11
\$\begingroup\$

I am designing the layout of a PCB for audio applications (no digital electronics, only analog).

All components are through hole, the PCB is pretty large (about 16cm x 10cm) and has 2 layers. Plated through hole are supported by the technology I am using. The circuit has a dual supply.

Which (and why) of the following is the best solution for routing signals, power supply tracks and ground?

  • TOP layer: ground plane; BOTTOM layer: signals and supply lines;
  • TOP layer: signals and power supply lines: BOTTOM layer: ground plane;
  • TOP layer: ground plane and supply lines; BOTTOM layer: signals;
  • TOP layer: signals; BOTTOM layer: ground plane and supply lines;
\$\endgroup\$
  • 2
    \$\begingroup\$ This question requires a kind of generalization that is likely to be either dependent on the design or totally irrelevant. The lowest-skill-required version is having an uninterrupted ground plane, so #1 sounds fine. Bypass as required and keep sensitive traces away from noisy signals. \$\endgroup\$ – Daniel Apr 26 '18 at 9:06
  • 1
    \$\begingroup\$ In general having ground around your signal lines rarely hurts. Whether this in done on bottom or top plane doesn't matter so I'd go with #3/4 \$\endgroup\$ – Humpawumpa Apr 26 '18 at 9:08
  • \$\begingroup\$ @Daniel Nominal frequencies involved in the circuit are below 5k, since the circuit is an analog effect for guitar signal processing. \$\endgroup\$ – Umberto D. Apr 26 '18 at 9:16
  • \$\begingroup\$ @Daniel ...And supply voltages are generated through a linear Power Supply, no switching PSU. \$\endgroup\$ – Umberto D. Apr 26 '18 at 9:24
3
\$\begingroup\$

I think all these other answers are over-complicating the issue. Through-hole designs are legitimate in many cases, and so are 2 layer boards.

I would recommend using a ground plane and a signal/power plane unless you have a reason not to. This design method is tried and true and I don't see any reason you shouldn't use it. I think it doesn't really matter which side you put the signals on.

You will need to make some jumpers in the ground plane, but this won't cause any problems if you avoid making large cuts. I made a quick and terrible image in paint to illustrate:

ground plane large cuts vs jumpers illustration

As Neil mentioned, your ground return paths do matter, you shouldn't just consider them finished when they enter the ground plane.

\$\endgroup\$
13
\$\begingroup\$

The one method I'd recommend is the one you haven't mentioned.

Generally, any arbitrary division of spaces into power, ground, signals, is going to give you some grief, because it's neither necessary to partition them like that, nor sufficient to get a good result.

If the board was 'difficult', so mixed analogue/digital, high speed signals, high currents, SMPS, then there would be benefit in starting with a full ground plane. But that's not sufficient, you need to know where the return currents are flowing in it, because you can still shoot yourself in the foot, even with a ground plane.

I would recommend Manhattan layout, with a gridded ground.

The great benefit of Manhattan is it means you can always find a route for your track. You never have to compromise and take a signal a meandering route away from its return path, or cut a ground plane to sneak a track through, destroying its integrity.

Manhattan routing involves dedicating one layer for North-South connections, and the other layer for East-West connections. Now you can always get from A to B with typically one via, and you never have to wonder about how you can cross a track.

Now you have a systemic way to route your board, start with a gridded ground. On one layer, put a track every 20mm or so, in columns. On the other layer, do the same in rows. Via them together at every intersection. Now you have a ground that is very nearly as good as a plane, and far more useable, because both layers are still available to route all your power and signals. Move the ground tracks around a bit to accomodate your ICs by all means, but don't move them too far apart.

Postscript - ground plane versus gridded ground.

I've had some interesting comments from Umberto, Scott, and Olin, which suggest I haven't quite got my point across. I'll perhaps clarify what's above, while documenting my reasoning below.

I'm now retired, and after a lifetime mentoring junior engineers, one of the biggest problems they face is doing a poor design on a ground plane board. They seem to think that the ground plane 'will take care of all that isolation stuff', and they stop thinking. As a result, they run high currents past sensitive inputs, and otherwise fail to spot the effects of return currents.

In order to help them debug these boards, I remove the ground plane, and force them to consider all return currents as discrete flows in separate tracks. Once the culprit has been found, and the layout fixed, the ground can be restored.

