hckrnws

> Other than increased miniaturization, the most striking change is the use of copper pours [...] Why did we start doing this?

We've been doing something a lot like this for as long as I can remember.

Back in the 1990s if there were any big unused copper areas on your PCB you'd mask them to save on etching acid - a gallon of acid would have a lifetime measured in square inches of copper removed, and the less copper you removed, the longer your acid would last.

Meanwhile, a lot of DIY etching processes were very basic. Sure, you could get translucent acid and a transparent bath and heat it to a controlled temperature and run bubbles through it and so on. But if you were on a budget, some room temperature ferric chloride in an old ice cream container would get the job done. And getting the etch resist onto the board? You could draw it by hand with special pens, use transfers, there were special printer toner transfer papers, or you could DIY UV photoresist using printable projector transparencies and the sun as your UV source.

This was not a super-scientific, tightly controlled process.

If you had narrow traces and narrow gaps on one part of your PCB, and large areas of copper to remove on another? Well, if you left it in the acid long enough to remove that large area, could be the narrow traces get etched away too.

So masking off any large areas meant all the copper getting etched was about the same width - thus compensating for the poorly controlled etching process.

Of course, these days professional PCB manufacturing is orders of magnitude cheaper than it used to be. When you send your design to pcbway or jlcpcb they have much tighter control over the process, so you no longer have to worry about this stuff.

> When you send your design to pcbway or jlcpcb they have much tighter control over the process, so you no longer have to worry about this stuff.

Funny that you mention jlcpcb. The last time I submitted a board with tight differential pairs (but still within their listed specs) to them they basically told me to increase the amount of copper, so I assume they had some quality issues in the past:

> we have new rule since Dec, 2022, if the copper areas are less than 30% of the board in each copper layer, the space between trace and trace should be at least 0.15mm to avoid short circuit.

So I had to add a few copper pours and everything was fine :)

Arguably, the fact that they knew in advance exactly what you would need to do to avoid the issue means their process control is incredible!

And that's one of the benefits of working with a high-volume prototyping service like JLC - they've built a lot of PCBs; they know all about how to maximize yield.

Well, you may not have to worry, but if you have large unpoured areas on a design with a professional PCB manufacturer (of the traditional, high-touch kind), they will ask if you want to pour some copper there. Reason being that it makes the process faster, more consistent and reduce possible side-etching on lanes. It may not a make a difference in most cases, but you may just save some time and effort by doing this.

The reason is that the copper is already there, it gets etched away. So it actually costs more to not have copper than to have it.

At industrial scale, surely they recover that copper from the etching fluid?

Even if they do, the recovery itself would surely have costs. It can't be easy.

Indeed, the enchant is very nasty stuff, it's not easy or clean to do so.

Yes, but this costs pales in the cost of redoing in case of problems with side-etching and the overall tightened manufacturing constraints.

And yes, they get to recover the copper, at the very least to make treatment easier for discarding (copper is a very bad pollutant). But not only there's a cost, this is dealt with by waste treatment companies that will at most use the copper value to recoup some of the cost of the treatment.

> The return current on the back is free to spread out, but in practice, it will prefer the path of least resistance — i.e., the shortest line between the two vias.

This is a bit misleading. It does preferentially flow along the shortest path, but not exclusively. It will indeed spread out. It takes all paths with a current proportional to their resistance, not just the shortest path. The percentage of total current that isn't flowing directly along the shortest path is still very significant.

Think of it as a bunch of resistors in parallel. The shortest path might be 0.1ohm, and the longest path 10x longer at 1ohm, but current will be flowing along both of those paths. If 1A is flowing down the shortest path, you will still have 100mA down the 10x length path.

At DC this is a good model. At higher frequencies no so much. At high freq the 'return current' is all basically right under your trace.

I don't know anything about electricity so this intrigued me. Is it related to the "proximity effect" [0]? Is it caused because of the fact that the magnetic field created by high-frequency current is always changing, so this induces a voltage in any nearby conductor?

[0]: https://www.sciencedirect.com/topics/computer-science/proxim...

When the frequency of AC divided by the speed of light gets close to the length of your wire (ie. around 1Ghz), the regular rules of electricity no longer apply.

