Question about PCB Trace widths & Grounding 2 PCB's together???

[Jasonmatthew911]

Hi guys, I've been designing my own PCB's since last year...I'm making a new design right now and I decided to go with wider traces this time because I have the space, but I want to make sure I'm not going too wide, as I really don't know all the rules to proper PCB design...I always figured that Wide traces/more copper is better, but I also read that wider traces means you also need more space between traces, but I have plenty of space between traces, so I'm not worried about my spacing...Anyhow, in my new project I had a lot of room on my boards for wide traces (This project involves 2 PCB's that will be stacked on each other with spacers in the same box), my signal traces are 60mil wide, and my +V Power traces are 80mil wide, and all my GND's are connected directly to GND planes that connect on both sides of PCB, as I'm doing 2-sided PCB printing...Are these trace widths good as long as I have the space for them?...Also, This is 2 questions in 1, my other question is how to properly GND the 2 PCB's together to avoid GND Loops?...Should the 2 boards be Grounded together at as many points as possible, or should there just be 1 GND path between the 2 PCB's?...Both Boards have GND Planes on both sides, the bottom GND planes almost have no traces, only a couple small ones, most my traces are on the top side, where I've eliminated any part of the GND plane that gets cutoff from the rest of the GND plane, both GND planes are connected together through many Grounded components all over the boards...Hopefully there're some PCB experts here that can help me understand better about trace widths and the proper way to GND 2 PCB's together...I had planned to GND the 2 PCB's together by using small shielded cables that will carry signals that have to go from 1 PCB to the other, and the shield would connect the GND planes of both boards together...So there're 5 connections/signals that need to go between my PCB1 and PCB2, I was just gonna connect those 5 connections at different points of the boards with the short shielded cables for Grounding the 2 PCB's together...So I was wondering if doing the shielded cables at many points was better or not a good idea?

[Kevin Mitchell]

A few things.

You're over thinking
You're over compensating
You're just... overdoing everything

In this case it may be best to share your layouts so the experienced folks can pick at it. While in theory what you're doing will work fine, there's much that you don't need to be doing for a good end result.

-KM

[bartimaeus]

i totally agree with KM

you only want one ground path between the two pcbs.

you really only want a ground plane on one side of the pcb, and it should be as solid as possible. having partial planes on the top layer just increases the risk of stray capacitance. all components with a ground connection should drop directly to ground, and if you're using smd then use separate vias for each one.

shielded cables are overkill, especially if this is going inside an aluminum enclosure that's already shielding the circuit.

in pedal building, i've never had a reason to go above 25 mils. even that is overkill unless you're drawing more than 1.5A, which is quite a lot for a pedal (think about how many 5mA fuzz pedals you could power off that trace). if you're getting the pcb made cheap, a thicker trace will be harder to lift accidentally, but that's still no reason to go above 25 mils. additionally, smaller traces are good because they can be spaced out more to reduce crosstalk and stray capacitance.


https://electronics.stackexchange.com/questions/5403/standard-pcb-trace-widths

[DrAlx]

i've never had a reason to go above 25 mils. even that is overkill unless you're drawing more than 1.5A

Looking at the graph, 1.5 amps at 20 degrees celsius is 25 ***square*** mil.
So a 25 mil track width would need to be at least 1 mil thick.  That is a seriously thick PCB track.  Tracks are typically fractions of a mil thick so one should account for that when using the graph.

EDIT: Ignore the above. I confused mil with mm. A track is typically more than 1mil thick.

[Jasonmatthew911]

i totally agree with KM

you only want one ground path between the two pcbs.

you really only want a ground plane on one side of the pcb, and it should be as solid as possible. having partial planes on the top layer just increases the risk of stray capacitance. all components with a ground connection should drop directly to ground, and if you're using smd then use separate vias for each one.

shielded cables are overkill, especially if this is going inside an aluminum enclosure that's already shielding the circuit.

in pedal building, i've never had a reason to go above 25 mils. even that is overkill unless you're drawing more than 1.5A, which is quite a lot for a pedal (think about how many 5mA fuzz pedals you could power off that trace). if you're getting the pcb made cheap, a thicker trace will be harder to lift accidentally, but that's still no reason to go above 25 mils. additionally, smaller traces are good because they can be spaced out more to reduce crosstalk and stray capacitance.


https://electronics.stackexchange.com/questions/5403/standard-pcb-trace-widths

Ok thanks...I'll lessen my PCB widths a bit...I've done a few good boards with 48mil traces, maybe I'll stick to that or lower since I do have a lot of spacing between my traces...I guess it's a mental thing that the thicker traces make me feel more secure about all the connections haha...The board design is for 18V 1A...

