Big Monk
Well-known member
You have to question the sanity of someone who WANTS to solder a metric fuckload of TH components to a board.
The fun is in the design and the playing!
Bring out yer Diptrace
- Thread starter Grubb
- Start date
You have to question the sanity of someone who WANTS to solder a metric fuckload of TH components to a board.
The fun is in the design and the playing!
Nostradoomus
Well-known member
It can be kinda meditative (if you have all your ducks in a row component wise 
), I really don’t mind it.
), I really don’t mind it.
PedalBuilder
Well-known member
Definitely takes all the fun out of it. Plus there are diminishing returns going from ±0.5% to ±0.05%. But an interesting idea for future use for sure.
pingpongcomputer
Well-known member
I just got diptrace and finished my first "original" design, it's cobbled together from online schematics that I've fooled around with on the breadboard for the last 2 weeks, anyway, please point out any glaring errors you see in the schematic. I ran the electrical rule check and corrected the errors it found, connections I thought I had made but didn't, but I'm not sure I have the switch pads all done correctly, or anything else from that matter. Please and thank you!
PedalBuilder
Well-known member
Congrats on making the leap! A few thoughts/questions:
- I'd recommend changing the polarity protection diode to a series diode, rather than the parallel diode to ground. A series diode is more reliable.
- I'm not sure if I'm reading the symbols correctly, but it also looks like your indicator LED is not connected to a switch pad and will always be on.
- Does the box with "IN G 9v OUT" represents four pads for wiring the footswitch? If so, you'll probably want to remove the 9v pad and replace it with a switch pad that connects to the cathode of the indicator LED.
- The clipping LEDs look questionable to me. A single transistor into a tonestack seems unlikely to produce a hot enough signal to reach the clipping threshold of the LEDs. I'd recommend moving them after the 1uF capacitor that follows the second transistor. you have a hot enough signal to clip the red clipping LEDs?
- What is the -9V(T) net? It looks like it's the same as ground.
- What is the difference between GND and GND(T)?
- Which potentiometers are external controls? Which ones are internal trimmers?
Last edited:
pingpongcomputer
Well-known member
Thanks for all the tips, I definitely need to rework the power supply section.
The clipping LEDs occasionally pulse while I'm playing, so I assume they're working? They're just there to prevent hard clipping from the jfets.
-9V(T) is the pad for the negative connection from the DC jack, I wasn't sure how to represent connecting it to ground, so that's what I came up with.
GND is ground reference and GND(T) is the pad for connecting to jack ground, so that was just showing all of that hooked up. Maybe I'll try to find some example schematics where everything is shown, usually that stuff seems to be omitted. I do have everything labeled on the schematic, but turned off refdes and justed showed values for the print image because it wouldn't all fit, but I realize now it would've been more helpful to leave the labels on and the values off. Thanks again, I'll get back to work on this tomorrow!
PedalBuilder
Well-known member
It’s possible that there is DC that’s making them blink. Try putting a large capacitor between them and the rest of the signal path and see if they still pulse.
Gotcha. I use V- or DC- for that pad on my schematics. It might be worth changing the name because the negative connection is 0v, not -9v.
I’d recommend keeping both refdes and values in your schematics. It’s difficult to discuss the schematic without refuses, and it’s hard to know what the circuit is doing without values. Check out the schematics that I’ve posted (or the schematics in the PedalPCB build docs, for that matter) for examples of schematics that include both.
Silver Blues
Well-known member
Runoffgroove is doing this in several of their circuits as well. The DC check suggested above is a good idea, but if you're not after the clipping character of the LEDs, I wouldn't recommend moving them. It also might be worth just keeping them in case you want to put a booster or something ahead of this circuit that might change the character.
pingpongcomputer
Well-known member
Feeling real dumb, -9V on one side and +9V on the other wouldn't be a 9V power supply. I wasn't thinking, just trying to fit things from the supply pins category of the rullywow library into the schematic for the pads I knew I needed for connections on the board. Many thanks, I also forgot I had one of your schematics to use for reference, that will be very helpful. I obviously need to do some more research.
That part of the circuit is modified from part of a ROG circuit, that's why it looks familiar, and I plan to keep the clipping sections for exactly that reason, since I'm a fan of gain stacking.
