Hallo Garth,

Thank you for your huge answer!



I held them against the light and could see the traces of the other side. The IBM boards had extra layers for sure: no peek through. There weren't +5V and GND power traces to be seen either. Those of the clone boards were clearly visible. When at home, I'll make a picture of one of them.


Very revealing and clarifying!


I have this ATX board in mind, a XT clone:http://baltissen.org/images/ATX-brd.png


Read that yesterday but didn't understand it at that time. Having read more of your explanation, I start to understand it.

Many thanks!

_________________

A Juko 10 MHz with a V30: http://www.baltissen.org/temp/IMG_1431.JPG

A unknown clone, 8 MHz: http://www.baltissen.org/temp/IMG_1432.JPG

OK, not the best photos but certainly only two layers.

_________________

There's a great demo I once saw showing how return currents in a ground plane follow - or try to follow - the forward path in the signal layer. I've tried and failed to find it. But I did find this demonstration, probing a deliberately defective ground plane with an inductive probe:
Gaps in Return Plane Demo

posted on stardot in response to Chris Morley:

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

I read through this thread and found many interesting links. I took Dr. Howard Johnson's week-long classes twice and they were certainly very instructive, especially in high speed designs involving modern FPGA, processors, and transceivers.

However, with 5V, hobbyist, retro designs I don't worry too much about high speed effects. Just about all my retro designs are under 30MHz. The pc board designs are all 2 layers. There are several reasons for this relaxed attitude:
1. Small pc board. Most (actually all) of my designs fit within 100mm X 100mm pc board. The round-trip propagation delay is less than the edge rate of the retro logic, so reflection is not generally a problem in small pc board.
2. Slow retro logic does not have the fast output drive capability to cause problem and the inputs have good noise margin and are too slow to see fast glitches.

I do have certain design rules I follow for retro designs:
* Use the slowest parts. Don't use fast logic if they are not needed, use slower RAM and ROM where possible.
* Reduce the signal distance by packing components as close to each other as possible. Use aggressive design rules and don't worry about too many vias. Auto-router is a wonderful tool, use it. Take advantage of the pcb fab capability where 7mil trace and spacing and tiny via are highly producible.
* reduce the design area by 50mil all around and bring multiple ground and VCC points to the edge of the board. When the routing are completed, expand the board outline by 50 mil and hand route a ground ring on one layer and VCC ring on the other layer. This give extra return paths for the signals and can really help the ground problems.
* clean clock is important. Design in series termination and test points for clock
* check your design margin by REMOVING all bypass capacitors as a test. You design should work with no or few bypass caps. Raise and lower the supply voltage by 5% and increase the clock by 25-50%
* If you suspect noise problem, reduce supply voltage, add more ground jumpers and test again. More ground, slower parts and terminating fast clock and control signals usually will solve the noise problem.
Bill

It seems to me that a lot of beginners want rules that, if followed, guarantee their design won't fail. But I don't think that there are such things. I like to think of it as: you pick and choose how and where you want your system to fail, and how much time, effort and money you want to spend mitigating these sources of failure. As your expertise grows, you will start using your knowledge in integrated, holistic ways that cannot be captured in rules, and you too will probably one day experience the frustration of trying to answer a beginner's questions by "back-forming" a set of rules that would have produced the right answer in those particular circumstances. (Just to leave no doubt: I am nowhere near this high level in hardware, though I am in certain areas of software.)


That's a brilliant article. I crack up every time I read, "Some people worry that conduction electrons are traveling so fast that they won't be able to make it around a square corner. Perhaps they might reflect back or fly off into space."

(I imagine that certain types of audiophiles have special paint that they can put over circuit board traces that would help reflect back into the traces any electrons that might fly off them. This might relieve a certain "hollowness" in the upper mids. But only a thin layer of paint must be used lest phase coherence be reduced!)


I read something really good, here or elsewhere, about ground return following the signal path and how power and ground planes work, and I felt that really helped me get what was going on. Maybe it was a combination of posts and that's why I can't point to just one.

But anyway, if I understand it all correctly, the real advice is not that fills are useless, but: "You can't assume that just pouring some fills will help anything at all." But fills can be useful, as opposed to not having them, if you have conductors on the other side running across the fills where going across the fills would be a preferred route for return current, right? And in those cases it's not the fill per se being useful there, but just the parallel current path, and just doing a ground return trace following the current trace on the other side would do just as well, right?

_________________
Curt J. Sampson - github.com/0cjs

I just found a recent video by Robert Feranec where he simulates some serpentine trace paths over a ground plane and shows the return current paths. The video itself is a bit long and has a few unresolved issues, but a couple of images from it make it fantastically clear how current flows in a ground plane work.

Here's what the return paths through the ground plane of 1 MHz signals look like:


And here's what happens when you have a gap in your ground plane over which the signal traces pass:

_________________
Curt J. Sampson - github.com/0cjs

Good find! I'm pretty sure I've seen a dramatic visual illustration with perspex/lucite but have never been able to find it again.

Illustrate perfectly why ground pour is ineffective in densely packed board. I prefer densely packed board to reduce signal length than loosely packed board with an effective ground pour.
Bill

Here's a keynote talk about multilayer PCB design:

The Extreme importance of PC Board Stack-up

It's about an hour. Several other related talks in the sidebar.

via

That one led me to another talk in that series, Eric Bogatin's The Value of the White Space. Even having read most of the stuff in this thread and seen the presentation you noted, this one (particularly from around forty minutes in) really expanded my understanding of what return paths are and how they work. Nearer the end it also taught me some tricks for dealing with interrpted return paths, such as by using return straps.

(Next on my list from there is a talk that I suspect may be close to the hearts of many here, Bil Herd on The Commodore Experience: Engineering the Early Generations of Home Computers.)

_________________
Curt J. Sampson - github.com/0cjs

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

As it turns out, the Bil Herd presentation is an interview, and though I'm sure the interviewer is fine as far as "modern" knowledge goes, she doesn't really seem to have the background in early '80s design to really bring out much of interest. There are a few good stories there, but they're ones that I'm sure everybody here has heard before, and in more detail. (For example, with a DRAM issue, using a light pen on a particular spot on the screen to trigger an analyzer to capture data at the right point to see the problem.)

So I don't think I'd bother with this one. But the other two that have been mentioned here are great, especially if you don't have a good intuition for what Maxwell's equations really say about PCB design.

_________________
Curt J. Sampson - github.com/0cjs

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

Over in this thread, BDD mentions that the ground pours are not a ground plane (which I knew) and also that they are actually harmful because they add "unwanted parasitic capacitance."

I have a vague understanding of what parasitic capacitance is, but I don't really see how the harm appears in this case. With what I understand from my post above on return paths it seems to me that while a ground fill may not help signal paths much (or even at all) if they cross cuts in the fill, the signal return path will never be lengthened by a ground fill, and may be shortened, so the capacitance of a signal path ought never be increased. Further, where power supply lines are crossing ground fill, I would think that this will simply add a teeny bit more bypass capacitance between power and ground (much less than would be provided by a typical bypass capacitor) on that area of the board, which never should be harmful (and might even be helpful).

So what's the issue here?

_________________
Curt J. Sampson - github.com/0cjs