In the high frequency rules, you should consider that the energy you're sending down a wire is instead transmitted in the insulator - ie. it is effectively a radio wave guided by the conductors on either side.

If one of your conductors is not a wire but a ground plane, then the radio wave will travel in the insulator between the other wire and the closest bit of ground plane. Further away bits of ground plane, the signal gets effectively cancelled out because all the alternate paths the signal could take all have different path lengths and therefore phase shifts.

Energy is always transported in the insulator, but the bigger point is valid - at high enough frequencies you have to actually think about it.

One of my all time favorite videos (one of the few that I rewatch once per year) is "The Extreme Importance of PC Board Stack-Up with Rick Hartley". It's fantastic.

https://resources.altium.com/p/the-extreme-importance-of-pc-...

Hartley is awesome. Plus one for that.

Grumble grumble. Professional here, and I really do not like this article.

There are a lot of things getting mixed up here: ground planes for EMC, ground planes for electrical performance, ground planes for DFM/etching, and ground planes as "fashion".

First off, let's just say that meeting radiated EMC ("47 CFR Part 15" according to the article, equivalent to CISPR 22/32 in Europe) is a bloody good idea. Yes, the testing labs are "a bit of a racket". But does anyone else remember the days when turning on the vacuum cleaner would knock out the TV? That wasn't great. And we have a whole lot more electronics in the world today. A world without Part 15/CISPR is an ugly world indeed.

Four-layer boards are cheap. Really cheap. They may be double the cost, but you're doubling pennies here. In fact, just checking in with one common low-volume supplier, they're not doubling: the price for 200mm × 100mm boards with good specs goes from $9.34 each in quantity 10 to... $10.59. For prototypes, that's basically a rounding error. Perhaps even literally a rounding error. So don't complain about the cost of four-layer boards anymore, it isn't 2004.

Internal ground fill layers are what people usually mean when talking about "ground planes". They have three key properties:

1. They are very easy to do and are very tolerant of mistakes. You don't have to calculate return current paths, you don't have to size and locate return current traces, you don't have to gum up your routing. You just dedicate the layer and it works, and it keeps working if you have to make changes later.

2. They help shield internal layers further down in the stack from radiating. This is usually minor, but for nasty digital stuff or high-power electronics, can be useful.

3. They develop inter-plane capacitance with nearby power layers, if inter-layer dielectrics are small. This is critical to maintaining power distribution network performance at high frequencies (>100s of MHz). This stuff is very, very important to make high-speed digital logic work well. Of course, it's only one link in the chain (GHz stuff gets handled on-package or even on-die; <100MHz is the job of on-board capacitors until you get into power supply dynamics in the kHz and below). This is the "increasing shunt capacitance" mentioned in the article. Yes, it can be bad news for analog stuff, but this is both very rare and the sort of problem where anyone who can do that kind of difficult analog design has the skill to punch a hole in the plane where it's needed.

There is also a manufacturing issue where the manufacturers find it easiest to have approximately balanced amounts of copper on opposite layers of a board. Copper pours are one solution to this. Copper thieving pads are another. This is important but easy to manage, and vendors are good at it.

So all of the above applies to internal layer copper fills. None of it is "fashion": there are good reasons to do it, the extra layers are cheap these days, and it's an easy and robust way to design things. Fills on external layers are a different matter; they're kind of stupid in a lot of cases. Unless you're doing a two-layer design, or a 4-layer that kind of ends up behaving like a 2-layer (this happens sometimes when stuff is very tight), the external fills are pretty worthless. I wrote more about this ages ago over here: https://www.eevblog.com/forum/eda/altium-article-on-never-us... This is the only real thing I'd agree with the article on.

There's a lot of stuff going on here, and I don't think this article does a very good job keeping it straight. If you take one thing away from all of this, it should probably be that internal copper planes are pretty great, and what happens on the outside of the board isn't so important.

A reason for more external copper pours might also be that the EDA tools have improved and can now handle the complex shapes. Back in the 80s/90s copper pours were a pain using Protel (later called Altium), as they were built using straight tracks rather than polygons. Eventually the program got actual polygons and life became easier.

