Feedback on my first pcb layout

[Analog_Fan]

Based on Matador's wonderful example above, along with all the other feedback in this thread, I've tried reconfiguring this board completely. I've totally overhauled my layout to more closely resemble the schematic layout a la Matador's. I've also completely changed the board size -- I was previously trying to keep it super compact because the project that I intend to use it in will have limited space, but I've now changed it to match the dimensions of a turret board that will house a separate part of the project so that they can be stacked. If anything, the board seems almost too spread out now.

I've added the suggested bypass capacitor. I've also added a footprint for two "optional" resistors to the bases of the output transistors. These were suggested by someone in another thread, but I have yet to clarify whether or not they will actually be needed -- if not, these will be populated with jumpers, which actually solves some minor routing problems anyway.

Before I send off for a couple of boards, any last changes you'd make? Am I still way off the mark?

View attachment 89429

you don't want any these 90º angles in the traces on the board.
source: datasheet CD4053, page 21.



You should place a VIA above C4 heading to the collector, having a roundabout junction or place a squared rotated 45º or triangle polygonº.
a triangle polygon on al of the power rail junctions.

the twin connections to GND on R8, should be one and connect to the other via the other layer, horizontal.
rotate J1 180º and connect GND to vertical to J3 via the other layer.

you want to add a (schottky) diode between GND and the positive rail or interrupt the power rail close to socket and place it there.
Making a mistake is easy and it will burn some of the components.

It's best to place the values/part designators of the resistor/capacitors/semi conductors rather than component numbers.

keep the power rail (horizontal) on one side of the board and (multiple connected) via('s) to pull down/up tracks vertical where it's needed.
do Horizontal tracks on one side and vertical track on the other side, if you would handle ic's you will get in trouble.

Please text where it's needed, like at the jumpers and what's it for.

 

[JMan]

Thanks, I’ll keep this in mind for future boards. I’ve already had these particular boards fabbed, so I’m kind of stuck with whatever imperfections there may be.

 

[Analog_Fan]

Thanks, I’ll keep this in mind for future boards. I’ve already had these particular boards fabbed, so I’m kind of stuck with whatever imperfections there may be.

You're welcome, a master did not drop from heaven.

In the Future, start with power rails first.

this is how i do it.
if you need to switch side, i use multiple via's connect them on both sides, the hole is the width of the trace and the diameter is 2 x width.
But if you have plenty of room, like on your giant PCB's, you might wanna use bigger bigger holes and ad the 2x width of the track to the diameter.

the calculator is my grid.

 

[Analog_Fan]

Here is another i made, a 24 dB filter.


the width is 25 mm.

 

[swpaskett]

Thanks to all the contributors on this thread. It is instructive to a lot of us who have been around the block a few times, too.

As a reluctant Eagle user who shelved it ten or so years ago, then picked it up again when I needed entertainment during the pandemic iso-crisis, I found that they had faithfully preserved much of their off-beat UI behavior over those years, such as doing group selects and operations. Definitely not an intuitive interface.
A lot of the grief noobs encounter with these tools involves establishing a workflow. You usually are on your own for that, a work flow must work for you and the tools you have. I started to write mine down, but it was way too much of me talking.

One thing I did not see in this thread is a caution to review Eagle's design rules and the design rules offered by your fab of choice. Eagle will allow 6-mil traces, an impossibility for many fabs, especially those doing cheap hobby boards. A safe minimum is 8 mil with the fab I use, but I go to 10 normally.

Kudos to the RF layout guys. Most of us are not too concerned about reflections in the audio spectrum. Sharp bends in the audio spectrum were more of a mechanical concern 50 years ago when copper peeled away from boards if you looked at it wrong. I worried about reflection doing GHz+ logic layouts years ago, but never in the audio spectrum. You need really fast edges for that to be a concern. Controlled impedance is another thing we can thankfully ignore. You can put away your Smith Charts.

 

[Analog_Fan]

i tend to use 0.4064 (16 mil), 0.508, 0.6096, 0.8128, 1.016 mm.
but the minimum is 0.4064 mm

0.4064 mm for signals and 0.8128 mm for power (+/-12V), my constraint is the 2.54 mm lead spacing of the dip's packages.
0.4064 mm is the widest you can snake around them pins.

the wider the track, the better for resistance.

In Spain the electric meter / counter of a apartment in a high rise building is downstairs, the first floors have something like 6mm² cable between the meter and the apartment but it gets gradually ticker the more floors you rise, on the 10th floor you might have 50mm² cable to be sure to have 220V up there.

 

[Analog_Fan]

here you have eagle pcb files validated by a external lab:

Mutable Instruments
https://github.com/pichenettes/eurorack

 

[user 37518]

You're welcome, a master did not drop from heaven.

In the Future, start with power rails first.

this is how i do it.
if you need to switch side, i use multiple via's connect them on both sides, the hole is the width of the trace and the diameter is 2 x width.
But if you have plenty of room, like on your giant PCB's, you might wanna use bigger bigger holes and ad the 2x width of the track to the diameter.

the calculator is my grid.

