I recently made Ben Eater's 6502 computer on breadboards, and I wanted to clean it up a bit. I designed the PCB, but with it being so complicated and my first PCB I made, I wanted to make sure that I made it correctly. I've already double checked it, but a fresh pair of eyes will probably help. Thanks!

Please review my PCB design with any issues I should look into.

front wires on top of back Files: https://drive.google.com/drive/folders/1yyrIxZ05xRHf_6apyVWN-MqQjlgbEwbP?usp=sharing

Ben Eater's Schematics: link

  • 2
    \$\begingroup\$ The first thing I notice is that you've omitted the decoupling capacitors ... you really do need them you know! \$\endgroup\$
    – jonathanjo
    Jan 10 at 16:39
  • 2
    \$\begingroup\$ ...and the power supply tracks are wholly inadequate. I think you should look at some articles and examples of good PCB design and do some more learning. \$\endgroup\$
    – Finbarr
    Jan 10 at 16:52
  • 1
    \$\begingroup\$ Your tracks are really unnecessarily thin and I would suggest redrawing with a very coarse (by modern standards) grid of 0.1-inch for the pins, and 0.05-inch for everything else. use much bigger vias. Allow a lot of ground. Give yourself space. \$\endgroup\$
    – jonathanjo
    Jan 10 at 16:53
  • 2
    \$\begingroup\$ Your layout software should also have Design Rule Checks, these will spot basics like tracks too close or touching pads/vias. \$\endgroup\$
    – Finbarr
    Jan 10 at 17:02
  • 5
    \$\begingroup\$ Voted to reopen. One major problem at a glance is that there's no decoupling caps. This might be because the schematic uses the old rotten way of placing caps in a dark corner of the schematics, so that nobody has a clue about which IC they belong to. Proper schematics place decoupling caps directly on each Vdd pin. \$\endgroup\$
    – Lundin
    Jan 11 at 12:03

2 Answers 2


For a first stab at a PCB, this is a pretty good start. But not good enough to go to production with.

The first thing you did which was excellent was ask for advice and review! As you have already built it on a breadboard, you definitely will be able to make a good working PCB for it, so stick at it.

Everybody will make the following assumption: that you're using the schematic capture portion of your CAD tool, but your files show that you are not. Until you do this, you are tying your hands behind your back and you will almost certainly not succeed in a good working circuit.

I see you're using KiCAD, which is perfectly good choice for this kind of project. Take the time to learn to use it, in the first instance, by redrawing the exact schematic of the circuit you want. You'll learn an enormous amount. The when you flip to PCB, you'll find your lift so much easier. Anybody who designed PCBs before CAD will confirm this. Even just checking that the nets are correct is a very laborious task without CAD: and this is what you have to do with your design as it stands, because you didn't use the schematic capture of your CAD tool.

You will need a library of 6502 symbols (specifically the CPU and the PIO 6522. There's one from Alarm Siren's repository which I believe is the one most people use. You could make your own, but that's not recommended for a first project. (It's a very worthwhile thing to do, but not the best place to start.)

This is a composite of the things mentioned in comments.

  1. Decoupling capacitors There are three in the original circuit diagram but none on your board
  2. Power tracks Your power tracks are certainly too small
  3. Ground plane It's (almost always) a good idea to have a ground plane


  1. Use a good grid For a first PCB, with plate-through-hole components, my suggestion is use 0.1-inch grid for the component holes, with an 0.05-inch grid for the tracks.
  2. Use fat tracks I'd suggest 0.5 mm tracks for general, and 1.0 mm tracks for power, a whole-side ground plane. Many people find it good to use one side for vertical tracks, one for horizontal, and it makes a nice clean layout.
  3. Use the design tools In particular, the Design-Rule-Check. Amongst very many things, it checks the PCB matches the circuit, and checks things aren't too close to each other or short each other out. As it stands, your PCB has hundreds of errors -- but most are caused by not having labelled nets, and will disappear when you use the schematic capture.
  4. Design in good order Place your mounting holes, connectors, switches, indicators first, then main chips, then subsidiary parts. Then design power and ground. Then put in the decoupling capacitors. Maybe add some depending on how the layout looks. Then start tracking. Do not be afraid to undo things, try things, redo things.

Some thoughts

  1. ZIP-socket for the EEPROM is a great idea
  2. Perhaps add a power-good LED.
  3. I like to add a pair of holes to make a "croquet-hoop" on ground, for attaching scope probes to
  4. Consider adding the switches and so on from the original design.

Concrete Suggestion

Here's a beginning of a layout which is along the lines I've suggested: with a ground plane (on the top), fat power (on the top), and the beginnings of tracking the database (on the bottom). Notice in the second image, because the circuit diagram is in KiCAD, it can label every signals, and show you the "airwires" of signals which still need tracking.

enter image description here

enter image description here


Ignoring that the schematic doesn't quite match the layout in many places, then:

Major remarks

  • You should have a more careful ground layout, start with it. Place for example all GND traces on the solder side and all +5V ones on the component side. Make sure that each and every GND pin takes as short a path towards the supply connector ground pin as possible. Wider traces don't hurt. Don't hesitate to connect different GND traces with each other. You can think of the supply connector as the root of a tree, with ground traces as branches and do a layout roughly like that.
  • Your board completely lacks decoupling caps which will become very problematic, particularly with old parts like these. Each and every VDD/VCC pin should have a 100nF (unless the manufacturer gives more detailed recommendations) decoupling cap close to the pin, the other side of it routed to ground.
  • Add designators to each component on the PCB, even if you don't order with silk screen. The game of "guess the component" turns old quickly.

Minor remarks

  • Don't use polarized caps just for the heck of it. For 100nF you can use ceramic (recommended) or film caps.
  • Always avoid 90° bends on traces as a good habit, to avoid crosstalk.
  • 1k pull-ups can be swapped to 10k without any problems, for less current consumption.
  • Maybe consider a LED on the supply and maybe one on the reset, to quickly spot if things are alive or dead.
  • There's probably no good reason why you can't have a local voltage regulator for improved EMC characteristics, even if it's just some old LM7805.

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.