Piggybacking onto this comment, but another reason for external pours is thermal performance. A copper pour on the surface on the PCB allows heat to convect off the board more easily. The gains aren't massive, but they can help as part of a larger thermal management scheme.

I've also heard, possibly apocryphally, that in the old days when we used harsher chemical etchants, removing all of the copper from unused sections of the PCB would increase the risk of thinning the traces beyond what was intended. So in those cases a copper pour would reduce the time the PCB would need to spend in the etchant bath.

I've worked with several stepper motor driver ICs that feature a ground pad on the bottom of the IC and recommend an unmasked copper pour connected to the ground pad via thermal vias, on the opposite side of the board from the IC, sized at least as big as the IC itself. Like, the manufacturer's suggestion is literally to use the copper as a heat sink. If you wanted, you could then affix dedicated heat transfer features, like a traditional finned heatsink, or a heat pipe to a dedicated cooler.

Thermal pads are wonderful. Most of the time for moderate thermal loads, an exposed pad soldered to an internal ground plane running through the whole board is enough, as the copper layer there spreads out the heat well enough to dissipate. It always amazes me that an outer-layer copper fill is not much better than an inner-layer one, so the larger coverage of the inner layer wins every time.

A great app note on getting started with thermal design from TI: https://www.ti.com/lit/an/snva183b/snva183b.pdf

Going by the inconsistent spacing and angles on that 1984 PCB, I'd almost guarantee that it was routed using black tape on mylar film, not a CAD package to be seen. Trying to create large fills back then would require manual positioning of tape over all of the copper fill areas. Tools is a big part of the reason for the shift, it's easy now, and the results are generally much better.

I think that one was actually done in an early Japanese computerized CAD package. There's a lot of weird crap in that layout, but it's the sort that the old-school computer layout programs made, not the sort that humans did. Take a look around U111 pin 30, or south of R112, or, heck, any of the text. Whereas there's no sloppy-but-OK vias or wobbly text or anything like that.

I actually prefer using plane layers with tracks to split to the messiness of polygon pours. It signals design intent to users and fab houses and doesn't require a ton of rules and calculations. Polygon pours have their place in top/bottom power nets.

"There's a lot of stuff going on here, and I don't think this article does a very good job keeping it straight. If you take one thing away from all of this, it should probably be that internal copper planes are pretty great, and what happens on the outside of the board isn't so important."

And then this article totally ignores solid metal PCBs, which are my realm of specialty and have their own inherent challenges when it comes to digital equipment.

So is the default for a 4-layer board something like components/ground/power/components?

The default today is likely signal/ground/ground/signal.

Or really, the default today is a 6 layer board because 4 is still kinda bad.

Today's engineers know that signal-top has a return path through ground-top. But if you ever were to via a wire from signal-top to signal-bottom, the return path gets lost (aka: return path is now through the board or worse, through the air and radiating off of your board).

To prevent this erratic behavior, you must continue to think about the return path and tie a via from ground-top to ground-bottom as close as possible to the via between signal-top and signal-bottom.

--------

6 layer can do signal/ground/signal -core- signal/ground/signal

Where core is the FR4 material (keeping the middle signals far enough apart that they likely don't interfere with each other). This allows vias between layer#1 and #3 without needing a secondary return via. (But if you need layer#1 to layer#6 via, then the previous advice still applies where ground-top needs a secondary return via to ground-bottom).

For anyone else that also wants a much more in depth explanation, this hour long talk is a gem.

https://resources.altium.com/p/2-the-extreme-importance-of-p...

That AC signal energy is contained in the field between the trace and it's return is such a powerful model compared to taking the DC model of "going the lowest impedance path" and just assuming it applies at AC. Very, very, very good talk.

This model also automatically makes clear why you'd want signal-GND-GND-signal instead of a power plane because that side's signals will have coupling into the power plane. It is mentioned explicitly in the video as well.

> 6 layer can do signal/ground/signal -core- signal/ground/signal

So preferring a fourth signal layer before adding a power layer?

Just route power as a signal. Maybe a really fat trace / signal but it's still a signal.

Power planes are overrated especially for 100mA designs. If you are running a 500Amp GPU obviously you should consider a power plane but what kind of designs are people doing here?

