[splaz]

I've noticed on an RJ45/8P8C socket that the tracks are arranged as capacitors on some of the pins. Layout would be roughly like if you spread your fingers on each hand apart and brought them together without touching.

I've also seen on circuit boards of some devices I/O lines have a section of trace zig zags like a resistor.

So I guess I'm curious why this is done? Is it a high frequency thing?

 

[tangent]

like if you spread your fingers on each hand apart and brought them together without touching 

 
What's the alternative? If you put a bunch of pins close together, the traces to them are necessarily going to have to get close to each other near the connector, and thus create a parasitic capacitance.
 
You could fix it by putting the pins farther apart, but then you're making connectors bigger than necessary.
 

 some devices I/O lines have a section of trace zig zags like a resistor.

 
It is almost certainly not a resistor.
 
Instead, the PCB designer has used that trick to make that trace longer, so that it is as long as a complementary trace that happened to need a longer path from its source to the connector. You see it in high-speed digital designs a lot because if you have a pair of related signals — most commonly, a differential pair — and the signal arrives earlier on one of them, you effectively have data corruption.
 
High speed digital folk like to say that the speed of light in copper is 1 foot per nanosecond. The inverse of 1 ns is 1 GHz, so if you're dealing with gigabit Ethernet, it can well make a difference if one trace of a pair is an inch shorter than the other.
 
(Grace Hopper, an early digital computer pioneer, is famous also for handing out "nanoseconds", being ~1 foot long chunks of copper wire.)

 

[splaz]

   
What's the alternative? If you put a bunch of pins close together, the traces to them are necessarily going to have to get close to each other near the connector, and thus create a parasitic capacitance.
 
You could fix it by putting the pins farther apart, but then you're making connectors bigger than necessary.
 

 
Sorry, I think I didn't explain this one clearly enough originally, the pins had what looked like a little capacitor made up of tracks on the board connected to them, like this:
   
|   -----------------|
|-----------------   |
|   -----------------|
|-----------------   |
|   -----------------|
|-----------------   |
|   -----------------|
|-----------------   |
 
 
 
The pin in question was connected to one side, the opposite side was connected to a via either going to the groundplane or other side of the board, which I couldn't easily check at the time.
 
Is this just a really tiny value capacitor or is there some other purpose ?
 

It is almost certainly not a resistor.
 
Instead, the PCB designer has used that trick to make that trace longer, so that it is as long as a complementary trace that happened to need a longer path from its source to the connector. You see it in high-speed digital designs a lot because if you have a pair of related signals — most commonly, a differential pair — and the signal arrives earlier on one of them, you effectively have data corruption.
 
High speed digital folk like to say that the speed of light in copper is 1 foot per nanosecond. The inverse of 1 ns is 1 GHz, so if you're dealing with gigabit Ethernet, it can well make a difference if one trace of a pair is an inch shorter than the other.
 
(Grace Hopper, an early digital computer pioneer, is famous also for handing out "nanoseconds", being ~1 foot long chunks of copper wire.)

 
Ahhh...  okay, that does make more sense than my inital thoughts.
 
Thanks as always tangent.

 

[tangent]

It looks like an intentionally designed capacitor to me. It's a way to get a free component. I doubt it's good for more than dozens of pF, but sometimes that's all you need to tune a circuit.

 

[tangent]

A few more thoughts on that:
 
An equivalent ceramic capacitor might cost only a few cents, whereas that PCB cap probably cost more than a few cents in PCB space. It can still be a net win.
 
First, the cost of the actual component isn't the only cost added to that of the final product. Every additional different component adds several costs to the manufacturing process. It's another part you have to order/qualify/stock, it increases your company's risk to obsolescence, it requires another reel on the pick-n-place machine... A board made with 50 distinct parts will cost less to manufacture than one that takes 100 parts, even if the BOM cost is identical.
 
Second, it may well be that FR4 and copper make a better quality capacitor than a 2 cent ceramic. I suspect this is true, since plastics tend to make more linear dielectrics than ceramics, and glass-epoxy is a plastic if you squint.
 
Third, doing it on one layer of the board like that allows higher capacitance per unit area than the more common case, where you're looking at solid plates on different layers, since capacitance is a function of plate spacing. (So is voltage, but with the low voltages used in most digital design, you're limited more by your board house's trace/space limits than voltage tolerance.)
 
