1
\$\begingroup\$

I am trying to design a Z80 Computer Boards from scratch, just relying on the Z80 datasheet and some assembly language tutorials (I have no experience with the Z80 and never used them before but I am learning computer engineering with it), I used an NMOS Z80 on a breadboard with pretty low operating frequency which result in unwanted reactions, after asking on another SE site I identified the problem, here is the other question if you want to see it.

So I have been designing a mother board and some cards to Home make those PCBs, yet it is the first time for me to design sensitive card circuit which should avoid any distortions that could affect the CPU (I am an Electronics hobbyist and learner at school so I don't have much experience in sensitive designing stuff), I tried to have smooth circular edges so that no radiations are emitted from my circuit but My question is: will those diagonal lines in my circuit affect the sensitivity of this circuit? plus is there anything I am missing in my design? (adding a ground plate is quite impossible for me)

enter image description here Here is my design

Shall I consider anything else in my design? I am actually willing to operate the Z80 at maybe 2 MHz or up to 10MHz if I replaced my CPU and I want my PCB to be ready for that, I actually have a limitations as I will manufacture it at Home, which is traces width shall not be smaller than 0.5mm and I shall have a clearance of at least 0.45 mm so I could refine the manufacturing if anything went wrong. Please if you have suggestions about it please tell me.

Thanks in advance.

\$\endgroup\$
9
  • 4
    \$\begingroup\$ Curved corners to avoid radiation is something you might do for signal rates above 10 GHz. Even then there is mixed data about whether it provides any advantage or not. At 8-10 MHz, there's no technical reason to do it. If you want to do it because it looks nicer, then that's fine, it won't cause any problems. \$\endgroup\$ Commented Aug 4, 2020 at 16:04
  • 2
    \$\begingroup\$ If anything, it has less coupling to other traces than if they were parallel. \$\endgroup\$ Commented Aug 4, 2020 at 16:09
  • 7
    \$\begingroup\$ A bypass capacitor on supply pins should be drawn there. \$\endgroup\$ Commented Aug 4, 2020 at 16:13
  • \$\begingroup\$ 10MHz clocks with have harmonics due to rise time f=0.35/Tr perhaps > 50MHz which promotes some crosstalk on high impedance with a few pF better adjacent tracks only. 0.5mm traces are pretty fat these days. Better shops do 5 mil ( 0.2mm) track/gap and best do 3 mil allowing more tracks or interleaved. What is on the other side and how long are the interconnections? \$\endgroup\$ Commented Aug 4, 2020 at 17:01
  • \$\begingroup\$ @TonyStewartSunnyskyguyEE75 Sorry But I couldn't get your question, I guess I didn't yet learn such phrases, but what I understand is you ask how long is the copper traces, in this case actually I have two boards, one with 5 40-pin female headers all connected in straight lines and a card which is what I show here, so probably The trace length will not exceed I think 15 cm long, and as you ask about trace width, I can probably manufacture my PCB with a width of 0.2mm but It won't be that easy and failure percentage will rise exponentially, I tried it before :) \$\endgroup\$ Commented Aug 4, 2020 at 17:09

2 Answers 2

Reset to default
2
\$\begingroup\$

There's no reason to use smooth traces at the frequencies you're working with. 45-degree corners are fine (they're done that way for manufacturing reasons, not SI necessarily.)

What is important, however, is that the Z80 signals have return paths. As you've shown, all your signals share only one ground, pin 29 of the IC. That's not going to work so well.

You can improve things by adding a ground plane to your board, and add some local bypass caps to VCC.

\$\endgroup\$
0
\$\begingroup\$

You won't have any problems with radiated noise at the frequencies and rise times you're working with. Since you are making these at home and don't have much experience doing so yet, I'd suggest using wide lines and large spacing to make it easier to fabricate. After you make a board or two you'll get a feel for it but the first boards might be pretty rough!

For reference, things that need to be considered at higher frequencies (GHz):

  • Radiation at frequencies determined by the rise time of clock/pulse edges - this is the highest frequency content
  • Radiation of the clock/data frequency and its odd harmonics
  • Coupling between adjacent/sensitive lines of these radiated noises

Mostly your circuit isn't too sensitive because it uses 5V signaling. Normal TTL interprets anything between 2V and 5V as a logic high, 0V to 0.8V as a low. It tends to take a very large amount of noise to throw a signal outside of those wide bounds. It's possible, it happens, but it takes serious interference.

Your circuit also isn't too sensitive to layout because at lower frequencies there just isn't as much effectively coupling between structures. Again, there is coupling, it's just pretty low compared to GHz signals.

The more common trouble spots are missing bypass near supply pins of each IC and using super long ground traces or wires for ground connections. Good luck!

\$\endgroup\$

Start asking to get answers

Find the answer to your question by asking.

Ask question

Explore related questions

See similar questions with these tags.