Here's an AIO layout for ROG's Thunderbird (Marshall Super Lead 100 inspired circuit) . This circuit was off my radar until I read @Chuck D. Bones's build report. 1776 used to offer a board for this one, but they're now closed and it seems nobody else is offering boards for this one currently. I have another layout without the built-in bypass, but including it on this one dramatically simplifies wiring and allows me to better isolate the high impedance input line compared to having the I/O connections at the bottom. A red board seemed fitting for this project, but that may change by the time it's ordered. According to a couple sources, this circuit has a tendency to be noisy, hopefully I've taken sufficient steps in the design to avoid some of that .
I almost always type "µ", it's easy enough on a Mac:
Hold "OPTION" key down and then hit "M" — gives me a perfect "µ" every time, so long as the caps-lock isn't on, then it gives me:
"Â".
NO NEED to type "uF", when "µF" is right there under the fingerboard...
I almost always type "µ", it's easy enough on a Mac:
Hold "OPTION" key down and then hit "M" — gives me a perfect "µ" every time, so long as the caps-lock isn't on, then it gives me:
"Â".
NO NEED to type "uF", when "µF" is right there under the fingerboard...
I was wondering if I can get a second set of eyes on my first KiCad project - a basic footswitch breakout. I had to make the symbols and footprints myself (based off some MadBeans libraries), so it seems like there's a lot that could have gone wrong.
I wanted the following features that I haven't seen on other breakouts:
All headers labeled
Silkscreen reminder of how the lugs were wired
Headers labeled on the reverse side as well
My own name on it .
In the screenshot above I hid the rear silkscreen for clarity. JLC isn't rejecting the gerber file, and I figured I'd use their panelization option (any panelization on JLC seems to add $4 overhead - an "engineering fee") to get 125 breakouts for $7. I'd upload the gerber file here but the forum doesn't allow it.
All connections look correct, your F.Silkscreen layer looks fine. I cannot confirm the footprint for the switch will work and the only recommendation I'd give is to increase your trace sizes a little. If you only increase the trace size on one, make it the trace carrying the SW net.
Thanks, @Brett! I've adjusted the traces for the footswitch to be .3mm (they were .2).
I've got a follow-up question for y'all - you seem like wizards here. I'm working on translating a simple board from Effects Layouts (the One Knobber - which supports various versions of a DAM Meathead). I've gone through a KiCad tutorial series ("Getting to Blinky"), and skimmed all 29 pages of this thread, but I can't seem to find any examples of a "good" way to set up a schematic, footprints, and layout for a pedal build. In particular the offboard wiring. I'm sure there's a good way and other less good ways of doing this, and I'm interested in feedback.
What I ended up doing was creating footprints for the DC holes, and for the IN/OUT/9V/GND adjacent holes. Then I created a schematic with three pages: one for the circuit, one for the input and LED, and one for connectors. For all the offboard connections I put a wire going nowhere with a label. Then on the connector sheet, I put the label to the footprints that represented the holes. For audio jack ground I just used mounting holes. It looks like this:
The power section looks a bit different than what I'd expect, but I think it's basically what the one-knobber schematic was showing. This seems relatively clean/scalable to other designs, but I also feel like I'm probably overlooking something. I left out values since the One Knobber supports a bunch of different values for different builds.
Then for my PCB I laid it out like below (I'm sure this is gross looking in general, and I still need to clean up the silkscreen and everything). One of the challenges was trying to figure out which connections I needed to actually route, and which the filled zomes would take care of on their own. I think this led to poor placement of some components because certain wiring wasn't needed. I was trying to make it as small as possible to mostly fit behind the pot, but still have full offboard wiring and an onboard LED.
Anything stand out as really wrong, either with the schematic or the layout? Apologies, I'm really confronting the limitations of my electronics and KiCad knowledge at this point, but I'd appreciate any feedback!
