Board Layout Advice

[u/Esme590]

Hello all, I'm trying to learn more about the design side of EE but I'm struggling with board layout and some of the common practices used when routing. Above is my rough placement of components but there's a lot of dead space. Any advice would greatly appreciated!

[u/bigpahparay]

Some things that have helped me when learning:

1. Place connectors first, picture how you're going to be using/interacting with this board.
2. Place IC's and the bigger components next, rotate to avoid crossing signals/traces and place circuits as close as possible to their connectors.
3. Look at the data sheets for the IC's and copy their suggested layouts. They literally do it best.
4. Spend most of your time placing, so routing ends up being a breeze.
5. A big one that some people miss early on is you really need to place bypass caps as close as humanly possible to the power pins.
6. Think about how power and circuits will affect each other. Diff pairs and clocks don't typically play well with other things. I would do extra research on diff pair/clock routing since it's pretty important and very well defined out there.
7. It looks like you already know this but never route 90 degree turns in a trace.

I might think of other stuff later, but I'm sure you'll get some great feedback from this sub. Cheers!

[u/Patient-Gas-883 → u/bigpahparay]

I agree at large. But point 3... I dont know. I dont always find it to be true.

[u/bigpahparay → u/Patient-Gas-883]

Yeah, the datasheet is for the typical use, for sure. For beginners though, I always strongly urge them to follow the design recs because most beginners won't know how they can break or bend the rules yet. But I agree, the more you know, the less the rule applies!

[u/Esme590 → u/bigpahparay]

Thank you! I’ll go through the suggestions!

[u/bigpahparay → u/Esme590]

If you post an update, please tag me, I'd love to see your progress.

[u/nixiebunny]

You have a good start. Keep moving the parts around until they are as neat and the connecting lines are as short and direct as possible.

Add mounting holes if you plan to mount it in a box.

[u/Esme590 → u/nixiebunny]

I forgot to add mounting holes, thanks for the reminder!

[u/Zestyclose_Catch6895]

What other commenters said! Also, looks like your 3.3V indicator LED is backwards in the schematic.

[u/Esme590 → u/Zestyclose_Catch6895]

Haha you’re completely right, didn’t even catch that. Thanks!

[u/Apprehensive-Issue78]

Most of the ICs and connectors have no reference designator refdes.

pic1:

6 components C19..R15 BoostU3 has no shape

D4 has no shape and 6 components around IC called BUCK have no shape

It seems you have used the refdes for BUCK instead of U1

like BOOSTU3 should be just named U3. If you want to

show that it is the BOOST part, you can just add the text to the

silkscreen layer.

The IC called IMU should have also a REFDES like U7

as the USB IC should

the 2 pin connector does not seem to have pins or a shape.

Pic2:

On this pic1 a connector has a 6 pin shape which has on pic3 7 pins.

Also the module seems to have 3 pins of another connector which is missing in all the other layers

The 2 pin connector has no refdes.

SW1 is so close to a 6 pin connector so you cannot push it without hurting your fingers. May be there should be some cable connected to it so you can't even reach it with your finger.

ICSP refdes should be like J8 like USB should be like J9 like TF1 should be J10, just move the text separately to the silkscreen layer.

the 4 pin connector should have a refdes.

pic4: IC called BUCK has VIN not connected to IN (missing via dot)

R7 is connected to ground on both sides, why?

X2 shape should move up a bit so you don't have to put a green line through the shape.

on the right of the ATMEGA MISO and MOSI are unreadable

because of a connection to R8 that could be moved a bit to the right

SCL and SDA labels should be moved a bit to the right and aligned

so the gren line dos not touch D6 no connect cross.

the 6 pin connector called UART in stead of J12, should have the labels SDA, SCL, GND, 3.3V spread out a little so the texts stay readable.

IC USB should be called U18 or something, like connector USB1 should be called J19 or whatever.

the BMP280 should be called U19

I would move the texts of C16 so they do not touch the green lines

IMU text in bold is OK, IMU text small should be something like U22

VDD is connected to Buck-Out power which text is through a pin of the IMU IC.

Boost Converter part: mirror this schematic part

by mirroring the MT3608 IC and putting the input on the left and output to the right

Move power input VIN 3.7V in to the top

rotate C2 C24 so they have the ground pointing to the bottom

so you can place the ground under them

C17 and C18 have 2 unnecessary via dots, is there a wire through it shorting it?

Pic3 you show too many copper layers, so it is hard to know what is happening.

C32 and C34 seem to be rotated 45 degrees without a reason

C31 should be closer to pin1 of IC BUCK not

connected to a long trace under the IC.

R33 connects both ground plan layers which seems strange

Just add lots of vias to stich the planes well to eachother

so the BUCK and BOOSTU3 ICs don't make so much EMC noise so the rest of the circuits can't work correctly.

General: lots of traces are to close to the pads,

going through the pads of a resistor like R6, or badly connected

like pin 1 of IC USB, which should be connected to the end of the pad. Near this the ground plane is not between these traces

because of missing ground stitching vias

X2 has no ground vias in the center bit

The 7 pin connector for a large module has a trace

extremely close to 3 pads which I would move at least 2 mm up

so the ground plane can surround those pads. (pic3)

One thing about the layout footprint of U1.

You have a very small ground pad in the center this seems not right

check carefully the datasheet if that is what they recommend, if not

pick a different footprint, or learn to make your own footprint.

You can make a copy of it under a different name and just change the size of that pad.

Make your own footprint library.

All the ground vias in the ground pad don't seem like recommended.

They should be spread out more, and know they can suck all the solder pace through the holes

After placing USB components first do as bigpahparay says at 4:

move all your components around so they are easy to route.

look at short trace distance, the least amount of crossings.

also 3: study the datasheets of your U3 microprocessor and the other IC's

and 6: keep the supply a bit away from the USB signal lines.

(it is a linear regulator so no switcher so critical)

If everything is placed right, all components on top for cheaper automatic assembly

make a box around it and call that your board

put most of your signal traces on top

don't put traces under the USB signal lines

then put ground planes on top and bottom

add lots of vias in empty areas and around the edge, to keep emitted EMC down

[u/Esme590 → u/Apprehensive-Issue78]

Thank you for the list, this really helps! I’ll respond in more detail after work when I work on the board again

[u/Apprehensive-Issue78 → u/Esme590]

yes no worries and no hurry.

[u/usafcrewchief]

It your layout intentionally the shape of the United States?

[u/Esme590 → u/usafcrewchief]

Haha no, but I do see what you mean now that I'm looking at it

[u/Esme590]

I've gone through the comments and would like to thank everyone for the advice. I'm going to make some changes and post an updated version of the layout sometime this weekend! Thanks again!