Criticism & suggestions wanted: First Circuit Board design

After years of building projects on perfboard with point-to-point wiring, having a PCB made is now so cheap as to make perfboarding not worth the effort. Using Eagle, I have designed my first full and complete circuit board design ready for fabrication. I didn’t take the task lightly, I read tons of articles about design rules and best practices. I spent nearly a week getting this design juuusssst right. Now it’s your chance to tell me everything I did wrong! Your comments, no matter how brutal, are welcome. Attached is a zip with the board and schematic, all the gerber layers, and everything else related.

This is not an Arduino project, but just a couple of logic chips and a timer to flash a bunch of LED Christmas lights for a twinkling effect.

Thanks! (1.07 MB)

So, where’s the beef ? (zip file)

Beef is now on the grill. Zip file didn’t upload the first time (too big, had to remove jpg renderings) then had to wait 5 min to repost.

OPs PCB jpg file.

Tom… :slight_smile:

Ah, you used one of the same sites I did to preview my work. Greate site!

Well, you asked for it. Since I know someone else is going to say this I might as well say it now. Whenever designing a pcb with digital ICs, you should have 0.1 uF decoupling caps as close to the positive power pin of EACH chip. (yes, that means within 1 cm). I don't know where to find an example but I'm sure someone else can. I don't design pcbs so I would guess they would be ceramic but could be something else:


When physically placing decoupling capacitors, they should always be located as close as possible to an IC. The further away they are, they less effective they’ll be.

decoupling caps

decoupling capacitors (one per I.C. at a minimum).

I always add mounting holes 6-32 or 4-40 in the corners.


Show us the top of the PCB.


The bottom of the board looks weird, like it has two ground planes. I was thinking that there's an analog and a digital ground plane but that's not it. The second area fill is the VCC power.

Unless you are pushing BIG AMPS through your board, the normal size traces are just fine for power. There are online calculators that work out how much current you can put through traces of specified thickness and width. I often design with 10 mil traces (0.010") for signals and 16 or 24 mil for the main power trace. If you do need big amps, draw on the solder mask layer above the 24mil trace so that it is left as bare copper. Then flood it with solder or even solder solid copper wire on top of the PCB.

There are a number of possible reasons for pouring ground everywhere, on both sides: 1. It makes for some pretty good RF shielding. Every trace has ground nearby and on the opposite side, so it is all shielded from impulse and RF noise. 2. Almost every component needs to connect to ground. Pour ground everywhere and then every component has a nearby ground. 3. Some PCB manufacturing processes are subtractive, which makes it faster and cheaper to leave copper on the board. It adds no cost to the additive processes. 4. Extending the shielding idea, analog circuits really need a good solid ground, which is not affected by the digital switching noise from the rest of the circuit. So sometimes you will put cuts in the ground plane to stop the return path for digital signals going right under your analog components.

I start with a guess at the overall size of the PCB and then I put ground planes on both sides. Every component that's dragged to the board will pick up all its ground connections on the next "ratsnest" command. There's no need to draw traces "under" the plane like you have.

Why does your schematic connect VCC and VDD everywhere? Why is VSS and GND connected everywhere? That might be why it is complaining at you. Each "net" must have only one name. Connecting a green schematic line to a GND symbol will name that net "GND" for you. It can't have two names. You might have different power rails for different purposes (12V, 5V, 3.3V...) but those should never be connected - which is why they have different names.

Once you get a bit more comfortable making PCBs and you find a good supplier with a good soldermask process, then you can switch to SMD components. With a stencil and solder paste, it's much easier to get a much better looking result and you get to select more components that only come in SMD packages.

Of course, I would not have used a 74HC154 chip. That's only able to drive 25mA and, as you wrote in your notes, it needs different dropper resistors for different supply voltages.

A MAX6971 can drive a lot more current and it will do that with varying supply voltage and different numbers of LEDs on each pin. Only one resistor is required to set the output current. It's a serial-to-parallel converter so interfacing might be a little more complex than the circuit you've drawn.

Hi, Can't see the other layers, without getting Eagle fired up. Can you export the different layers as jpg/png?

Tom... :)

Thanks to everyone for the feedback so far! I do appreciate it. (And good Karma to you all!)

Decoupling Capacitors: Know about 'em, but this thing has no processor and the oscillator runs at under 100Hz. In this case, according to what I've read, they're not needed.(?) But that does bring up an interesting question: The power supply will be a good distance away and this will be powered via a long wire. So I was thinking of adding a, say, 10uf or so capacitor across VCC and GND to smooth out any noise or interference on the power line.(?)

VCC connected to VDD: because in the Eagle parts libraries, it is not consistent how parts get power. Some use VCC, Some use VDD, and some use GND and some use VEE or VSS. Slowly, I am building my own personal parts library and correcting some of these inconsistencies.

Ground (Power) Planes: There are actually 3. VCC, GND, and the LED common along the right edge. Total current draw is only about 30ma, so big planes certainly are not needed for power. But at the low frequency, neither is a RF ground shield. Having the VCC plane on the left side and the LED Common plane along the right edge simplified the layout and made it cleaner.

Mounting holes: Not needed for the current project, but good suggestion! I think I will add them. I'm gonna end up with 40 of these boards even though I only need 5. The rest may get repurposed so the holes might come in handy later.

MAX6971: Great chip, love it! But VERY EXPENSIVE (even the Chinese counterfeits) and would require more sophisticated and expensive circuitry to feed it. Also, only 1 output needed at a time.

SMD: As discussed in the design notes, I considered it, and for the reasons given in the notes decided that DIP and thru-hole was a better option for this particular project. May reconsider it in the future.

Keep the feedback coming! And if someone can explain why I truly need the decoupling caps on this low-frequency, no-processor circuit, or if I should add a power cap, I'm listening.

Pic above is the bottom of the PCB. Here's the top: |500x386

You are switching relatively large currents (25mA) with a digital chip. This will generate very sharp square waves, which will contain high frequency components. Even though you are switching infrequently, you are still using digital chips. Yes it will work 99.99% without the decoupling caps but it is good practise to put them in, for your future designs which actually need them.

There are formulas for working out what power supply smoothing you need. Usually you would always need a bulk capacitance such as an electrolytic. With long power leads that is even more important. 10uF to 100uF is probably about right for this circuit.

I don't usually consider the RF radiated from my circuits. The shielding of the ground planes is to prevent it coming in. But that does usually do a good job of not letting it out.

LarryD: decoupling capacitors (one per I.C. at a minimum).

I always add mounting holes 6-32 or 4-40 in the corners.


One per power rail, that means Vcc and AVcc on the '328

Why not ground-pour on the top. Ground pour both sides, cross-connected with vias to form a continuous ground plane is the way for high-speed logic. Its especially important when lots of signals run in parallel that there is a parallel ground route for the return current, otherwise the return current transfers to the parallel signals and you get cross talk.

Whew! Managed to cram in 3 decoupling caps, a power filter cap, a reverse-polarity protection diode, and 4 mounting holes! Then managed to cram in the new labels and rearrange them all so hopefully its not toooo confusing which label is for which part. Left the power plane as-is. (Will pour the whole thing, including possibly the top as Ground if I do something high frequency where RF matters.) It was a tight fit, will definitely have to reconsider SMD if I make more of them.

I think it would look more festive in red.

Make sure the package you buy for the 154 matches the PCB I.C. footprint, 3/10" wide.


If you plan to use screws with the mounting holes, make sure there aren’t any components within the diameter of the screw head.