Vertical/Horizontal tracks grid - Page 1
Forum section: electronics / general

author: josuah
author_rank: Regular Contributor
timestamp: June 24, 2022, 03:08:20 am
content: I just came upon that design file from Silicon Labs, for their dev board.While I am used to PCBs with tracks going from source to destination, these guys are using a different approach:The top copper layer has traces going vertically only.The bottom copper layer has traces going horizontally only.And vias reach the dots.There are very few exceptions.That looked like a very pragmatic approach to PCB design that can solve most if not all wiring.Is it a well-known method? Any advantage or downside you would see for it?What is your opinion?

author: ataradov
author_rank: Super Contributor
timestamp: June 24, 2022, 03:16:15 am
content: This is a standard method that was used since 1970s at least. This was used on all old computers full of DIP ICs. This is basically the first routing method after they were done using mylar sheets and black tape.This looks like a job of a really basic autorouter. Or they went for a vintage look.This is absolutely horrible for signal integrity. It probably does not matter on a board with slow ICs, but I would not use that as a universal method.Look at USB routing. This is nuts. I assume USB here is full speed, so it does not matter, but this routing at high speed would be questionable.

author: Feynman
author_rank: Regular Contributor
timestamp: June 24, 2022, 09:37:40 am
content: Quote from: josuah on June 24, 2022, 03:08:20 amIt is even an exceptionally well-known methodI don't see any downsides from this routing technique alone. General principles for signal integrity, power integrity, EMI, DFM and so forth apply to this technique as for every other technique, of course.

author: josuah
author_rank: Regular Contributor
timestamp: June 24, 2022, 11:52:21 am
content: Quote from: ataradov on June 24, 2022, 03:16:15 amThis reminds me of these single-side PCBs with all tracks at the back, and plain wires soldered like THT components to jump over something else.Quote from: ataradov on June 24, 2022, 03:16:15 amIIRC vias can introduce some noisehttps://www.nwengineeringllc.com/article/img/via-induct-3.pngand this has a via for every single net.As the T-Shirt says:https://farm6.staticflickr.com/5582/14248405503_a47ed6bb0f.jpgAs Feynman says, it does not prevent to keep an eye on...Quote from: Feynman on June 24, 2022, 09:37:40 amQuote from: ataradov on June 24, 2022, 03:16:15 amThis is a track hide and seek party!Thank you for sharing your seasoned feedback on it to me freshman.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: June 24, 2022, 12:16:54 pm
content: The attached picture is only of one side of an old TTL PCB, but you can guess what the other side would look likeThe tracks on this side are also not completely vertical, but by allowing some small bends the number of via's is reduced quite a bit. Also note that power (and GND) is also routed in the same pattern.

author: josuah
author_rank: Regular Contributor
timestamp: June 25, 2022, 11:36:00 am
content: It looks like, instead of today's single-chip'em'all approach, aggregating many chips together in a grid was much more common.In a grid array, routing things with that grid method even sounds like the only possible way.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: June 25, 2022, 01:33:41 pm
content: It is indeed a way of routing that fits very well with that kind of circuit, but only with that kind of circuit.Quote from: josuah on June 24, 2022, 03:08:20 amSo the method is well-known, that's clear by now.It does not solve "all wiring". It does not make much sense for discrete analog circuits, where most footprints have 2 or three pins (resistors, capacitors, transistors). Analog circuits quite often also have severe constraints for voltage drop due to current through PCB tracks. Forking of a T on the wrong side of a track can ruin a design, especially where high currents and sensitive inputs come together in products such as for example audio amplifiers. An audio amplifier can have 10A (or more) currents though it's power and output section, while the input is around 1V max, but also with a dynamic range of 120dB or so, which means signals down to microvolts are important.And indeed, also by high pin count IC's that kind of routing simply does not work. IC's with 1500 pins are not exceptional, and for those you need multiple layers just to get the tracks away from it. And with today's much higher signal frequencies, signal integrity is a much bigger concern and things like differential pairs and length matching for bus signals is mandatory. Quite often it does not matter much how long a track is, but via count is reduced to a minimum for a lot of signal tracks because they cause impedance mismatches because of their irregular shape.Also note that an IC with 1500 pins is quite likely to have 200 or more pins (pads, balls) just for GND and power, Decoupling of the power is very important. High end PC processors can have a TPD of 200Watt or more, while the core works with a voltage of around just 1V, and that is more then 100A (over different power rails) going to and coming from such an IC. 100mV ripple on the power supply probably also kills the whole thing, while 500mVpp of ripple does not matter at all for those old TTL boards.

author: josuah
author_rank: Regular Contributor
timestamp: June 25, 2022, 11:57:53 pm
content: The word "solved" in "can solve most if not all wiring" was chosen poorly by me: as you teaches me, if a signal is carried from point A to point B but barely looks like what it was at the end, nothing is "solved".Textbooks are teaching the basics of electronics with wires linking components.PCB design seems to pay attention to just these wires that "do nothing":QuoteI am impressed by these BGA fanouts. Nothing like what I am used to play with!Quote from: Doctorandus_P on June 25, 2022, 01:33:41 pmThe more I read about it, the more I realize that precaution used for kilometers transmission lines should be taken for tracks on a PCB if dealing with such frequencies.QuoteSo reducing a chip power (for permitting embedded low-power for instance) could also be a matter of being able to reduce noise, or the (too low) signal would be burried down the noise?QuoteI imagine this refers to decoupling capacitors? Or is it using separate ("decoupled") ground zones to isolate the noise from the various kind of signals?I learned plenty today!

author: eugene
author_rank: Frequent Contributor
timestamp: June 26, 2022, 03:26:08 pm
content: Maybe only marginally related, but when I layout a PCB with multiple internal signal layers, I just naturally tend to put most of the traces that are mostly vertical on one layer and most of the traces that are mostly horizontal on another layer. All of these traces are accessed through vias anyway, and it's a relatively quick way to a clean working design.