Finally, I found an EE.SE question about this.

 

[splaz]

  A few more thoughts on that:
 
An equivalent ceramic capacitor might cost only a few cents, whereas that PCB cap probably cost more than a few cents in PCB space. It can still be a net win.
 
First, the cost of the actual component isn't the only cost added to that of the final product. Every additional different component adds several costs to the manufacturing process. It's another part you have to order/qualify/stock, it increases your company's risk to obsolescence, it requires another reel on the pick-n-place machine... A board made with 50 distinct parts will cost less to manufacture than one that takes 100 parts, even if the BOM cost is identical.
 
Second, it may well be that FR4 and copper make a better quality capacitor than a 2 cent ceramic. I suspect this is true, since plastics tend to make more linear dielectrics than ceramics, and glass-epoxy is a plastic if you squint.
 
Third, doing it on one layer of the board like that allows higher capacitance per unit area than the more common case, where you're looking at solid plates on different layers, since capacitance is a function of plate spacing. (So is voltage, but with the low voltages used in most digital design, you're limited more by your board house's trace/space limits than voltage tolerance.)
 
Finally, I found an EE.SE question about this.

 
 
Wow, thanks for the extra info.
 
I think you'd be very much on the money, in a nut shell the board was just a very basic conversion of one type of terminal to another connector for data, there is only 2 actual parts to it with both being through hole connectors, I'd imagine fiddling with a surface mount or even a small through hole ceramic capacitor would cost drastically more to assemble when board space is not at a huge premium and I wouldn't be surprised if they fit within the confines of the space physically needed for the board in the first place.
 
I'd also imagine doing it on the board is actually a bit more mechanically robust and reliable in a way.
 
So probably the best design choice all round, but I was very curious as not something I've personally seen before.
 
Thanks again, above and beyond tangent, you're a fountain of knowledge.

 

[wakibaki]

It's quite common to use components fabricated on (FR4) PCBs, but they don't really come into their own until you get to microwave frequencies >1GHZ (because the values achievable are comparatively small), and usually with a limit of ~2.5GHz, because FR4 doesn't have reliable enough characteristics for use higher than this, the dielectric constant and loss tangent then varying as a function of frequency based on the Kronig-Kramers relations, IIRC. 2.4GHz equipment is pretty much the highest frequency stuff built on FR4. PTFE starts to take over, and other exotic materials. Sapphire is used as a substrate for some MMICs.
 
Both inductors and capacitors can be fabricated, of course these are pretty much in the pico- and nano- ranges. Inductors can sometimes be seen in the form of spirals (or 'square spirals'), caps are formed as interdigitated 'fingers'. At higher frequencies transmission line 'stubs' are employed, an open circuit parallel stub will act as a capacitor, a shorted (to ground) parallel stub will act as an inductor. Microwave filters are a common application making use of such technologies. Stubs are often used as resonant circuits in distributed element filters, these will commonly look like a series of staggered unconnected parallel strips of trace.
 
w
 
Dielectric resonators can sometimes be seen, they will typically be a small cylinder (puck) of dielectric material, often ceramic, although more latterally plastic, offset by a small distance from a passing trace. These can exhibit an unloaded Q in the 10s of thousands.

 

[jcx]

1 ns/ ft is about the speed of light in a vacuum, wave propagtion on pcb, guided by the trace is ~ 50% of that http://www.hottconsultants.com/techtips/rulesofthumb.html
 
and electron drift velocity at our mA currents, visible trace size is less than a slow stroll:
http://books.google.com/books?id=mMJxcWqm_1oC&pg=PA304&lpg=PA304&dq=pcb+trace+electron+drift+velocity&source=bl&ots=71uqNZCocm&sig=h4Xl8y0x1U2VmNxl3YGPnA_Dy4A&hl=en&sa=X&ei=aUszUu24Dsj64APb0oDYCw&ved=0CDsQ6AEwAg#v=onepage&q=pcb%20trace%20electron%20drift%20velocity&f=false

 

[fakir]

@splaz, it’s actually a type of filter, a smartly designed filter. In my opinion, since the long track widths have their own inherent resistance and there will be some capacitance which effectively are the components of a filter. There’re many research papers on such filters and designers these days just copy the designs from these research papers with some modifications. The advantage of such filters is that the designers don’t have to rely on components which increases the durability of the overall design.
 
circuit board assembly