I don't see any ground planes anywhere in sight in your design...

Having the vertical traces on one side and horizontal on the other might be useful to make the tracing easier for the PCB designer, but signal integrity and crosstalk wise it is a disaster, unless you have some extra layers with ground planes that you are not showing, I don't even see ground fillings.

My contribution: In a 2 layer design, try to route as much as possible on one side whilst keeping a continuous ground plane on the other side. Avoid crossing traces on top of each other (like Analog_Fan did), specially if they are carrying different audio signals like busses in a mixer.

If you don't use a ground plane, you should still provide a ground trace at the opposite side of the signal trace so you can control how currents return through that ground trace. The faster you start thinking of traces as transmission lines (microstrip or strip line) rather than 'cables' which join things together, the better your designs will be.

 

[Analog_Fan]

i didn't press ratsnest and the ground plane wasn't generated.
i use trillions of vias to keep the ground plane intact

i have considered the magnetic fields between the layers when crossing them, but what can you do!
i created them all or many like that and the all work, maybe in the future i have a gHz scope and can do a better investigation.

 

[user 37518]

i didn't press ratsnest and the ground plane wasn't generated.
i use trillions of vias to keep the ground plane intact

i have considered the magnetic fields between the layers when crossing them, but what can you do!
i created them all or many like that and the all work, maybe in the future i have a gHz scope and can do a better investigation.

You don't need a GHz oscilloscope, a regular 20 MHz scope should be enough to test them.

 

[Analog_Fan]

You don't need a GHz oscilloscope, a regular 20 MHz scope should be enough to test them.

You can detect stuff using inductors attached to your probe and hover over the pcb's while functioning.

 

[Matador]

Having the vertical traces on one side and horizontal on the other might be useful to make the tracing easier for the PCB designer, but signal integrity and crosstalk wise it is a disaster, unless you have some extra layers with ground planes that you are not showing, I don't even see ground fillings.

Can you elaborate, as this doesn't make sense to me. Having a two traces cross on separate layers at 90 degrees minimizes the cross sectional area where they overlap, which (all other things being equal) would minimize crosstalk.

I think I said earlier that ground planes (in audio, mind you) always work except when they don't. At higher audio impedances (especially in common tube topologies), even 1pF imposed across 1M is a LPF at 15kHz, so 5 or 6 inches of trace over a ground plane can easily reach down into the audio band if you aren't careful. This bit me once when I tried to jog a grid and plate trace over each other which formed a few pF worth of layout capacitance which significantly altered the gain characteristics of the stage.

If you know you are dealing with impedances of 100k or less then it probably matters much less.

 

[user 37518]

Can you elaborate, as this doesn't make sense to me. Having a two traces cross on separate layers at 90 degrees minimizes the cross sectional area where they overlap, which (all other things being equal) would minimize crosstalk.

I think I said earlier that ground planes (in audio, mind you) always work except when they don't. At higher audio impedances (especially in common tube topologies), even 1pF imposed across 1M is a LPF at 15kHz, so 5 or 6 inches of trace over a ground plane can easily reach down into the audio band if you aren't careful. This bit me once when I tried to jog a grid and plate trace over each other which formed a few pF worth of layout capacitance which significantly altered the gain characteristics of the stage.

If you know you are dealing with impedances of 100k or less then it probably matters much less.

Having two traces cross at 90° does minimize crosstalk, but the best solution is that they do not cross at all, that is my point, that you should strive to not cross traces rather than make them cross like you don't care just because it makes the tracing easier, crosstalk is not the only issue, it also provides a discontinuity for the ground plane or ground conductor, the fields spread and leak to other places, etc... I do agree that with only 2 layers it is very hard to only route stuff in one layer and prevent traces from crossing, but one should do this only when no other tracing solution is available. More importantly, what I am saying is that in a 2 layer board, not having a ground plane and/or not providing a clear trajectory for the return currents so you can just use that layer to facilitate the routing is not the best approach, which is exactly what Analog_Fan is doing, I can't see any clearly designed ground, be it a ground plane or return conductors, it just seems that he uses 2 layers to facilitate the routing and nothing else. This is what I am criticizing, also, neither the PCB posted by Analog_Fan nor the one in the first post seem to be tube-based or very high impedance circuits.

I've also pointed out that even if you don't have a ground plane you should really provide a defined ground trace for the return, ideally at the opposite side of the signal trace to control and guide the return currents properly, and to confine the fields to a certain volume/area; in tube circuits another approach might be more suitable. But be it a ground plane or not, you can't neglect ground.

Ground planes do not work for everything, I agree, for high frequency circuits they are the best, for audio, its more of a compromise, but if you don't know what you are doing its best to have a ground plane than just use two layers to route stuff willy-nilly and hope that the signal will find its way back somehow.

 

[JMan]

Do you have thoughts on ground planes vs a good fat ground trace (that doesn't meander) in a low voltage power supply section? I'm thinking of your standard LM317 circuit and variations thereof. I see that you say ground planes are something of a compromise for audio, and I wonder if there are similar pros/cons to consider with power.

