PCB design review - Page 1
Forum section: electronics / projects

author: tomshirvo
author_rank: Regular Contributor
timestamp: March 10, 2015, 04:55:42 am
content: Hi All,This isn't my first PCB I have designed but I am a newbie so I was hoping I could get some feed back on this design.These are screen nodes that communicate over RS485. My project has a need for 6 of these screens. They are spread over 4 metres but cable length will be over 8 metres.They are powered by Arduino Nanos', also using Sparkfun level shifter boards to convert the 5v from the Nano to the 3.3v for the screen. These screens are also touch but I am only using the interrupt from the screens as I don't need to know the location that was pressed. These will all be controlled with an Arduino Due. The baords also have ID chips on them so I can run a setup script on the Due and setup the location of them so they don't need to be programmed for the specific location.Any feedback would be great. Also I am usingwww.pcbway.comfor the printing of the boards and I will assemble them myself. Has anyone used this service before as I got 10 PCBs for $13 USD, sounds to good to be true.

author: tautech
author_rank: Super Contributor
timestamp: March 10, 2015, 05:09:20 am
content: Nice effort.Despite the presence of a top overlay, it's good practice to have a square pad or similar for polarised components.Likewise for pin 1 of IC's.You could also change a pad to identify the collector for the TO-92'sYour pads for TH passives could be larger, say 100 mil.Those are the things that hit me, others will have differing opinions.

author: sacherjj
author_rank: Frequent Contributor
timestamp: March 10, 2015, 03:43:28 pm
content: Depending on speed of signals, you have possible problems.At frequencies above 10 KHz, the power moves around a PCB by electric and magnetic fields. In other words, it flows in the plastic of the PCB. This is why the speed of signals in a PCB slow based on dielectric constant of the board material.When a signal starts flowing down a conductor, the field induce a immediate and opposite current on the closest conductor. This would be the plane below the conductor, until you break that plane. Then you get a field that expands to capacitively couple to whatever it needs.In the places I have indicated in the image, you have a break under conductors. If you do this on high frequency circuits, you create great EMI and don't pass FCC certification. You also induce signals into all the conductors the field crosses.Also, you have plenty of space to move conductors away from each other. You never want to run conductors for any length along with each other. If you have to, give them all the space you can. The important space is the distance between the two copper layers. i.e. the height of your core material (H). The induced signals happen because of the sharing of the fields.Try to get your conductors 2-3H away if possible. I would theorize that much of the return current is actually occurring on other data lines next to each other for much of this board, due to the thickness of a 2 layer core and proximity of the conductors.Again, all of this depends on how much noise levels you can deal with and how fast you are going. But it is good to get into habits of thinking through these things when doing a PCB design. Many of these are hard to solve on 2 layer designs (and the layer coupling is so bad, due to large thickness of core material, that it has less effect.)

author: PeterHouse
author_rank: Contributor
timestamp: March 10, 2015, 04:04:54 pm
content: 1. The board is generally lacking in part nomenclature. Each part should have an identity for reference.2. There is a trace just above the lower left 6 pin inline connector in the shape of a "T". The right hand "armpit" of the T is cut in such a way that in production there is a good chance the etching process will deepen this "armpit" and may even blow through the trace. In general this is not a good practice. On a small run of prototypes, you will most likely get away with it and never notice - in high volume, something like this will cause a good number of PCBs to fail either due to trace blowout or if the trace is merely narrowed the current density will go up causing a hot spot. There are a few of these on the board.3. U3 seems to be 780X part. Make sure you have enough heat sink area for the power it must dissipate.4. The top left mounting hole and the two bottom mounting holes look crowded with not enough room for tooling to work around a screw and nut type fastener unless it is a snap in type fastener.Pretty good for a first board.

author: tomshirvo
author_rank: Regular Contributor
timestamp: March 10, 2015, 09:34:29 pm
content: Thanks for all the feedback it is great for helping me learn the best way to design PCBs.So I updated the board with a few of the suggestions given.QuoteAll these packages are just standard in Eagle, do you think I should go through and change them?QuoteI fixed a few of the things you recommended but it is hard to do some.Would it be just as bad to have a resistor go over a serial communication line? My communications will run at 115200 Baud so do you think I will get lots of noise at that speed. If so I can just slow it down as the data being sent is only small. I also have error checking in my software for all communications.QuoteAll the yellow shown on the board is the silkscreen, what else should I have to identify each part?QuoteI put in a bunch of via stitching to help remove heat. The device is a 3.3v regulator upto 800mA but the screen only gets upto 400mA or so. I thought the over kill would allow for cooler running.I have attached the updated board.Thanks again it was very helpful.

author: tautech
author_rank: Super Contributor
timestamp: March 10, 2015, 09:44:29 pm
content: Quote from: tomshirvo on March 10, 2015, 09:34:29 pmHell yeah, they might be std but that doesn't mean it's perfect.Just edit the pad properties.ALL components that have a intended orientation should have an identifiable pad on their footprint.Lets say you have to rework the PCB, you'll have to endlessly turn the PCB over to see the overlay to identify a particular pin.STUFF THAT.Change pads to help you.