Do you think that I should connect the 2 PCB's to each other or connect the GND planes of both PCB's at the Power input jack instead?...So either a GND wire between PCB's then another wire going to supply GND from the main PCB, or 2 wires from each PCB's GND Plane connecting directly to the Power jack GND?...Which option would be less problematic with GND loops?

[bartimaeus]

i totally see where you're coming from mentally, when i started i had the same mindset (and i was afraid of vias too). but when you start looking at bga stuff where there's hundreds of vias and 2 mil traces and it still works fine, you realize that even 25 mils is total overkill for guitar signal trace. 48mils is twice what you'll need for a 1A circuit, and even then you only need the thicker trace for power. for signals you can go much smaller. remember, the more copper you have on the top layer, the more of a capacitor it forms with the bottom layer ground plane (in a 2 layer board, anyway).

maybe ground them together at one point near where power connects to the boards? but to be honest, you may just want to try both and see which works better for your setup (if you notice any difference), since all it takes is moving a couple wires.

[Jasonmatthew911]

i totally see where you're coming from mentally, when i started i had the same mindset (and i was afraid of vias too). but when you start looking at bga stuff where there's hundreds of vias and 2 mil traces and it still works fine, you realize that even 25 mils is total overkill for guitar signal trace. 48mils is twice what you'll need for a 1A circuit, and even then you only need the thicker trace for power. for signals you can go much smaller. remember, the more copper you have on the top layer, the more of a capacitor it forms with the bottom layer ground plane (in a 2 layer board, anyway).

maybe ground them together at one point near where power connects to the boards? but to be honest, you may just want to try both and see which works better for your setup (if you notice any difference), since all it takes is moving a couple wires.

Hey, thanks for all your input...I tend to question everything, and I've had mixed advice on the GND plane subject...I have read about one full GND plane on bottom layer being best, but I'm just wondering why I've seen so many professional made PCB's that actually have the GND plane on the Top layer as well...Also an old Tech that also gives me advice said that it was better to surround the circuit with GND on Top and Bottom if I could, because basically through the components that connect directly to GND you are connecting the Bottom GND Plane to the Top GND plane all over the Board through the Via's, since the GND doesn't travel through actual traces, the Top GND plane basically becomes part of the bottom GND plane since they connect directly to each other, making it a bigger GND plane and surrounding the circuit with GND for extra shielding...That makes sense to me, as long as you don't have the GND's connecting with traces and a bunch of wires, otherwise, why do so many professional made PCB's have Copper planes all over the Top and Bottom of 2 layer Boards?...Does it make any sense, or am I wrong, as well as the tech that told me to make GND planes on Top and Bottom?...He does good repair jobs, he's Cuban and is especially good with old Tube amps, but I know it doesn't mean he knows all the right and wrongs about making proper PCB's, though he does see a lot and repairs a lot of PCB's...He probably sees how most Boards come full of Copper planes on Top and Bottoms as well, even if the Top Planes are cut up a bit, any copper that gets cut off from the rest of the GND plane due to traces usually gets eliminated...Let me know your further thoughts on this if you can, thanks. 

[R.G.]

PCB traces need to be wide enough to carry the signal current without (a) overheating the trace and (b) having trace width and it's side effects change the signal.

For pedals, the currents are too small to worry about traces wider than about 25-30 mils. There are some issues with very narrow traces - maybe 10 mils and narrower. These narrower traces are more fragile, and so they are prone to crack where they run into a pad. I have used traces 200 mils wide for high current situations, although in general if I need over 100mils, I'll generally use a fill or pour. That's for traces that carry 20 amps and up. Ideally, you wouldn't do that in a pedal.

As to trace width affecting the the signal, very narrow traces tend to be routed to places that are very narrow. This can cause capacitive coupling problems. Not usually a problem with audio frequencies, but with digital edges it's worse. And ground planes/pours can affect things, as noted below.

By now you clever and insightful readers will have figured out that trace width and spacing makes a difference depending on what the nature of the signal running through the trace might be. The real answer to trace width is to know the nature of the signal in the trace - how much current is there, and what the source impedance is on the driving end of the trace, and the receiving impedance on the driven end. The traces to really worry about are the ones that go to high impedance inputs - FET gates and Darlington or bootstrapped bipolar inputs, opamp inputs and such. Mostly these have nearly zero currents, but are high impedance and collect crosstalk easily. They can be any width you like, but they ought to be spaced away from other traces that carry big, fast-changing signals, like especially switching edges.

