks for the replys.Yes the feedbackresistor was wrong. I dont know how I did not see that. Thanks for the tip.Regarding the gerber. I thought it was the most universal option to transfer the schematic. But I agree that it is easier with the pictures. Sadly I dont really see a good option of exporting pictures so I hope the export from the 3D viewer are good enough. Otherwise I will look into it.@JustMeHere:Well in theory there should be a good return path for all the different parts. The control signals should not need to go on the power GND and vice versa. So there should be also no real current flowing between them. At least that is how I understand it. Please correct me if I am wrong.Regarding the book: After a first quick search I can only find it for above 100€. Sadly a bit expensive for me right now. Also I am not sure if 1.5MHz really classifies as HF. The description of the book itself states > 10MHz but I will surely keep it in mind. Thanks

author: schratterulrich
author_rank: Regular Contributor
timestamp: August 14, 2019, 11:47:22 am
content: It seems to be a well designed layout where all critical loops with fast current transients were kept small.I have only one comment about the splitted gnd planes:Splitting planes works for low frequency and DC - but this is not needed hereAt higher frequencies the splitting does not work, because inductive and capacitive coupling nevertheless couple currents into the "quiet" GND.With the disadvantage that a noncontinuous GND plane can increase the inductivity of critical loops (which are well designed in this layout).In my experience, ferrites at all connectors (except GND for your digital return currents) work better against GND bounce and EM radiation than splitting GNDs...another comment:You should have a GND return on J4

author: homebrew
author_rank: Frequent Contributor
timestamp: August 14, 2019, 06:49:09 pm
content: Could it be that LOB HOB on U3 swapped?

author: Ice-Tea
author_rank: Super Contributor
timestamp: August 14, 2019, 07:05:42 pm
content: Quote from: nuclear213 on August 14, 2019, 10:23:52 amCommon trap for young players: clock speed does not matter, rising/falling edges do. Think of it this way: if you use a recent FPGA to drive a 9200kbps it will still do so with the same silicon as it would driving a 300MHz signal off chip(yes, yes, I know you can modify drive strenght, slew rate,...)

author: nuclear213
author_rank: Newbie
timestamp: August 14, 2019, 07:46:17 pm
content: @homebrewyes you are totally right. Damn. I switched the pins of the MOSFETs so I would have shorter tracks on the pcb but forgot to change the drivepins.. Thanks so much. I would have ordered it and woundered why it just will not drive one side of the h-bridge. Thanks so much again.@Ice-TeaOk I get that. Especially with the MOSFETs and drivers designed to switch within 10's of ns the frequency there is a lot higher. I really need to think about the transients.@schratterulrichWell I split the ground planes because the design rules of the buck-converter controller ic stated that. I guess I will read more into all of the different cuppling mechanismns. I guess I will bite the bullet and buy myself the book.Thanks again to everyone. You are awesome.

author: JustMeHere
author_rank: Frequent Contributor
timestamp: August 14, 2019, 11:59:54 pm
content: See chapter 5.http://electronix.org.ru/books/high-speed-digital-design.pdf

author: schratterulrich
author_rank: Regular Contributor
timestamp: August 15, 2019, 10:11:20 am
content: Quote from: nuclear213 on August 14, 2019, 07:46:17 pmIn the datasheet a layout is shown with the starpoint at the output capacitor:The IC compares the voltage at the output capacitor to its internal reference. So you want to sense this output voltage without any interferences.When you look at the layout there is only the quiescent current of the IC flowing int the GND plane between the output capacitor and the IC GND connection.So there will be minimal galvanical coupling and the GND split make sense.You have placed the starpoint at the input connector:If the IC senses Uout, the voltage drop of your power currents will add to the voltage sensed at the feedback input. I would suggest to move your GND starpoint and your feedback sense line directly to the output capacitor C8.

author: nuclear213
author_rank: Newbie
timestamp: August 15, 2019, 02:47:26 pm
content: Ok I will change that. I guess the ideal place for the feebbackwire would be the input in the driver, since it would compensate the entire losses that way.However I am not sure about the control loop stability then, so I will just route it on the bottom layer directly from the cap pin.So thanks a lot everyone. You were a huge help. I will order the pcb and the parts in the comming days and build it up.