EDIT: 10 Amp on 1oz according to first trace width calculator is supported by 20mm or 300 mil trace width. There's no reason to have a full power plane on amperage grounds.

And if you need board capacitance for your design to work then yeah, Power Planes can be useful for that. But only the highest of frequency circuits (think GHz+) seem to require those.

And if you do use Power Planes, then return currents may be induced on the Power plane instead of the ground plane, which is bad and hard to think about. (Power Planes cannot be shorted to Ground, meaning your return current needs to go across a high inductance via, into a capacitor, through to the ground plane where the return current should have been in the first place).

---------

Basically, power planes are one of those things that work at 50MHz just fine (enough random capacitors that magically transfer signals to the ground plane). But much above that frequency and those capacitors look more like a parasitic inductor. 500MHz signals will NOT go through a 100nF 0402 cap, that thing is practically an indicator by those frequencies. So it's not like power planes are easy to use.

The people who 'Need' a power plane are doing far more complex designs than the vast majority of board designers. And if they really need it, then they are using complex FEA simulations and calculations of PDNs that far exceed the scope of the level of advice in this topic.

> EDIT: 10 Amp on 1oz according to first trace width calculator is supported by 20mm or 300 mil trace width. There's no reason to have a full power plane on amperage grounds.

I mixed up internal vs external trace width here.

700mil or 20mm internal trace.

300mil or 8mm external trace.

Yes and it sucks people copy this.

The default should be X / GND / X GND to maintain tight coupling of both signals and power to the GND plane and stitch the GND planes together with vias close to any other via that changes layers to maintain return paths.

Power should be routed normally, except it should use widest practical traces and get decoupled with C close to ICs that consume it.

But in any case, you always need to think about the signal and return. Even for power. It's never truly DC.

If you do the "classic" signals / GND / VDD / signals, you are routing over VDD plane and your ground is waaay farther. Means all accidental VDD noise (you can't pinpoint, because it takes frequency dependent paths across the VDD/GND C) gets coupled into your signals on the back side.

So don't do that.

I don't follow you.

The standard configuration, with a "fat core", is pretty much the best you can do in 4 layers for a "modern" design. By "modern" I mean something with a dense component load, probably double-sided load, and random-ish routing (so, exactly the opposite of the old '80s TTL design shown in the article image we're discussing in sibling comment). All the "better" 4-layer stackups require outer layers to be doing a lot of heavy lifting, which they cannot do if they are filled with parts. When you assume they have to be filled with parts -- because if they aren't filled with parts then I can make it smaller and people want that! -- then you just cannot use that space as anything else. Henry Ott discusses a number of stackup options for four layers, and the standard one is the only option of his that survives with this restriction. If you don't like that, tough, I guess you're paying for 6 or 8 layers. Which isn't too bad these days!

You complain about power (VDD) plane noise. This might be important in ultra-low-noise design, I don't know, I try not to do that sort of work. In normal work it is not a factor. Your power and ground planes should be connected by a pretty thick network of capacitors, so they are transparent to each other. Your power plane is as good as a ground plane for AC, and AC is the only thing that's hard to deal with. So there is no issue routing the bottom layer on the other side of power, not ground. (Of course, that is no longer true if your power plane is split. Split power planes in a high-speed 4-layer design can be nasty, and are how I justify my worth to my employers!)

Nailed it. This was confusing to me too hearing about other stacks, as they stopped being effective once I used the top (And sometimes bottom) for components, which happens on every design I make. If not, I'd shrink the design! EM concerns aside, I want easy access to power and ground.

https://m.youtube.com/watch?v=60RxCiZuD9E

Rick Hartley explains.

I don't think you are arguing for the same thing as Hartley. I strongly approve of some things he says: "people believe that just pouring ground on top and bottom lowers EMI... well it doesn't!" (6:04) or "there is no four layer stackup that's wonderfu... no 'gosh, isn't that great?' four-layer stackup, they just don't exist, it's four layers, you know, you can only do so much with it" (7:29). No mention of VDD noise or discussion of how a good, well-decoupled power plane is basically as good as a ground plane for AC return currents.

