Advice on First Large(-ish) PCB Design - Page 1
Forum section: electronics / beginners

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 01:35:02 pm
content: First, picsTop Outer Apearance:Top Insides with Main Ground Plane:Bottom views in album:https://imgur.com/a/t90SMalThis design is a few months old, but Dave's recent video inspired me to join the forum and look for advice on it. It's already been ordered, and has been sitting in package limbo at my university since they closed, so any recommendations probably can't happen aside from bodges. Better late than never, I guess?The design is for a club I'm in. The aim was to get a Raspberry Pi to interface with any hardware it may encounter in our underwater robot, without buying 15+ prototyping boards. The general goals were basic sensors for monitoring the robot (mostly top right of board), leak sensing, some decent (>1A) power switching, and general GPIO/ADC/PWM control.PDFs & Eagle files are too big for forum, so are in my Github repo:https://github.com/CuUwrRobotics/interface-boardSome specific questions:The I2C lines seem a little convoluted to me; are they problematic? How I could have avoided that?The lower-middle part of the board has a lot of signal traces going across to some ADCs, while also having some power traces going along right along them. Would that cause any problems? Is it bad practice at all?Is there anything this design is missing from a feature standpoint? Anything that I should have had for a robot that I didn't think of?I'd like to improve the current-carrying capacity of the power switching at the bottom of the board. The PCB is the bottleneck there; the MOSFETs are capable of ~40A and the connectors ~17.5A. I provided a way to tin the traces, but one idea I had (which I got from a 30A ESC) was totin/solder a wire along the trace. Has anyone done this? Is that better than plain tinning? Or even equivalent to direct wiring?Some regrets I have already:A single 0402 part, used for the reverse-polarity protection circuitry.I didn't connect one of the power pins for the ATMEGA328, since I thought I didn't have the space. Looking back, I definitely did.The "Arduino" section is messy from an appearance standpoint.I didn't put amplifiers on the telemetry/monitoring ADC, because I was scared of analog. This results in, for example, a tolerance of +-1.2A on the current sensors, which could have been halfed.The schematic should have been done in multiple pages.Obviously, any other advice is welcome!

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 02:46:39 pm
content: First, a little bit of manual DRC...Top side:IC4,IC5 thermal pads are not connected anywhere, probably they should be connected to GND or something...Q1 and other power MOSFETs have many open vias under the big terminal (drain?), this may be a trouble for automatic assembly, but considering the current... this may be necessary to have them for cooling.R15,R17 are too close, spacing may be not enough for solder mask bridge to stay there.Two LEDs in the bottom right - too close, PB1(PR1) - huge vias in the lower pad.SPI connector - overlapping silkscreen, below GPIO0 - silkscreen is over IC pads.Bottom side:Y1 - better remove polygon fillings; R27,R28 - too close.Schematic: I2C pull-ups ? GPIO extenders and other ICs address selector pull-ups ?Quote from: nichlock on July 25, 2020, 01:35:02 pmThey are low frequency anyway, I see no problems.Quote from: nichlock on July 25, 2020, 01:35:02 pmMaybe, I would separate them with a via stitched ground trace all way long. In any case you have to make sure there's no high current path going near these traces, including return path via ground. Separating grounds of functional blocks may help.Quote from: nichlock on July 25, 2020, 01:35:02 pmWhat MOSFETs do you use (part number)? PCB traces look pretty wide even for this current... maybe bigger 7.62/10mm screw terminals would work?Removing thermal isolation from high current screw terminal pads would be good idea.

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 04:00:41 pm
content: Thanks for the replies!Do you mean that the MOSFETs would have been better off without those vias? I was trying to use both layers for the high current, do you think would it be more optimal to just have no vias/only use the bottom layer? Those are SiS476DN, so I'll be seeing an R_DS(ON) of around 3.5mOhms in this design. Screw terminals are a nice idea.For the other posts:The thermal pad should have been connected - looks like I've put too much trust on the default library!Thanks for the advice on vias and assembly, didn't think of that. Fortunately, this will be done manually, but I'll incorporate this into rev two.JLC PCB claim they can do the resistors and LEDs, so my DRC settings allowed it, but you're right that .25mm is a bit too close for comfort. I'll fix that for rev two as well.Silkscreen mistakes are frustrating!I'm relying on the I2C pullups in the Raspebrry Pi here, but good point. Added to rev 2. Address selectors were left open on purpose.

