Looking for some advice on PCB design/layout

[SpaceCowboy]

Hello all, so I've built a FV-1 based FX platform and it's gotten past the prototype stage and now I'm looking to design some PCB's to mount the design...

Anyway, after screwing around a bit in Eagle I've laid out the schematic and started the corresponding PCB layout.
Attached are some pictures of the schematic and the PCB.

With regard to the PCB's I've minimized the number of vias and spaced out the traces quite generously.
But I know there's a whole bunch of stuff that I probably didn't cover so,
any advice and critique of the layout would be appreciated! Thanks


(Sorry schematic is cut off, the 24lc32 eeprom is at the bottom.)

[R.G.]

But I know there's a whole bunch of stuff that I probably didn't cover so,
any advice and critique of the layout would be appreciated!

It's certainly not a bad job.

I did not delve through it in detail, just looked enough to get the sense of the layout style.

Meta-advice:
- know what voltages and currents travel on each conductor, and what the source and load impedances at each end of each trace are.
Yes, I know that sounds like saying "know everything". But there is an order of criticality involved. The more that there are (1) fast voltage changes or (2) high voltage, or (3) fast current changes or (4) high currents or (5) high impedances the more you need to worry about that trace. The faster the voltage changes on a trace, the more the trace has to involve RF techniques of short, direct, and controlled impedance to keep from radiating to other things near it and avoid unwanted resonances and ringing from the impedance of the trace itself. Fast digital edges qualify here. The clock and crystal signals on your PCB are satisfyingly short and direct, and over ground plane. What about the other traces? What signal is on them? Logic speed? Audio? Ground? Ground carries the mix of all signals. That's a big deal. High impedance inputs can be contaminated by the 1-2pF of capacitance to a nearby trace.

Part layout:
- Put in the mounting holes FIRST; then the positions of any parts like controls which have to fit other external mechanical positions. Compared to the position of a tone or volume knob, the resistors and caps can go anywhere.
- Put all the polarized caps and diodes pointing the same direction. It's less confusing to stuff parts.
- Don't overly contort the traces to do it, but minimize the length of traces by putting components right next to each other
- Spread components out for easy insertion.
- Yes, those last two contradict one another.
- Don't split your ground plane. Small divots and crossovers breaking the plane aren't too bad, but long plane-side traces defeat many of the purposes of a plane.
Better to do a number of vias and short crossovers than to split the plane with long traces. Of course, if your highest frequencies are audio, the currents are low, and the impedances are high, then you need to worry more.
- There is no perfect layout.

[Labaris]

Looks great SpaceCowboy (I can´t give you any advice, sorry)

And golden rules R.G.! Thanks  

[slacker]

Why are you connecting Switch pins 1 and 2 to ground? That will only let you select two programs on the EPPROM, is that what you want?
Are you using a ground plane on the other side of the board for some of the ground connections? If not you've got a lot of grounds missing.

[SpaceCowboy]

But I know there's a whole bunch of stuff that I probably didn't cover so,
any advice and critique of the layout would be appreciated!

It's certainly not a bad job.

I did not delve through it in detail, just looked enough to get the sense of the layout style.

Meta-advice:
- know what voltages and currents travel on each conductor, and what the source and load impedances at each end of each trace are.
Yes, I know that sounds like saying "know everything". But there is an order of criticality involved. The more that there are (1) fast voltage changes or (2) high voltage, or (3) fast current changes or (4) high currents or (5) high impedances the more you need to worry about that trace. The faster the voltage changes on a trace, the more the trace has to involve RF techniques of short, direct, and controlled impedance to keep from radiating to other things near it and avoid unwanted resonances and ringing from the impedance of the trace itself. Fast digital edges qualify here. The clock and crystal signals on your PCB are satisfyingly short and direct, and over ground plane. What about the other traces? What signal is on them? Logic speed? Audio? Ground? Ground carries the mix of all signals. That's a big deal. High impedance inputs can be contaminated by the 1-2pF of capacitance to a nearby trace.

Part layout:
- Put in the mounting holes FIRST; then the positions of any parts like controls which have to fit other external mechanical positions. Compared to the position of a tone or volume knob, the resistors and caps can go anywhere.
- Put all the polarized caps and diodes pointing the same direction. It's less confusing to stuff parts.
- Don't overly contort the traces to do it, but minimize the length of traces by putting components right next to each other
- Spread components out for easy insertion.
- Yes, those last two contradict one another.
- Don't split your ground plane. Small divots and crossovers breaking the plane aren't too bad, but long plane-side traces defeat many of the purposes of a plane.
Better to do a number of vias and short crossovers than to split the plane with long traces. Of course, if your highest frequencies are audio, the currents are low, and the impedances are high, then you need to worry more.
- There is no perfect layout.

Hmm that's some insightful stuff lol. Wrt current & volts, max amount of current drawn should be ~80 milliamps and this is drawn by the power supply and supplied to the IC's through the power supply trace. The 10mil trace width should be more than enough for power and signal currents. Now, wrt signal freq and rf interference... the max signal freq should be < 25kHZ and the large 100uF cap should filter out high frequncy rf interference from the power supply. I've taken care to space traces out so that stray capacitance between traces is minimized. Now, the traces to the audio in and out are quite long and have a impedance of ~6000 ohms at 1kHz, but that rerouting that would mean having to re layout the PCB. Oh well. Lol.

Otherwise I've rerouted some of the traces the SOIC so that solder bridges don't form when soldering and put some vias so there are less top traces under the IC's and moved the decoupling caps closer to the parts they are supposed to decouple.

Why are you connecting Switch pins 1 and 2 to ground? That will only let you select two programs on the EPPROM, is that what you want?
Are you using a ground plane on the other side of the board for some of the ground connections? If not you've got a lot of grounds missing.

Yeah only two programs are selected using a toggle switch... don't have enough room for a rotary switch and yeah the ground plane is the bottom black layer... i presume. Lol.

Edit: total input impedance is the total impedance of the all passive components in the input signal path to the pin1 of the FV-1, right?

[SpaceCowboy]

Hmm just a question... I'm planning on getting the board printed at oshpark. I've already uploaded the board file to their site and got the preview for the layout. My question is,are the ground plane connections to all the grounded pads good to go? In the Board Bottom it didn't look like there where any of those cross shaped leads to the ground plane on the grounded pads, though the bottom copper layer preview did have them. I've followed the guideline for grounding the board the the polygon named GND and rat's nest and such... anyway am I good to go?

[CodeMonk]

Looks good to me.
Although the traces near the pads of R6, R7, and R8 are a little to close for comfort, for me anyway.
I see a few other spots like that as well.
On your first image that is.

Having boards made for you, its probably not a huge deal, but I make a lot of my own boards and that would be an issue.

[SpaceCowboy]

Yeah, the traces come close, but nothing that sets off the oshpark DRC. But it's worth it, total board size is a partial 60 mm x 45 mm!