I believe you are trying to get a stackup that supports use of stripline for signals. That is a reasonable goal but it is only appropriate for very high speed digital designs. If you route stripline on a regular basis, you're either very experienced or clueless. No middle ground!

Really, for heavy-duty work, you need six. And you can argue with me, and say that by great skill you can get things into four layers, and that is true. But six-layer boards are cheap compared to what they used to be, so for anything not going into true high-volume manufacturing, just go for six or eight. In all other cases, the design cost hit will outweigh the parts cost savings.

Signal is a wide definition of possible traces. Signal can be status LED toggling every 3 seconds, it can be I2C in kHz range or SPI running 80 MHz or 100Mbps Ethernet. I don’t mind routing slow signals over power plane. For the fast ones I would go through pcb and route over GND plane with equal vias amount for each trace. So classic signals/GND/(split)VDD/signals is absolutely fine for simple applications.

There are different options.

If you put the power planes on the inner layers and the signal on the outer layers, it's much easier to visually inspect the signal layers. And if you got something wrong on the prototype and you have to fix it manually, the traces are right there where you can get at them.

On the other hand, if you're doing some performance-critical RF wizardry, you might put the ground planes on the outer layers and the signal on the inner layers, sandwiching your signal between two ground planes. So if you look at a wifi module or something like that, sometimes the outer layers will have very few traces.

Yep. And then for 6 layers, depending on the actual needs of the design, it'll often be components/ground/signal or power/signal or power/ground/components. Some designs need a lot of signal routing space. Some need a lot of split power rails. And some are nice and easy and don't need either.

If you don't need components on the bottom side, it saves money to not do so. That means the board doesn't need to go through another pass on the SMT machine.

Even if a board is double-sided, it is common to avoid putting major ICs on both sides, unless the space constraints are severe. Often, people will only put passive components on the bottom side.

A bit related: we developed CapExt for extracting parasitic capacitances and resistances on PCBs and 3D models. It’s mainly for capacitive touch applications, but it could also help in cases like this, where copper pours and ground planes are in play.

If anyone’s curious, you can check it out here: capext.com

I don't think the article's audience are professional EEs/PCB designers otherwise they'd know all of this stuff and then some. So anyone serious should probably seek out a better reference.

That's a reasonable take, but in my opinion, is not what a non-expert reading of this article seems to be suggesting. So I wanted to state the alternative case.

I have some experience that tells me that not all professional PCB designers know this stuff...

Great article!

> To keep things simple, some hobbyists opt for four-layer boards, with the two inner layers dedicated to GND and Vdd. This works, but means paying about twice as much.

With the prices out of Shenzhen, there is IMO no reason to use a 2-layer board, outside of trivial cases (Like a CAN terminator etc). 4-layers are a bit more expensive, but make routing much easier. I don't want to spend the time solving the routing puzzle on a two-layer board, then worrying about inductance (the article's topic) on top of that.

Baseline 2024 plan: Start with 4-layers as a generic baseline. Go to 6 (or higher?) if your design is sufficiently complex, and/or complex. (Or has high-frequency signals). More layers = more easier.

There is no reason to use 4-layers either. With 6 being so cheap, you can save time on routing and head scratching.

The simple explanation is that glue logic and wide busses have mostly disappeared from contemporary electronics. Now you have a smattering of peripherals with point to point links leaving board space for fills that would have been pointless attempting with pervasive Manhattan routing on the outer layers.

Solid fills also had a propensity to warp boards, requiring hatched patterns to relieve the imbalance. That constrained their use to boards with sufficient free space to maintain connectivity of the fill areas. PCB manufacturing has improved enough to minimize this concern.

> In electronic circuits, the flow of electrons is confined to conductors, but the transfer of energy doesn’t involve these particles bouncing off each other; instead, the process is mediated through electromagnetic fields. These fields originate from charge carriers, but extend freely into the surrounding space.

That's a great couple of sentences; it really clearly explains what's going on.

I don't see it mentioned here but I may be too much of an amateur but I use copper pours because it reduces the work my ferric chloride has to do when I'm making prototypes. Having a mask cover all unused areas on the board vs. letting the acid eat through it seems like a waste.

Your logic is definitely sound for a hobbyist or prototyped, but the copper dissolved off a board in a commercial setting is recycled.