I'll be the first to tell you that I, for one, am no wizard. If I were, I'd probably be doing something more interesting. All of what I am about to suggest is just how I do things, not that it's the "best" or "right" way to do things. Everyone has their own way of doing things, these are just suggestions based on what works for yours truly.
Then I created a schematic with three pages: one for the circuit, one for the input and LED, and one for connectors. For all the offboard connections I put a wire going nowhere with a label.
Not that you can't do it this way, but it seems overly complicated to create separate pages for each section of the schematic with a circuit as simple as this. This circuit is all analog and is relatively small, usually separating schematic sheets is typically reserved for high pin count mixed signal designs. In my own opinion, off-board connections can be made more simply and cleanly using a named PAD footprint or a global label. Something like this:
The power section looks a bit different than what I'd expect, but I think it's basically what the one-knobber schematic was showing. This seems relatively clean/scalable to other designs, but I also feel like I'm probably overlooking something.
This power supply design is usable, but you might find that using a series Schottky diode is more effective. Follow along with the majority of the projects on PedalPCB and use a 1N5817 in series. See my thumbnail posted above. You'd just put the diode in series in lieu of the placement of D1 in your schematic.
I know you said that you didn't assign values to passive components but it's generally good practice to assign some "default" value to components. Otherwise, asking anyone for guidance on whether or not your circuit is going to work as drawn is very difficult to determine. Case in point, if you intend to use a 100µF bulk capacitor in C1, that would work fine. If you chose to use a 1µF, it *may* also work, but not as well as a 100µF. Additionally, knowing values of capacitors is important as it relates to the size of the footprint. If you do plan on using a 100µF in C1 and this circuit needs to accept up to 18V, you may have a difficult time finding a 100µF electrolytic capacitor that fits the footprint you've chosen to use on your layout.
One of the challenges was trying to figure out which connections I needed to actually route, and which the filled zomes would take care of on their own. I think this led to poor placement of some components because certain wiring wasn't needed. I was trying to make it as small as possible to mostly fit behind the pot, but still have full offboard wiring and an onboard LED.
Everyone has their own opinions on this subject, but I am not the biggest fan of putting my positive or negative power rail (in cases where a dual supply is used) on a copper pour. I don't have concrete evidence for why I avoid this other than trying to keep potential sources of noise away from sensitive signals. Using a single bulk capacitor in your power section isn't doing much (if any) filtering on your incoming power. Any noise introduced by your incoming power will surround all traces where your copper pour for the +VIN rail on your board. With high speed designs, it may be beneficial to handle copper pours like this, but not so much with low-level analog. Instead, I like to have ground pours on both sides of the board and keep power connections as isolated from high-impedance paths (your input traces, for example) as possible.
Another thing I'd recommend is to add a little more separation between your components/pads/traces. I like to have enough separation between tracks and pads so that my copper pour (and I use ground here) can flow between them, especially if I know there will be some signal difference between them. This gives me some comfort in knowing that I've established at least some layer of separation between them, even if it's just in one direction. Not everyone does it this way, and to each their own. This is just how I route traces if at all possible. Take a look at your resistor footprints, you can add some separation by using footprints with 7.62mm pad spacing rather than what you're using now. That'd give you a little more space on the board.
Without knowing any cap values, I can't tell you whether or not the footprints will work. Based on the circuit, I'd assume that film caps C1-C3 would all be < 330nF caps, so you're probably okay with those. As soon as you get any higher than that in capacitance, the width starts climbing, at least in box film caps. If you're planning to use a 1µF box film cap for C5, the footprint is probably too small. There's very little wiggle room around your components, so if you get the sizing wrong, it may be difficult to assemble the board.
Thoughtful component placement is one of, if not the most important characteristic to a good layout. Your input signal flows directly beneath the output signal. You're amplifying signal in this design and by having your high impedance signal (input) running directly beneath your output, you're increasing the likelihood of oscillation. Add as much separation between IN and OUT traces as possible to lessen the chances of oscillation.
I hope at least some of this was helpful and that I wasn't rambling for no reason.
.
.