On a 4 layer board, there's enough space to dedicate one to a solid ground. On a 2 layer board, there is a premium on routing space. That's why Manhattan, which gives you a systematic way to route any track from A to B, is so useful. If you dedicate one of your 2 layers to ground, any non-trivial layout will result in one, or two (or several, hey, it's only one more) tracks cutting the ground apart, wrecking its integrity.

With no ground plane, a gridded ground is the next best thing. It's flexible, you can increase the number of ground tracks where you need to. It's totally compatible with Manhattan routing. When you've finished the layout, by all means flood with ground copper. You'll end up with something that's better routed than a chopped-up ground plane, because you've been able to think about all those return currents you might have otherwise hoped would be OK.

Good board design is almost as much an art as a science. You can't teach artists to create, you can't teach engineers to 'feel' where currents are going to flow, until they 'get' it. Designing without a ground plane is one way to speed up the 'getting it' process.

\$\endgroup\$
  • 3
    \$\begingroup\$ I'm not sure I see why this is as good as a plane. It really depends on what's sucking current where on your grid, and it feels like not enough care can result in a ground loop. \$\endgroup\$ – Scott Seidman Apr 26 '18 at 12:07
  • 1
    \$\begingroup\$ I can recommend Manhattan routing. For low speed design (<10Mhz), this is an quick method to get a board done. \$\endgroup\$ – Jeroen3 Apr 26 '18 at 12:17
  • 1
    \$\begingroup\$ @ScottSeidman read my answer very carefully, I say 'very nearly as good ...'. You're right, not enough care can result in all sorts of bad things, no matter which 'process' you're following. \$\endgroup\$ – Neil_UK Apr 26 '18 at 12:42
  • 1
    \$\begingroup\$ @ScottSeidman I have your same concern. \$\endgroup\$ – Umberto D. Apr 26 '18 at 13:50
  • 2
    \$\begingroup\$ I agree that a "good" gridded design can be effective, but I believe that a bad gridded design can be bad, and that it might be difficult for someone not attuned to ground design to know when the design starts getting bad. For example, screwing up with a high-current audio output driver can be pretty disastrous. Fairly, though, the same can happen with broken ground planes. \$\endgroup\$ – Scott Seidman Apr 26 '18 at 20:50
8
\$\begingroup\$

All components are through hole

For this reason alone I would consider using a ground plane on the bottom so that components can be mounted without worrying about whether their bodies might make contact with ground copper.

Given that it is for a guitar effects box with potentially a lot of vibration and movement due to foot controlled buttons and controls I would also consider how signals are routed under compenents too in order to avoid the problem mentioned in my first paragraph.

But, why limit your self to two layers - get the signal tracks off the top layer entirely and use a 4 layer board. Cost wouldn't be much more and peace of mind is a good thing.

\$\endgroup\$
  • 1
    \$\begingroup\$ 4-layer board are more expensive compared to 2-layer. Assuming a 2-layer PCB is used, I think that ground plane and voltage supply tracks on the top could be better. Since larger tracks and vias are used, I do not see so much to worry about contacting. In addition, solder flows easily through the via... What do you think? \$\endgroup\$ – Umberto D. Apr 26 '18 at 13:53
  • 1
    \$\begingroup\$ When you consider "environmental issues" and the number of potential failures due to poor design and the likely loss of customer faith and the rework/fixing cost, you have to convince yourself that straight-up "extra" PCB cost is the best reason to only use two layers. \$\endgroup\$ – Andy aka Apr 26 '18 at 13:56
  • \$\begingroup\$ I probably misunderstood your concern. You are worried about unwanted contacts of metal body of components. Correct? \$\endgroup\$ – Umberto D. Apr 26 '18 at 14:06
  • 1
    \$\begingroup\$ Yes I am and given the nature of the abuse that this sort of product receives at the feet of guitarists it makes sense to take precautions. \$\endgroup\$ – Andy aka Apr 26 '18 at 14:10
7
\$\begingroup\$

None of your proposed layouts are good. A better scheme than any you mention is to use SMD parts. This has a number of advantages:

  1. A much wider range of parts are available.

  2. The same parts will be cheaper.

  3. It will take much less hassle and time to solder the parts onto the board.

  4. It leaves you more flexibility for routing.

For a two layer board, put the parts on the top. Use the top layer for as much of the interconnects as you can. Reserve the bottom layer as a ground plane, and use it only for short "jumpers" of other signals.

