Next level PCB layouts

[m_charles]

Hi there, this is kind of a two part question.

I've begun working with KiKad, gotten to the point where they look nice, work well, etc. Now trying to go beyond simply making things work, and connecting what needs connecting, delving more into laying things out intelligently, for quiet operation, etc.
I do realize there are huge books just on this subject alone, but figured I'd ask here for any quick tips or definite dos and don'ts you folks keep in mind when making layouts.

Starting a new design (typical 2 layer SMD project, components on one side only) and had the thought of separating all input and output lines on different sides of the board in order to use the ground plane to isolate things. Figured this would be good for high gain style circuits. Seem like a good idea? Good practice?

Would put signal from in-jack to switch, then from switch to circuit input on one side, opposite for the outputs. Then use a via for whichever is on the component side. think it matters which line is on the component side?

Anyways, thx in advance for your tips!

[phasetrans]

...Starting a new design (typical 2 layer SMD project, components on one side only) and had the thought of separating all input and output lines on different sides of the board in order to use the ground plane to isolate things. Figured this would be good for high gain style circuits. Seem like a good idea? Good practice?

Would put signal from in-jack to switch, then from switch to circuit input on one side, opposite for the outputs. Then use a via for whichever is on the component side. think it matters which line is on the component side?

If you really want to learn this topic for the general case, Robert Feranec, Eric Bogatin, and Richard Hartley are the names I suggest you start with.

That said, analog audio circuits, while governed by the same physics, are idiosyncratic in a number of ways:
1. Frequencies are very low, so return currents tend to spread out in planes / pours
2. We rarely have to worry about emitting EMC, and if we do is typical well below 150kHz where the emissions levels start to tighten
3. Currents are small
4. We don't need to much consider parasitics of board features, or distributed capacitance or inductances
5. Again due to low frequencies, the impedance of power distribution in the board usually is well below parasitic resonances
6. We are sensitive to noise
7. We can have high gains in some circuits

Practically, a 2 layer board with everything routed as microstrip on a single layer will almost always be fine. The only really low level signal is the initial input before it is gained up.

Otherwise, keep loops small for any switched currents, bypass your opamps, keep some pads open to slow down an opamp when needed. Use a thinner dielectric, typically down to 0.8 or 0.6 is the same price from Asia.

Or, go enjoy the relative flexibility analog FX offer for PCBs and start looking at clever artistic things like BeeTronics or the pcb artwork of Saar Drimer.

[m_charles]

...Starting a new design (typical 2 layer SMD project, components on one side only) and had the thought of separating all input and output lines on different sides of the board in order to use the ground plane to isolate things. Figured this would be good for high gain style circuits. Seem like a good idea? Good practice?

Would put signal from in-jack to switch, then from switch to circuit input on one side, opposite for the outputs. Then use a via for whichever is on the component side. think it matters which line is on the component side?

If you really want to learn this topic for the general case, Robert Feranec, Eric Bogatin, and Richard Hartley are the names I suggest you start with.

That said, analog audio circuits, while governed by the same physics, are idiosyncratic in a number of ways:
1. Frequencies are very low, so return currents tend to spread out in planes / pours
2. We rarely have to worry about emitting EMC, and if we do is typical well below 150kHz where the emissions levels start to tighten
3. Currents are small
4. We don't need to much consider parasitics of board features, or distributed capacitance or inductances
5. Again due to low frequencies, the impedance of power distribution in the board usually is well below parasitic resonances
6. We are sensitive to noise
7. We can have high gains in some circuits

Practically, a 2 layer board with everything routed as microstrip on a single layer will almost always be fine. The only really low level signal is the initial input before it is gained up.

Otherwise, keep loops small for any switched currents, bypass your opamps, keep some pads open to slow down an opamp when needed. Use a thinner dielectric, typically down to 0.8 or 0.6 is the same price from Asia.

Or, go enjoy the relative flexibility analog FX offer for PCBs and start looking at clever artistic things like BeeTronics or the pcb artwork of Saar Drimer.

Not sure what you mean by "bypass op-amps". Can you clarify?