The article misses the real reason why pours were uncommon in the 80s, which is that people had to actually “tape out” the whole thing, and it was very annoying to do pours that way.

Lots of manufacturers will add copper pours to your board unless you explicitly tell them not to, for electroplating reasons. Here's a link to a JLCPCB post about it: https://jlcpcb.com/blog/the-importance-of-copper-pour-in-emp...

JLC never added the pour for me. Not even for larger boards. Not sure this is up to date.

In any case, if you have to add the top layer pour, make sure to:

1. Use high clearence so as not to introduce edge coupling that changes your carefully calculated trace impedance.

2. Stitch the pour to actual GND with vias. Thoroughly. Do not let it float.

You do calculate trace impedance, right? :-)

I am only half joking. Some components let you specify source impedance. RP2040 has GPIO drive strength in mA, but they roughly correspond to 12 mA / 33 Ohm, 8mA / 50 Ohm, 4 mA / 70 Ohm and 2 mA / 100 Ohm. I usually use 100 for 2 layer boards and 70 for 4 layer boards. This is effectively series termination.

> JLC never added the pour for me. Not even for larger boards. Not sure this is up to date.

It seems to depend on the design - how close you are to the design limits and how much copper is exposed on the outer layers.

A message someone got from JLC for an open source project recently:

> When the copper pour is less than 30% of board area, we suggest to keep at least 0.15mm trace spacing.

> Or the dry film debris might have chance make short circuit, it will make quality control more difficult

That article says that they only add copper in the handling/bridging parts of the panel, not to the actual finished PCB.

Same goes for milling a pcb!

One reason for copper pours in a DIY hobby context is that copper pours vastly reduce how much copper has to be etched away. This requires less chemical like ferric chloride and less time.

You are making a capacitor, though, when you do that.

Surely the capacitor effect isn't that significant if you add in a bunch of stitching vias though, right?

This article is a bit superficial on EMC compliance, but they get one thing right, and that’s this:

Adding a solid ground plane to your board is one of the single best choices you can make in your PCB design.

It really depends on the design.

Say more.

I don’t really agree with you, but I’d like to know more about why you hold this view.

Ok I'm gonna ask a potentially stupid question as someone who knows little to nothing about electronics. The article (and every other source I looked at when trying to answer my question) points out the blank spots on the board as a copper pour. Where, exactly, is the copper? I just see green plastic. Is it on the back side and nobody is taking photos of it?

A PCB is a layer cake of fiberglass and copper, with the green stuff just being paint on top to make manufacturing easier. The copper is glued to the fiberglass and etched according to your design files. (This turns a plate of copper into a bunch of very thin wires, basically.) If it's a multi-layer design, a bunch of these etched boards are glued together. Holes are then drilled for vias (which are rivet like things that electrically connect arbitrary layers according to your design file) and through holes (for through-hole components, or for screws to attach a board to an enclosure, etc). Finally, a solder mask (the green stuff) is applied over the parts of the copper that don't need to be exposed (for connecting components), covering the copper on the outside layers.

The solder mask prevents solder from sticking to parts of the board that don't need solder on them.

To add components, solder paste (little balls of metal embedded in a flux) is applied to the areas without solder mask (using a metal plate that is laser cut to have holes where solder is needed), and then an optical/robotic system called a pick and place machine places each component at the right spot. (Or you can do this with tweezers.) Finally, the board is heated to the melting point of the solder, and because of the solder mask, pulls all the components into the exactly right place (by minimizing surface tension, something liquids like to do). Through hole boards are a little different, they get "wave soldered" where the board floats on molten solder and attaches to the metal areas. The solder mask is even more helpful here. If you didn't have solder mask, you'd just get a thick layer of solder on top of every trace, and potentially bridges between adjacent traces, which is bad. (But people do apply solder to exposed traces to increase their current carrying capacity.)

TLDR, the plastic on top is paint that makes manufacturing easier. If you make PCBs in your own shop with a laser or mini CNC, you won't have solder mask, and you can see how much more difficult soldering components is. It's not impossible. Just a little bit more work from your hand and brain is required, and that's expensive at scale. So, plasticy paint.

