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.
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.
My newb 2 cents is that I had two versions of a board made recently, one with the best I could do, but still not optimally placed 9V routed trace with ground pours on both sides, and another with a 9V pour on the component side and ground pour on the reverse and then nicer/shorter routing for signal traces. It's a pretty high gain design, but the power pour version was much noisier with the gain/volume turned up.
With a layout redesign, it's difficult to say that the copper pours were the most significant contributor. If your design was high-gain and your high-impedance path was in close proximity to any amplified signal on the board, especially later stages, short traces aren't going to save the day. I'd be curious to see both layouts you did to see the differences.
Clean layout! I like the "flexible" resistor footprints. If you don't mind sharing, how are you handling the relay bypass? I see an SOIC-6 footprint, is that being used as the relay controller?
With a layout redesign, it's difficult to say that the copper pours were the most significant contributor. If your design was high-gain and your high-impedance path was in close proximity to any amplified signal on the board, especially later stages, short traces aren't going to save the day. I'd be curious to see both layouts you did to see the differences.
All I have left are the actual PCBs. I was in the habit of overwriting the layouts when I updated them. I'm saving independent versions now so I can look back at what I did. But yes, it was very much not a scientific test, lots of variables.
I've come back to this thread like a proud grandfather. Didn't expect it to still be rolling 2 and half years later! I love seeing the stuff some of you guys are making.
Quick question - any advice before I tackle my first stacked PCB design? I'm working on a designing a custom modded Univibe for someone and I'm going to need to stack PCBs to make it work with the pedal format I've chosen. I haven't even assembled a PedalPCB stacked design before so I'm flying a bit blind here trying to design one. I'd be keen to hear any lessons you've learned about PCB stacking.
Thanks so much, @Brett, your advice was really helpful! I finally got a chance to rework everything based on what you said. I figured I'd keep the separate schematic sheets since it seems like a good habit for larger circuits. I added values to the schematic (for the standard Meathead variant), ending up removing the LED and putting the diode in series:
And I reworked the PCB. I wasn't 100% sure what you meant about not doing a copper pour (I removed the power fill and moved the ground pours to the sides, like a breadboard). I tried to keep power to the top/right of the board, and then then input along the left. A big help in simplifying the layout process was adding separate colors for the different nets (via the appearance pane). This layout at least looks cleaner to me.
Great that you added values. Removing the CLR, LED, and using the SW pad may have been a mistake, if you plan to use the SW pad like most projects do. If you ground your SW in this configuration, you're going to short your power supply. You'd want to come off of your 9V pad with a CLR with the LED in series (anode facing CLR), then the SW pad.
And I reworked the PCB. I wasn't 100% sure what you meant about not doing a copper pour (I removed the power fill and moved the ground pours to the sides, like a breadboard). I tried to keep power to the top/right of the board, and then then input along the left.
You could just make the ground pour on the back cover the entire board in one polygon rather than separate rails and traces going to either. The way you have it now won't give you much benefit and may increase your resistance to ground in some areas.
It does look like you've given things a little more room, just be careful with the trace running from C1 to C2 that passes beneath C5 and the trace running from R5 to C5. C5 carries the most amplified signal in the circuit. You may want to try to rearrange those caps or make sure you have ample space between any copper (traces or pads) connecting those nets.
Ah, I misunderstood your previous post. I thought you were saying that pours for power or ground were bad. But it sounds like you were just saying power, or power and ground together.
I had just enough room for the LED and resistor in the corner, so I've added those back in.
Thanks for the advice on the C5 capacitor. I tweaked the layout and now there's more space between C2 and C5.
Out of curiosity, is there any way to test or "score" these layouts for the kind of interference you're referring to? Or are there any guides you'd recommend? What's killing me is that right now it seems I'd have to learn all this by experience, but "experience" takes at least 2 weeks of JLC build+shipping+build on my end, before I figure out if I messed up - and even then I'm just as likely to attribute it to a noisy circuit rather than my own poor layout (or if I attribute it to my layout, I might not know what's causing the problem). As an example, I'm not sure how I'd begin to assess the impact of moving or flipping C5 (below), to avoid routing a trace under the capacitor itself and to put the trace next to it. Perhaps there's no impact, or perhaps it adds a lot of noise...
Most of the calculators I’ve seen for stuff like this are more focused on signals with far higher frequencies or much larger currents than we deal with in pedal building. I would be very interested to know too if I’ve missed calculators that would apply! Douglas Self covers some of this in Small Signal Audio Design but a lot of it is open ended
I don't think there's an all-in-one type tool to do this in KiCad, or at least I haven't seen one. If you understand the schematic and can identify nets that are susceptible to crosstalk, high-impedance sources for example, you can use the Inspect > Net Inspector for insights into how long the traces are on that net. Long traces can act like antenna, so this tool gives you *some* insight, but it's not conclusively going to tell you if you did something wrong. Another tool that may give you some insight is the Parasitics add-on (available on the plugins menu). I've never used it or downloaded it, but it appears to measure trace parameters to give you data that may assist in reducing potential crosstalk.
I'm certain that more knowledgeable PCB engineers use software that can provide some quantitative measurement of potential issues between traces, but alas, I am not one of them. I do this because I enjoy it and the majority of my learning has been through practice and the school of hard knocks. We are designing low-level analog signal circuit boards and from what I've learned so far, these designs are pretty forgiving as long as you take basic precautions when doing a layout (most of which I've already mentioned).
I've only done one of these so far, but I can share a few things I took into consideration when doing the layout:
1. 7mm capacitor height is about the max I could use with the headers and standoff I used. I had to make sure that any electrolytic capacitors used the correct diameter footprint and pad spacing because low profile sometimes means a different footprint. I used Kemet ESS series caps on my build. If you're interested in looking at those, here's the datasheet.
2. I tried to strategically place components on the top board so that the pads for the components did not overlap any electrolytic capacitors on the bottom board. I didn't want to accidentally puncture any of my electrolytic capacitors when I sandwiched the boards together.
3. When I did the layout in KiCad, I actually designed both boards on the same "Master" project so I could ensure the alignment of the boards and standoffs was correct. I then duplicated the project twice and had one project for the top board and one for the bottom before generating gerbers to send to the fabricator. Doing this gave me all sorts of DRC errors (which I could have fixed), but I knew the design was DRC-compliant in the Master project before splitting things up.
4. One advantage to stacked boards is the opportunity to isolate parts of the circuit that may not interact well with others. For example, having the power supply and LFO to one board and the audio on the other. If you're mindful with your headers, you could also create a sudo star ground between the different parts of the circuit and the voltage input source.
5. Another consideration that relates to isolation of conflicting circuits in the overall design is which side of the board your traces are on. For example, if you place your LFO and power on the bottom board and route the traces on the bottom of the bottom board and your audio circuitry on the top board with top layer traces, you could have two layers of ground separation between them. It's just something to consider.
If you have any specific questions that you think I might be able to help with, feel free to tag me and I'll help the best I can .
Here's a snapshot of the boards I designed for the MOS-TRON Envelope Filter project I did in case you'd like to see them:
A few pictures showing the stacked boards can be seen in the build report I posted for the project as well.
.
.