[PRR]

https://app.thebookpatch.com/BookStore/pcb-layout-for-musical-effects/5cfb5bb2-4c9e-4b4f-864d-b03134a327a2

[m_charles]

Ha, didn't even know that existed. will def pick it up. Does RG sell a PDF version?

[FiveseveN]

I like videos more than books: https://www.youtube.com/playlist?list=PLXSyc11qLa1b9VA7nw8-DiLRXVhZ2iUN2

[phasetrans]

Not sure what you mean by "bypass op-amps". Can you clarify?

Bulk capacitance from rail(s) to ground immediately adjacent to the power input(s) of each opamp.

[phasetrans]

Any easy way to immediately make your boards look cooler is using OSHPark "after dark"

This is black FR-4 core, ENIG, clear soldermask, white silkscreen:

https://blog.oshpark.com/tag/after-dark/

[PRR]

Does RG sell a PDF version?

You can only sell one PDF. (Same as cassettes and MP3s swamped LP sales, PDF piracy quickly damps book sales.)

[Processaurus]

Use a thinner dielectric, typically down to 0.8 or 0.6 is the same price from Asia.

Why?

[Processaurus]

RG's book is a great buy if you are getting into fx pcb design.

The advice I could add is to start the PCB layout with all of the mechanical stuff first- don't wait to figure out how to mount the board in the box, or where you want the controls, or where you want the wires coming in. Group wires that will be coming from a pot or switch together if possible, and it's nice to have them at the edge of the board. Always make a few extra ground pads around for testing and mods. A piece of bare solid core wire attached to two ground pads is very nice for hooking up a scope or meter. If there is extra room on the board make a .100" spacing perfboard area for mods and experiments.

If you can do CAD figure out how to export a DXF layer from the CAD into the PC board design program, and everything fits like glove. Don't worry about pc board mounted pots unless you're making more than a couple, panel mount parts flying out on wires are much easier and actually more reliable, it just takes longer per unit, so you avoid it for mass production. One offs, the wires are good. The drilling can be a little off and everything will still fit.

On the power connection, I'll do a .100" spaced 3 pin header. Ground goes on pins 1 and 3, +9v power goes in pin 2. This way if you use a little connector, you can reverse the connector orientation and not reverse the power polarity.

Get your silkscreen labels on early, before you run out of space by running your layout everywhere. Circuit name, your handle, year, revision number (don't space on that one), a blank white space where you can serialize the board with a sharpie. There should be a way in your pcb program to use special TrueType fonts to personalize it.

It's helpful to route the board after the silkscreen part designators get sorted out, otherwise it is easy to get into trouble where the designators get confusing because they're all crammed together weird. I like orderly rows of parts but don't compromise too much on the layout, and definitely don't bother with with twidgey symmetrical stuff, let the layout happen organically and keep traces short. It is very helpful to orient electrolytic caps polarity all in one direction, so you can tell at a glance if they are all stuffed right. It's nice to have the outline of LEDs with the flat spot in right place so there isn't head scratching putting it in.

After doing the layout I go back and re-annotate the part designators so they are in order on the board going top to bottom, left to right. It makes it random on the schematic but it is so much nicer assembling the board, not having to hunt around for every resistor.

I got into integration with the component parameters and BOM this year, putting in part numbers and supplier numbers as parameters in the schematic stage, so it was possible to generate a shopping list at Mouser semi-automatically, or at least keep track of special part numbers and where to get them, or notes attached to a certain component that shows up in a cell on the BOM, even if the note isn't cluttering up the schematic.

[PRR]

PCBs in another field:
The Original Macintosh: PC Board Esthetics
https://www.folklore.org/StoryView.py?project=Macintosh&story=PC_Board_Esthetics.txt

[soggybag]

I'll second Processaurus, look at the outside of the box first. Think about where you want your volume knob and other controls, think about the size of the knobs, placement of switches, where you want the foot switch, where you want the DC jack etc.

Put all of those parts on the board first. Then add all of the other components.

If you're trying to make a product that people can use and enjoy using you have to start with the things people will be working with.

Getting all of that stuff right is a whole game in itself. It doesn't always put the other components in the most advantageous locations either.