For trace widths in most pedals (that is, low enough currents to not worry about heating) use 20-30 mils, or even bigger if you're feeling frisky, but think about what traces and signal are next to the trace you're routing. For spacing, the rule is to move anything you can as wide apart as practical to avoid crosstalk. If you have lots of room, use it.

PCB makers talk about trace and space rules. You'll see thing like 10/10, 8 and 8, and so on. These numbers are the minimum recommended trace width and trace spacing that their manufacturing process can handle reliably. They tend to be the same two numbers, as the photographic processes are about as good for trace width as for spacing. That doesn't mean you have to use those narrow traces and spaces, just that if you don't go below that, they can make the board. In the bad old days in the 1970s, you had to pay handsomely to get under 15 mils, but today, you can get 4 mil traces if you want. Again, unless you have some special needs (and can write these down coherently     ) use 20-30 mil traces and space them generally about that far apart or more where you can.

As to pours and planes: this is closely related to grounding in most cases, and that's another kettle of fish-worms. Sure it looks fancy to have that nice plane on both sides, but it may serve little purpose than looking good. There isn't any substitute for knowing what the nature of the signals are, which is one reason that autorouting is >still< not great for analog boards.

At low frequencies (that is, audio) signals follow the path of lowest resistance, no matter how convoluted that path may be. At higher frequencies, field effects take over from resistance, and signals flow where the fields tell them to. In this case, a plane serves as the other side of a transmission line carrying the signal. The signals flow from the source to the sink, and the return is through the conductors most closely capacitively available. For RF signals, you need either a true transmission line (matching traces top and bottom sides) or stripline - a signal trace over a broad ground plane. There is a gradual changeover from resistance being the big decider to needing planes to carry the RF components.

There is another aspect of ground planes - they allow lazy layouts. A general rule for audio layout is to concentrate on signals other than power and ground first, and connect up power and ground last. There are reasons for that, but then I'd need to re-type the book if I went much deeper. Given that ground should be considered first but actually routed last, if you plan to use a ground pour/plane, you can simply put a via wherever you need a ground on a component, and a plane will make that magically come true at the end. Lazy layout work.

Questions? Have I just muddied the issues up?

[bartimaeus]

when using a split up ground plane on the top layer, you'll want to be careful how you connect to it, and also how you connect each segment to the bottom layer ground plane. one option is stitching vias, which you mention. that's what you see more often see on professional pcbs, but you also need to be careful about via spacing. you should really find resources that go in depth on how its done, because if this is digital or mixed then it's too easy to mess it up by implementing the top ground plane poorly. none of this matters too much if it's an analog design though.

so it's a lot easier to just use a bottom ground plane, with vias at each smt component to connect it directly to the bottom layer. sure, that extra shielding would be nice in theory, but if this is a pedal then you're already putting the pcb in a grounded metal enclosure that does all the shielding you need anyway.

one other thing you see on professional pcbs is thieving, where you have a bunch of sections of disconnected copper on a layer. it might look like a hatched ground plane, but it's just a technique to improve the manufacturing process.

[R.G.]

Yes, there are situations where using ground planes willy-nilly is not a great idea. The big one is in mixed signal designs where you really ought to consider analog ground and digital ground as two separate signals and connect them very, very carefully to make sure they're at the same voltage potential.

And that gets us into the issues of grounding. Grounding well simply requires that you know what currents are flowing through the "ground". There are no zero ohm grounding wires available to us in PCBs. We must deal with the fact that any ground wire has resistance, and so it generates a voltage proportional to the current flowing through it. Every "ground" point has a voltage imprint of the currents flowing past it. If you want quiet circuits, you have to take this into account.

The only way to have two points forced to the same voltage is to either have the connection between them have zero resistance or have zero current flowing in that wire. So practical grounds will always have some tiny voltage differences. For RF, the currents will follow the most direct route to minimize the area of the current loop; for audio, you can force the currents to flow where you want them by running separate ground traces. These traces still have offset voltages proportional to the currents flowing in them, but by using separated ground traces, you can force the ground offsets to have voltages proportional to only a single stage, not the conglomerate of al the other stages that pass by. In the limit, this becomes star grounding.

