5 ms·

PCBs, copper pours, ground planes, and you

284 points by surprisetalk 2y ago

yujzgzc 2y ago
All I know is that it makes it very hard to solder anything to ground with my cheap underpowered soldering iron
- deleted 2y ago
  [deleted]
- pjc50 2y ago
  Can be improved with proper thermal reliefs!
  - buildsjets 2y ago
    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.
- mikeInAlaska 2y ago
  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.
fargle 2y ago
@dang title is wrong ground planes not plates
- dang 2y ago
  Fixed. Thanks!
mmcwilliams 2y ago
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.
- nickff 2y ago
  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.
  - murderfs 2y ago
    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-empty-areas https://jlcpcb.com/blog/the-importance-of-copper-pour-in-emp...
    - mordae 2y ago
      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.
      - bogantech 2y ago
        > 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
exmadscientist 2y ago
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-using-ground-pours/msg2841186/#msg2841186 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.
kazinator 2y ago
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.
- mort96 2y ago
  Surely the capacitor effect isn't that significant if you add in a bunch of stitching vias though, right?
michaelt 2y ago
> 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.
- aylons 2y ago
  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.
  - iancmceachern 2y ago
    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.
cushychicken 2y ago
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.
- hulitu 2y ago
  It really depends on the design.
  - cushychicken 2y ago
    Say more. I don’t really agree with you, but I’d like to know more about why you hold this view.
roland35 2y ago
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.
MisterTea 2y ago
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.
pcdoodle 2y ago
Without a ground pour, isn't each trace basically an antenna?
- mort96 2y ago
  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.
- SV_BubbleTime 2y ago
  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.
tverbeure 2y ago
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-board-stack-up-rick-hartley https://resources.altium.com/p/the-extreme-importance-of-pc-...
- cushychicken 2y ago
  Hartley is awesome. Plus one for that.
mikeInAlaska 2y ago
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.
the__alchemist 2y ago
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.
- varispeed 2y ago
  There is no reason to use 4-layers either. With 6 being so cheap, you can save time on routing and head scratching.
bigstrat2003 2y ago
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?
- lexicality 2y ago
  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
- jrockway 2y ago
  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.
kevin_thibedeau 2y ago
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.
- deleted 2y ago
  [deleted]
dtgriscom 2y ago
> 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.
hex4def6 2y ago
> 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.
- avsteele 2y ago
  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.
  - ChadNauseam 2y ago
    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/proximity-effect https://www.sciencedirect.com/topics/computer-science/proxim...
    - londons_explore 2y ago
      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.
pourmeahotone 2y ago
[flagged]

284 points by surprisetalk 2y ago

yujzgzc 2y ago

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

deleted 2y ago
[deleted]
pjc50 2y ago
Can be improved with proper thermal reliefs!
- buildsjets 2y ago
  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.
mikeInAlaska 2y ago
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.

fargle 2y ago

@dang title is wrong ground planes not plates

dang 2y ago
Fixed. Thanks!

mmcwilliams 2y ago

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.

nickff 2y ago
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.
- murderfs 2y ago
  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-empty-areas https://jlcpcb.com/blog/the-importance-of-copper-pour-in-emp...
  - mordae 2y ago
    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.
    - bogantech 2y ago
      > 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

exmadscientist 2y ago

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-using-ground-pours/msg2841186/#msg2841186 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.

kazinator 2y ago

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.

mort96 2y ago
Surely the capacitor effect isn't that significant if you add in a bunch of stitching vias though, right?

michaelt 2y ago

> 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.

aylons 2y ago
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.
- iancmceachern 2y ago
  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.

cushychicken 2y ago

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.

hulitu 2y ago
It really depends on the design.
- cushychicken 2y ago
  Say more. I don’t really agree with you, but I’d like to know more about why you hold this view.

roland35 2y ago

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.

MisterTea 2y ago

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.

pcdoodle 2y ago

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

mort96 2y ago
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.
SV_BubbleTime 2y ago
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.

tverbeure 2y ago

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-board-stack-up-rick-hartley https://resources.altium.com/p/the-extreme-importance-of-pc-...

cushychicken 2y ago
Hartley is awesome. Plus one for that.

mikeInAlaska 2y ago

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.

the__alchemist 2y ago

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.

varispeed 2y ago
There is no reason to use 4-layers either. With 6 being so cheap, you can save time on routing and head scratching.

bigstrat2003 2y ago

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?

lexicality 2y ago
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
jrockway 2y ago
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.

kevin_thibedeau 2y ago

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.

deleted 2y ago
[deleted]

dtgriscom 2y ago

> 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.

hex4def6 2y ago

> 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.

avsteele 2y ago
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.
- ChadNauseam 2y ago
  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/proximity-effect https://www.sciencedirect.com/topics/computer-science/proxim...
  - londons_explore 2y ago
    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.

pourmeahotone 2y ago

[flagged]