Keep these jumpers separated from each other so that ground currents can flow around each one individually. You want to minimize the maximum dimension of any hole in the ground plane, not the number of holes. Put another way, lots of little dispersed disruptions are better than a single big disruption.

Make all ground connections with separate vias right by each pin that has to be connected to ground. This makes each ground connection solid, and also minimizes the ground connections getting in the way of routing the other traces.

Of course you still have to pay attention to routing the signal traces. Audio is all about keeping the signal to noise ratio high. Don't route amplified output traces near sensitive input traces, for example.

For more information, see this answer.

\$\endgroup\$
  • 5
    \$\begingroup\$ Ah but if you were an audiophile then you would know that through hole parts sound better! /s But seriously in the guitar pedal building community there is an aesthetics thing about through hole \$\endgroup\$ – loudnoises Apr 26 '18 at 12:17
  • 5
    \$\begingroup\$ @OlinLathrop I downvoted for the reason that your answer has nothing to do with Through Hole routing, which is what OP asked for. If they wanted to do SMT, I am sure they would have. This answer is more of a 'here is my opinion, and this is how to make use of it.' So that was my reason. To me, the first sentence of your answer was unnecessary. \$\endgroup\$ – Curious Apr 27 '18 at 13:22
  • 1
    \$\begingroup\$ Olin, why did you ask downvoters to tell you why they downvoted if you aren't going to address the replies? By the 4 upvotes, it seems @Curious wasn't the only one with those thoughts \$\endgroup\$ – MCG May 1 '18 at 10:08
  • 1
    \$\begingroup\$ @Olin, I agree, vandalous downvotes do happen far too often! I have seen you a few times now assume that people do things due to personal hangups or religious reasons... This is not always the case. With things like this, it really doesn't matter why they want to use through hole... Maybe they just prefer it, maybe it is a task they have been set, who knows, it doesn't matter. Just because they ask for help with something you view as not good enough shouldn't mean you offer no help and instead answer with something based on your opinions. \$\endgroup\$ – MCG May 1 '18 at 11:16
  • 1
    \$\begingroup\$ Maybe he's a beginner. I started using through hole right at the beginning when I was learning. I only had very basic equipment and didn't have the tools to make surface mount stuff. So I designed in through hole till I could afford the correct equipment. You should just accept not every reason is religious or a personal hang up, and stop assuming. If you don't agree with the method, don't answer it! If I was the OP and was wanting to do a through hole design, this is a useless answer. Some people design differently to you. Deal with it, you don't have to bring everyone to your way of thinking \$\endgroup\$ – MCG May 1 '18 at 11:20
0
\$\begingroup\$

If you are wondering about ground planes, you have to forget through-hole! Having dedicated ground and power layers is all about maintaining low-impedance paths for all currents. Through-hole components have much additional impedance just from their bulky size and their wires.

If you want to stick to through-hole, I recommend a board that looks pretty much like the schematic. Use ground areas in both the middle of the top and the bottom layer. Use the long edges for V+ and V- paths. Create "copper fingers" from ground to V+/V- or vice versa to account for radial components. If your amplifier circuit needs three or four voltages, use the top layer for one voltage pair and the back layer for the other.

enter image description here

Please also remember, from AC view, V+, V- and GND are just the same. It's as important to have low impedance V+ and V- as GND.

The bottom ground fill is continous where the V+/V- fingers break the top one, and vice versa. Use the THT component's vias for the connection of the two GND fills. That way you give the through-holes a reason for existance. Use additional vias where required.

This is just the opposite from the board design a digital circuit needs. Now imagine the headaches of creating a mixed-signal board.

\$\endgroup\$
  • 1
    \$\begingroup\$ I do not understand why a ground plane is not useful when through hole components are used. I understand the larger impedance of the connection beteen the component itself and the copper layer caused by the component leads (compared to SMD). However, I think a gorund plane contributes to lower the noise of the circuit, since the ground level of a component in the top-right zone of the PCB would be almost the same as the ground of a component placed in the bottom-left area of the PCB,... What do you think? \$\endgroup\$ – Umberto D. Apr 27 '18 at 12:33
  • \$\begingroup\$ This is about having a dedicated ground plane vs. having a ground fill on both the top and the bottom layer. Clearly, the latter has lower internal resistance for the most prevalent currents between adjacent parts of the circuit (because it's two copper layers.) \$\endgroup\$ – Janka Apr 27 '18 at 18:13

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.