Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › How to optimize a PCB?
New Posts  All Forums:Forum Nav:

How to optimize a PCB?

post #1 of 8
Thread Starter 

When designing a amplifier PCB is there any rule to make it sound best? Or just make every signal trace as short as possible in one side and another side is full ground plane? I ask this because when i make a point to point o2 in a perfboard (the wiring was very nasty, and there were some very long traces but every ground points were star grounded at one point) and it sound as good as a well build O2. Next time i design a very compact o2 board, the wiring is clear, signal traces were very short, and i tried to make ground plane as close to an original O2 as possible but in the end, it sound weird: the sound was very close in, feel like my head is inside a box, details is still great though.

post #2 of 8

No knowing the specifics of the circuit, keep in mind that AC is noisy, so keep the AC portions of your circuit as far away from the signal path as possible.

post #3 of 8

Designing a PCB is a true art.

 

Two designers, both following the exact same set of design rules,

will design very different boards for the same circuit.

 

As far as optimizing...I try to keep and neat and tidy,

organized as to signal flow and divided into functional blocks.

I will probably go through a half dozen versions before

I settle on one that looks good. Then I sit on it for a week

or two and then review it again.

Some people seem to have a natural knack for it and some

always seem to struggle.

 

There is something to be said for untidy wiring. Wires run

parallel to each other can couple signals. Wires that cross

at right angles interact very little. Traces on a circuit board

behave the same way.

post #4 of 8

There are multiple rules.

 

Keep the inputs away from the outputs. For example, keep the inputs on the LHS and the outputs on the RHS and feed the power in from the top or bottom, keeping any PSU section from invading the signal parts..

 

Don't run signal traces in parallel, cross them at right angles if absolutely necessary.

 

Run the power traces as close together as possible, particularly for any class B sections.

 

Run the ground returns from each section independently, or at least keep the low current returns at the far end of the string and the high current returns close to the ground point. Google 'star grounding'. If you do use a ground plane try to make sure there is an uninterrupted 'line-of-sight' return for each grounded point and that the sightlines don't cross. Sometimes a slot in the groundplane can serve to keep unwanted mingling of ground returns to a minimum.

 

Keep power supply decoupling caps as close to the pins they serve as possible. Keep the loop area enclosed by the pins as small as possible.

 

If any transformers or inductors are used, give due consideration to the fields generated by them, amplifier output inductors for example should not be placed inline as the interaction will be at a maximum. Distance is the cheapest isolator.

 

Don't run traces under IC components or between pins if at all possible. This is of lesser importance in digital circuits, but signal integrity is of increasing importance as clock frequencies rise. Don't locate vias under ICs.

 

Keep any digital section away from the analog section, with an independent ground plane. Join the ground planes at a single point and consider what currents may pass through that point, organizing the layout to minimize them. Don't use higher frequency clocks if it is avoidable.

 

These rules are important, but can be modified by other considerations, for example a commercial product may have style considerations affecting the input and output positions on an enclosure, plus there are volume and maybe tone controls, LED indicators, input selectors, etc.

 

Be prepared to respin a board on the basis of what is learned from the first iteration.

 

Don't join traces at less than 90 degrees, this is called an 'acid trap'. It increases the difficulty of isolation routing if it is used at some stage. Chamfer all right angle turns. This is of less importance in low frequency (baseband) PCBs, but it's a good habit to get into. Beef up the tracks, as a general rule make them the same size as the component pads. You can use thinner, in some cases it's necessary, but same size as the pin pads is a good rule of thumb.

 

I'm sure there are other things other people will think of, this is just what occurs to me off the top of my head.

 

w

post #5 of 8

 

I can add that at higher frequencies, the return signal tends to follow the signal trace

rather than taking a direct route. Avoid cutting a ground plane where a high frequency

signal will cross it.

post #6 of 8

Here is a good article on mixed signal grounding techniques.

Part 1

Part 2

post #7 of 8
Thread Starter 

Thanks all for your replies, i have just read nwavguy blog and found some helpfull information about pcb routing:

Quote:
EMI Loops – Think about where the higher currents flow. You want to keep the “loop area” of those currents as small as possible. For example, I’ve seen several boards that more or less route a power supply rail up each edge of the board and the ground up the center. It’s very logical, neat and tidy. But it’svery poor practice for analog audio. All the currents flowing from the rails, through the load, and back to ground are spread wide apart creating a single turn coil or inductor with your entire circuit nestled right in the middle of each “loop” where all the resulting EMI fields are the worst. And even a 3 channel or bridged (balanced) amp doesn’t solve the problem because the return current is to the opposite rail which is still on the other side of the board. It takes some serious thought to imagine all the current paths and the loops they form. Then it’s even more of challenge, especially on a cramped board, to minimize those loops while still being able to route the entire PCB in 2 layers.

 

Can some one give me some more examples about current loop?

 

Quote:

Inductive Currents – Don’t run high gain input signals parallel to anything with much current flowing. There will be inductive coupling that can (depending on the signals) significantly increase distortion, degrade crosstalk, and worst of all, create instability if it’s out of phase with whatever it’s next to or generates positive feedback to an amp input. Doug Self has examples of 100 times greater distortion and I’ve seen similar results from various half-baked designs.

 

Does "high gain input signals" is signal from the source or signal from the voltage stage to output stage? When he said "Don’t run high gain input signals parallel to anything with much current flowing" does that mean i can still route input signal traces and high current trace near each other but with different angle that make them not pararrel? And is it fine if i make these trace parrarel but in differnet side of pcb?

 

Quote:

Watch Parasitics – If you dig deep into datasheets and/or application notes, especially for faster parts, you’ll often find some advice on keeping the part stable. One problem can be parasitic capacitance and inductance. Amplifiers hate positive feedback as it turns them into oscillators. Yet I see all sorts of questionable routing where outputs are coupled to positive inputs in ways they never should have been. You may not always want ground fills around the input pins of op amps, for example, as that creates parasitic capacitance that can degrade stability.
post #8 of 8

A typical example of where a current loop applies is the power supply decoupling capacitors. The general advice is that a 100nF cap should be placed between the power rails of an audio chip or between the power pin and ground of a digital chip. These caps are positioned absolutely as close as possible to the pins which they decouple. In the case of high-speed digital circuits trouble is taken to route directly to the ground plane by using via-in-pad because of the improved decoupling achievable. This minimises the loop area of the circulating currents which arise because of the varying demands the chip makes on the power supply. The way these caps function is sometimes thought of in 2 different ways, they can be thought of as providing a reservoir supplying the short-term current demands of the IC, or they can be thought of as providing a low-impedance path for the dissipation of high frequency currents flowing between the IC pins.

 

For 'high-gain input signals' read 'input signals'. The inputs have a high gain with reference to the outputs. You should keep input signal traces away from high current traces, but crossing them at right angles is better than running them in parallel. You have to think about this sensibly though. It won't be a problem to route an input trace parallel to a trace carrying DC that activates a relay, even though this may be a high current, because it has no significant AC component. Traces on opposite sides of the board are not immune from crosstalk if routed in parallel.

 

w

New Posts  All Forums:Forum Nav:
  Return Home
Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › How to optimize a PCB?