Thanks very much @PedalBuilder and @Silver Blues , I'll be begging for help again soon with a pcb layout review and will hopefully include all relevant information.
pingpongcomputer
Well-known member
Ok, well I got sick and the circuit went through about 10 more iterations, but I got way better at diptrace schematic drawing, and schematics in general. Here's my first PCB attempt, from what I've read I think I should do a copper pour on the top layer too, but I left it off here so you can see all the traces. Almost everything is on the top layer except for a few stretches that couldn't be made and the ground pour. Hopefully the color scheme is high contrast enough for everything to be visible. Any critiques are appreciated.
Edit: I already want to change the transistor labels to Q1, Q2, etc rather than the type.
Edit: I already want to change the transistor labels to Q1, Q2, etc rather than the type.
Brett
Well-known member
Can you take a snap shot of the board showing your ref des and share it here?
I see at least one trace that can be shortened significantly but telling you it's the 470pF capacitor does less for you than telling you it's C3.
Your 1µF capacitor footprint at the top is a bit too small if you're planning on using a film box cap.
Make sure you use thermal reliefs on your ground pours, otherwise, you'll struggle soldering them.
Your round solder pads at the bottom could probably use an increase to the annular width, otherwise, they may be difficult to solder.
This is just on a quick glance. Share the ref des when you get a chance so we can take a look.
pingpongcomputer
Well-known member
Thanks very much, I think I fixed everything you outlined except didn't see the path to be shortened, but I'm still heavily under the influence of dayquil. I used 4 spoke thermals without doing any research, I'm guessing there are some sort of guidelines for what to use when if I do a little googling. I just copied the width of the pads for the resistors for the 3dpt connection solder pads, with 1.1mm holes, now that I'm looking at it maybe I want to bump up the pad width a little more.
Here's the revised layout with refdes:
derevaun
Well-known member
I'd check the C17 traces against the schematic--if it had you follow a ratsnest line, there could be an incorrect connection.
The G2 pad takes a long and convoluted path to the ground pad at the top, including passing through R1's thermals. I like to evaluate the ground pour after every trace I put on that layer, making sure it's a pretty solid path to the primary ground pin. Vias can help a lot with keeping traces short on a pour layer.
The G2 pad takes a long and convoluted path to the ground pad at the top, including passing through R1's thermals. I like to evaluate the ground pour after every trace I put on that layer, making sure it's a pretty solid path to the primary ground pin. Vias can help a lot with keeping traces short on a pour layer.
pingpongcomputer
Well-known member
Thank you! Man, I made one last minute addition and two part swaps on the schematic before converting it to PCB and totally wrecked my connections in the boost circuit. Still passed all the verifications because they were connected to something, but not the right things. I would not have caught that looking at the PCB. I'm going to stop now and re-check everything tomorrow, thanks for saving me from wasting my first trial run.
pingpongcomputer
Well-known member
yep, that was part of the tornado of destruction I made adding one resistor and swapping 2 patterns.
szukalski
Well-known member
@pingpongcomputer your audio path should be as short as practically possible and avoid crossing over itself where you can.
Your input and output traces overlap each other, albeit on different layers. This could bring oscillation, especially in higher gain applications.
Your input and output traces overlap each other, albeit on different layers. This could bring oscillation, especially in higher gain applications.
Brett
Well-known member
I've designed and verified several boards successfully, but I have no formal education in PCB design, so take my suggestions at face value.
Referencing this post:
If your nets are connected correctly per the schematic, this trace is much longer than it needs to be:
To piggyback on what @derevaun said, your ground pour isn't ideal for the G2 pad. You also need to be sure to remove copper islands, otherwise, you may inadvertently create more noise in your circuit. Areas in green are connected. The uncolored portions are islands:
The component placement could be optimized in several cases. Like @szukalski mentioned, you want to keep traces as short as possible and keep traces carrying your input as far away from traces carrying output as possible. Even on opposite sides of the board, if in/out traces run parallel in close proximity, you're inviting potential problems.
Referencing this post:
If your nets are connected correctly per the schematic, this trace is much longer than it needs to be:
To piggyback on what @derevaun said, your ground pour isn't ideal for the G2 pad. You also need to be sure to remove copper islands, otherwise, you may inadvertently create more noise in your circuit. Areas in green are connected. The uncolored portions are islands:
The component placement could be optimized in several cases. Like @szukalski mentioned, you want to keep traces as short as possible and keep traces carrying your input as far away from traces carrying output as possible. Even on opposite sides of the board, if in/out traces run parallel in close proximity, you're inviting potential problems.