I'm continuing to try to learn and improve my pcb layout skills. I've come a VERY long way since the first post, but of course the things I don't know still massively outweigh the things I do.

 

[JohnRoberts]

Do you have thoughts on ground planes vs a good fat ground trace (that doesn't meander) in a low voltage power supply section? I'm thinking of your standard LM317 circuit and variations thereof. I see that you say ground planes are something of a compromise for audio, and I wonder if there are similar pros/cons to consider with power.

not an either or but sometimes both or all of the above... We want ground and power traces to be low impedance while ground planes also offer some shielding.

I'm continuing to try to learn and improve my pcb layout skills. I've come a VERY long way since the first post, but of course the things I don't know still massively outweigh the things I do.

It can be a very long journey to make perfect PCB layouts (no such thing).

One thing that helps me visualize current flow is to think of PCB traces as resistors which Ohm's law teachs us develop voltage drops across them from flowing current. Of course this is only one dimensional thinking, next we need to consider magnetic fields radiating into 3d space and capacitive coupling between effective plates, or antennas.

I don't mean to scare you, master one concept at a time.

JR

 

[Analog_Fan]

Do you have thoughts on ground planes vs a good fat ground trace (that doesn't meander) in a low voltage power supply section? I'm thinking of your standard LM317 circuit and variations thereof. I see that you say ground planes are something of a compromise for audio, and I wonder if there are similar pros/cons to consider with power.

I'm continuing to try to learn and improve my pcb layout skills. I've come a VERY long way since the first post, but of course the things I don't know still massively outweigh the things I do.

you can use starground aswel, have localized ground planes around your groups and later join them, just don't place a giant polygon of a total pcb area.
aswel different types of "polygon pour". in eagle you got up to 6 layers or ranks and it will be subtracted from from the main polygon as long as that one is highest ranked. that's something you do around a crystal on both side.

You can be Rembrand if you wanna be.

 

[user 37518]

Do you have thoughts on ground planes vs a good fat ground trace (that doesn't meander) in a low voltage power supply section? I'm thinking of your standard LM317 circuit and variations thereof. I see that you say ground planes are something of a compromise for audio, and I wonder if there are similar pros/cons to consider with power.

I'm continuing to try to learn and improve my pcb layout skills. I've come a VERY long way since the first post, but of course the things I don't know still massively outweigh the things I do.

Added to what John said.

My emphasis on the ground plane or trace under the signal trace applies mostly to AC, not DC. There is a general misconception that current takes the path of least resistance or the shortest path, that is only half true, the real thing is that current takes the path of least impedance, which does not necessarily means the shortest path nor the path of least resistance.

As the signal frequency gets higher, the path of least impedance for the return currents is directly under the signal trace, since this is the path with lowest inductance and greatest capacitance, and resistance can be neglected in most cases, thus, the path with lowest impedance is simply the square root of L/C; this means that even if there is a shorter path someplace else, the return current will not necessarily take it. This doesn't happen with DC since the frequency is essentially zero, making the contribution of the imaginary part of the impedance zero as well. With DC it does take the path of least resistance, which usually means the shortest path.

With DC linear power supplies like the LM317 that you mention, usually what matters the most is that you have beefy ground and voltage traces, regardless of whether the ground trace is directly under the voltage trace or not, aside from the advantages that John mentioned. Also, having a ground trace directly under the voltage trace can help you control the amount of "spreading" of the current and fields and the path it takes, with DC, current and fields tend to spread out or occupy a larger area/volume than high frequency AC. In this case, a ground trace rather than a ground plane, allows you to have better control of the path the return current takes, with ground planes you have no say in it...

 

[JMan]

Added to what John said.

My emphasis on the ground plane or trace under the signal trace applies mostly to AC, not DC. There is a general misconception that current takes the path of least resistance or the shortest path, that is only half true, the real thing is that current takes the path of least impedance, which does not necessarily means the shortest path nor the path of least resistance.

As the signal frequency gets higher, the path of least impedance for the return currents is directly under the signal trace, since this is the path with lowest inductance and greatest capacitance, and resistance can be neglected in most cases, thus, the path with lowest impedance is simply the square root of L/C; this means that even if there is a shorter path someplace else, the return current will not necessarily take it. This doesn't happen with DC since the frequency is essentially zero, making the contribution of the imaginary part of the impedance zero as well. With DC it does take the path of least resistance, which usually means the shortest path.

I hope you'll forgive the question, but can you explain what you mean by "the path of least resistance" versus "the path of least impedance?" In my layman's mind those two terms are synonymous.

 

[JohnRoberts]

I hope you'll forgive the question, but can you explain what you mean by "the path of least resistance" versus "the path of least impedance?" In my layman's mind those two terms are synonymous.

impedance is different for different frequencies... so a simple resistance analysis may not be fully representative for HF current flows.

JR

 

[JMan]

impedance is different for different frequencies... so a simple resistance analysis may not be fully representative for HF current flows.

JR

Thanks, John! I hadn't ever considered this, but it seems so obvious once it is said.