Review of my first board

I finally finished my first PCB in KiCAD and in general.

I will post in here, if you want to take a quick look at it.
KiCAD did not complain, but some vias seem close enough to footprints.

Here it is:

Is this supposed to mate with a specific board?

The mounting holes are awfully close to pins and traces. Consider a nylon washer if you use a metal screw with a wide head that may short to the track. Consider moving U3 away from the hole.

Place Vias that will link top & bottom Gnd areas.

I can’t tell if you have silkscreen on top of the pads. May be an image artifact.

Good luck!

It’s not just:

This hole is partly overlapping with the connector, and you probably wont be able to fit a screw in it.

Also, from your screenshot I can’t see much of the bottom layer, but it’s looks like you’ve made some attempt at a GND plane, but it’s cut to pieces by all kind of random tracks. This looks like a fairly simple circuit and a full GND plane may not be very important in this intstance, but it’s still good practice to get into a habit of making a full GND plane on one side of the PCB.

I don’t know what sort of IC’s you have on this board, but they probably need decoupling capacitors. Or are your C1 through C7 supposed to be decoupling capacitors? C1 through C4 are connected parallel. Why?

All of your tracks are very thin. It probably is the default 0.25mm which is good enough for low currents, but even then it may be better to sue a bit wider tracks. But it all depends on how the PCB is going to be manufactured. I also see the Vdd net routed through these thin tracks at some places.

SW1 may be burried and unreachable if you put another PCB on top of it.

Often the mounting holes are connected to the GND plane. If you want this then use the “MountingHole_Pad” schematic symbol.

You’ve used different sizes for the footprints of the resistors. Why?

It looks neater if you make neat roes of the resistors. It is mostly cosmetical, but it also helps a bit during soldering. You can also consider to use SMT resistors and capacitors for your next design. For around EUR25 you can buy a “book” with smt resistors, and thees “books” from Ebay / Ali / China have over 8000 resistors, usually 50 for each value and you can do a lot of projects with such a book. Resistor sizes of 0805 is easy to solder for almost anybody. and 0603 is doable for most people under the age of 40. If you can solder the SOIC’s you can also do 0805.

The layout of the connectors looks similar to an “arduino” board. Did you use one of the templates delivered with KiCad for that? If you need your connectors to match the locations must be the same. If it does not have to match an “arduino” board it’s better to put all those connectors on a 100mil grid. This makes it better compatible with matrix board and unexpected modifications.

With such simple PCB, try to rearrange the tracks to avoid vias as much as possible.
Also, if you pour ground plane make sure to avoid dangling “islands” of copper as they do more harm than good.
It might be not important for this board (depends on frequencies, signal slew rates) but it’s a general good practice and might be beneficial for learning.

I’d like to add two things to the others:

  1. The tracks are very thin compared to the simplicity of the circuit. This would make your design manufacturer sensitive. Make them wider and you can get away with even ironing.

Edit Note: Later seen that @paulvdh has already mentioned this.

  1. Like others mentioned the assembly holes don’t look right. If you take metric screws in to consideration, the head to thread diameter ratio is not correct in your design. You should have wider annular ring or smaller hole diameter.

The barrel? connector on the left. The ground connection is a thin trace, will fuse easily.
Does it really need routed slots or can you use circular holes and save money?

“Does it really need routed slots or can you use circular holes and save money?”
Excuse me, i did not understand this…
I used one of the KiCAD footprints that i think would work well.

Is my footprint “wrong”? Should i use another one?

NOTE: This i a standard arduino barrel connector.

Thank you everybody for your kind suggestions and for taking the time to review my board.
Here are some answers to your kind suggestions.

It is an arduino Mega shield.
I used the template that KiCAD provides.
Mounting holes will not be used…

The bottom is indeed a GND layer.

C1 to C4 are connected in parallel, because i could not find 400pf capacitors, so i will place 4 X 100pf caps.
The rest of the capacitors are decoupling caps.

About the traces being thin… This is my first board that i will print.
I plan on using jlcpcb as a service, and about all the width parameters, i used the template for jlcpcb that a github user has uploaded.

“You’ve used different sizes for the footprints of the resistors. Why?”
The resistors fall in two different fottprint families, their sizes are different.

Why do you want 400pF, a very non-standard value?
In the vast majority of circuits, you would use 390pF

My OCD is kicking in. I would orientate the IC’s all the same way. If you are manually soldering lots of these it’s easy to slip up and put one the wrong way around if the other 2 are different.

Also move the decoupling caps as close as possible to the IC’s

Nice one
Even for the first board it`s very good

1 Like

There are a couple of redundant tracks linking through hole footprint pins from the top layer to the bottom ground plane (higlighted in cyan).

In a manufacturing process that does plated through holes (also used for vias), the pad is already connected to the bottom layer by the hole plating.


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.