Ground pours work mostly in audio work because they offer the lowest resistance path you can get on that PCB layer. But some critical stages with high impedance nodes are better served (i.e. quieter) by specified ground paths. This is mostly a non-issue for most pedals, but sometimes you get zapped by these subtleties.

[Jasonmatthew911]

Yes, there are situations where using ground planes willy-nilly is not a great idea. The big one is in mixed signal designs where you really ought to consider analog ground and digital ground as two separate signals and connect them very, very carefully to make sure they're at the same voltage potential.

And that gets us into the issues of grounding. Grounding well simply requires that you know what currents are flowing through the "ground". There are no zero ohm grounding wires available to us in PCBs. We must deal with the fact that any ground wire has resistance, and so it generates a voltage proportional to the current flowing through it. Every "ground" point has a voltage imprint of the currents flowing past it. If you want quiet circuits, you have to take this into account.

The only way to have two points forced to the same voltage is to either have the connection between them have zero resistance or have zero current flowing in that wire. So practical grounds will always have some tiny voltage differences. For RF, the currents will follow the most direct route to minimize the area of the current loop; for audio, you can force the currents to flow where you want them by running separate ground traces. These traces still have offset voltages proportional to the currents flowing in them, but by using separated ground traces, you can force the ground offsets to have voltages proportional to only a single stage, not the conglomerate of al the other stages that pass by. In the limit, this becomes star grounding.

Ground pours work mostly in audio work because they offer the lowest resistance path you can get on that PCB layer. But some critical stages with high impedance nodes are better served (i.e. quieter) by specified ground paths. This is mostly a non-issue for most pedals, but sometimes you get zapped by these subtleties.

Awesome, thanks for all the input RG...So basically my design and both PCB's are all Analog, and it will be going into a stainless steel enclosure, but it's not exactly a pedal, it will operate on 9V - 18V like a pedal though, it's a 2 input line mixer that will have (2) TL072 Pre-Amps, one going into an analog CabSim which can be turned on/off via 3pdt switch, both signals will go to a D.I. Jensen transformer with XLR output and to an unbalanced PreAmp out for connecting to Amps as well, additionally it will have a headphone amp for silent practice/jamming...So you can use this as a mini 2 instrument mixer for Guitar/Bass/Synth, and a splitter for recording or Live situations, to get a direct sound and mic'd amp sound simultaneously or one or the other...So basically 2 Pre-Amps, 1 CabSim, a headphone amp, and a DI Transformer all in one small consolet stainless steel enclosure...I managed to make the 2 PreAmps with headphone amp on 1 Board, and the small DI circuit with Analog CabSim is on the other board...

Knowing all of this, would you say I can still do the (2) GND planes on both sides of both PCB's knowing that all GND components are connected directly to both planes through their direct vias?...Lastly, where would you connect the GND planes of both PCB's together, either with a wire connecting them together and 1 PCB going to Power jack GND, or maybe connecting both PCB GND planes together at the Power Jack instead?...I can't decide if it would be better for the GND's of the 2 PCB's to connect together through a wire or a shielded cable that's connected to GND and then just 1 PCB going to the Power jack GND, or if both PCB's should be wired directly to Power jack GND?

[bartimaeus]

i assumed the two boards were more interdependent (for example one board with controls and one with components). if the boards have separate circuits that only connect at inputs/outputs, you're essentially daisy-chaining. connect each board at the power jack, and add separate bypass caps (and other filtering, if you use it) for each board.

[Jasonmatthew911]

i assumed the two boards were more interdependent (for example one board with controls and one with components). if the boards have separate circuits that only connect at inputs/outputs, you're essentially daisy-chaining. connect each board at the power jack, and add separate bypass caps (and other filtering, if you use it) for each board.

Cool, thats what I'll do, thanks, and yes each board has it's own bypass caps and reverse polarity protection, all the components that mount on top part of enclosure, which are 3 Pots, an LED and a 3PDT toggle switch are on the reverse side of the board with the 2 Pre-Amps and headphone amp, then the other board with CabSim circuit and DI stacks on to that board with spacers and screws, everything is analog, no digital in this design...Since there's no digital you think I'm good to do the GND planes on both sides of PCB's, or would you say better keep the GND planes only on bottom with least cuts as possible?

[PRR]

> you think I'm good to do the GND planes on both sides of PCB's, or would you say better keep the GND planes only on bottom

[Jasonmatthew911]

Hahaha, I think I'm thinking too much...I always tend to overthink things when it comes to electronics, sorry.