Thank you for the explanation! I had no idea about any of this, I figured that circuit boards were just plastic with metal traces etched in somehow. I didn't know that so much went into them.

Every time I order these things I am astounded at how cheap they are for what you get.

Sometimes volume really is magic!

This is a great explanation for the uninitiated. Kudos. You can get the green stuff in any color, of course. Hence red or blue circuit boards. There is lore about why green but whether it was chosen deliberately, copper traces appear darker through green than other colors because they're reddish. So one might prefer green for development.

The natural color of the most common fiberglass used in circuit boards is a straw color - you will see this from time to time, either on very low cost boards or where solder mask has been deliberately left off.

Vias were literally rivets in the very early days of PCB fabrication. Someone might still be selling a kit of that kind of thing for people who etch boards themselves. I'm not going to look, but they were still around 20 years ago, they were obsolete then, and things hang around in this industry for a long time after they're obsolete. Actual through-rivets have very poor mechanical performance and crack easily. Vias and through-holes for parts leads are typically plated now. You can only get plated through holes from the quick-turn suppliers hobbyists use, and that's a good thing.

stupid answer: copper goes green when it oxidises

actual answer: PCBs are covered in a protective film to prevent damage to the extremely thin layer of copper on them from bumps

The green is solder mask. It's just a coating that goes over most of the board, to prevent oxidation and accidental electrical shorts and to prevent solder from sticking where it isn't supposed to at the assembly stage. (You can get solder mask in different colors as well. The board itself is usually actually a sort of yellowish white and made of FR4, a kind of fire-resistant fiberglass.)

Generally you can sort of see through the soldermask to see the copper traces underneath. In the example images in the article, the lighter areas are copper and the darker areas are the space in-between.

> to prevent ... accidental electrical shorts

It frequently does that, so you are not wrong, but it is not a reliable insulator. If you need insulation or spacing for engineering or compliance reasons, you cannot rely on solder mask to provide it.

I mean the kind of shorts where you accidentally drop a screw on the PCB, drag a loose wire across it, or something like that. Not foolproof, but it probably reduces the risk of damage somewhat.

Right, and I think your language was careful to imply that, but others reading this should understand solder mask does that but it's not what it's for, if that makes sense. The bit of mechanical and environmental protection it can provide after assembly is similarly incidental.

There are a few other benefit to copper fills as well - it makes routing power much easier, it separates analog and digital regions of a PCB, and it helps with heat dissipation.

I do agree that just because you have a fill, that doesn't mean it is necessarily doing much help. You need to be careful that it isn't too broken up.

All I know is that it makes it very hard to solder anything to ground with my cheap underpowered soldering iron

Can be improved with proper thermal reliefs!

Can be improved by purchasing a decent soldering iron, which seems like a reasonable step to take if you need to solder something more than once or twice.

I switched away from full solid copper floods due to this. (Even with nice soldering equipment.) I still use full size floods but they are more like basket-weave patterns, probably 50% copper. I rotate the pattern on my second inner plane.

Four layer boards are so cheap now, it's all I choose. I usually do two internal ground planes and route my power on one side unbroken. I haven't made an interrupted return path since watching Rick Hartley videos.

Without a ground pour, isn't each trace basically an antenna?

Well not if there's a ground plane beneath, with 4 layers you can have signal traces on the outer layers and make the inner layers ground and every trace will have a good ground reference.

With a 2 layer board though, one layer's "copper pour" is the other layer's "ground plane"... Yet the article seems to advocate that you shouldn't use copper pours for 2 layer boards either? That's weird.

You want a ground opposite of the signal, next to it doesn’t count.

When you understand that the electrical field of your signal is in the fiberglass not in the copper, you’ll understand why.

@dang title is wrong ground planes not plates

Fixed. Thanks!

[flagged]

This is blogging for the sake of blogging. "A closer look at a fashion trend in printed circuit board design" reads like its going to be a history lesson in PCB aesthetics that quickly veers off into the weeds with copper pours that the author confuses with ground planes. There's no fashion or history here. Just another mostly useless article to pad out their blogger merit badge.

If you want to write a genuinely useful technical article then have someone in the relative field read it and give feedback. Otherwise you are wasting peoples time or worse, misleading them and causing harm.