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 04:15:53 pm
content: Quote from: nichlock on July 25, 2020, 04:00:41 pmNo, from thermal and current carrying considerations it is better to have them, but then you have to think carefully about the manufacturing process.For manual assembly - no problems, you can apply as much solder as you need, but there may be not enough solder paste to fill all these vias in reflow oven.

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 04:25:23 pm
content: Quote from: nichlock on July 25, 2020, 04:00:41 pmIs this a clearance between copper pads or a solder mask width? If 0.25mm is a safe value for solder mask width, then clearance between pads must be 2-3 times of that.

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 04:34:15 pm
content: Thanks for the advice! Hopefully the tenting on the other side of the board will help with the vias. Is trial and error the only reliable way to know if these issues will come up in automated manufacturing?The clearance is between copper pads, so I think I'll be in the clear, but the spacing is on my to-do list now either way. No reason I should have had those so close.

author: mariush
author_rank: Super Contributor
timestamp: July 25, 2020, 07:51:55 pm
content: Just looking at the circuit board picture....I'd move the opamps IC4 and IC5 closer to the top left corner and align them so that the 2 groups of jumpers are right next to each otherAlign those resistor networks near pwm0 and pwm1 ... actually i'd use a smaller font for those two texts and drop the line drawing ... then you could have the two resistor networks on each header more towards the center, and have 0 15 and 7 8 text near the pins. Losing quite a bit of pcb space where that silkscreen text is.At very least you could move the jumpers between the chips and in a vertical column, just like all the other jumpers (opamps)adc0 and adc1 silkscreen text is confusing ... why is adc0 0..3 at top , 4..7 at bottom and adc1 is 4..7 at top, and 0..3 at bottom, or is the text wrong? why not route the traces to be same... if not messing up something, maybe leave a space between so you could put text between the headers?fuse is kinda in a bad place, may be difficult to desolder it due to the other components around.lots of empty space if that could be used for traces if you use a bit smaller font...just shifting things around on the board could give you more roomhere's just a few things moved in ms paint ...

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 08:47:56 pm
content: What is the type and current rating of F3 fuse? For currents as high as you mentioned above I would strongly recommend to switch to a through-hole type fuse, SMD package can desolder itself in case of a failure and in worst case short something else while leaving PCB.

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 09:02:04 pm
content: Thanks for the feedback, all great points, and all added to my rev two list!Spacing/appearance is a bit weird here. We wanted to have something we could show off at fundraisers, hence the big text and woo-woo lines, but at the same time we had to meet a deadline much closer than expected with the rapidly changing situation. (In the end, we missed it anyway due to shipping delays.) There were also couple of major changes to our design goals made in the middle of designing... I'll be avoiding that mess in the future.The ADC layout is weird because of how I did it in the schematic. Honestly, I thought I had fixed this - must have gotten distracted midway through. On my to do list for rev 2!Misaligning those resistor networks was a painful thing to do to the appearance. I'll use some smaller text in my next version which will help.Never considered the positioning of the fuse! Luckily, this fuse is resettable, so it should not need replacing unless there are some very exceptional miskates.

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 09:23:21 pm
content: All fuses are PTC resettable. F3 and F1 are both 3A, and F2 is .5A. Fuse F1 only goes to an off-board buck converter, it's really just there in case of shorts to that converter, as the 12V coming in may be fused for higher loads. F1 is for the 5V rail, which is meant to power the Raspberry Pi. F2 is only for the current sensors at the top right of the board.The 3A fuses claim a tripped power dissipation of 1.5W, so that could definitely be an issue! As I said in my other post, I hadn't put too much consideration into fuses; I just chose the ratings I needed then minimized the time to trip.When should I choose a through-hole fuse over SMD for these PTC fuses? Is power dissipation the only major consideration?

author: Unixon
author_rank: Frequent Contributor
timestamp: July 25, 2020, 09:46:31 pm
content: Quote from: nichlock on July 25, 2020, 09:23:21 pmPower dissipation is one of things to consider, another one is that PTCs can be irreversibly damaged while soldering and the higher rating a fuse is the more thermal mass and power dissipation it has and must be attached to PCB in a proportionally more reliable way which may mean in turn soldering it down with a higher melting point solder than anything around. Through-hole PTCs are harder to overheat during assembly. Once overheated PTC can have many times out of spec trip current and eventually turns into a jumper.

author: nichlock
author_rank: Newbie
timestamp: July 25, 2020, 10:05:42 pm
content: Now I know! Thanks for all the help.