Burns Buzzaround PCB- Can you all review and critique?

Synchrony Pedalworks

Synchrony Pedalworks

Well-known member
I am new at the PCB design (in otherwords, I have never done it), and was wanting to expand my abilities. I was hoping that some of the guru's could critique these PCBs and give me some tips. I used the PedalPCB schematic and layout for the Burns Buzzaround (@Robert - If it is not ok to do this, let me know and I not use it). I added 3 resistors across the base and collectors to simulate leakage (I have a bunch of Russian transistors). I also have a board for a foot switch for a charge pump to get -9V power. This board is for a different project. I am using EasyEDA, due to it being linked with JLCPCB and The Tone Geek used it for his tutorial. I did a copper pour for both layers, but I don't know if that is needed or appropriate. I also did an auto routing for the traces. For future PCBs, I was going to run the traces myself, but with this project, I wanted to make sure that I could make a board that worked.

Below are pictures of the boards and schematic. If I need to post different information, please let me know. Thanks in advance!

TOP Layer:
1749251327975.png

Bottom layer:
1749251919609.png

1749251399342.png

Top layer
1749251514887.png
Bottom Layer
1749251969343.png
 
My only comment is that some of the wires and vias are very close together. Maybe adjust the settings in the design rule to make the clearance a bit more. Perhaps 0.15 to 0.25mm.

Is your copper pour connected to any nets? It doesn't seem to be. Or if it is connected to ground, you have wires connecting ground as well which is redundant. I often do a ground pour for both layers and I find that it makes circuits a bit more quiet.

When autorouting, try skipping the ground net, then do a pour with the copper area as GND.
 
Paths and vias unnecessarily so close to the pads. You have plenty of free space available.
 

Attachments

  • 1749286602452.png
    1749286602452.png
    281 KB · Views: 11
  • You don't need to route ground traces if you are using a ground plane.
  • Auto-routing is ass. You will end up with the mess you have here. You do you, it'll probably work but auto tracing isn't thinking about a good audio path.. Look at the trace from volume to the output pad. It's going right through Q2. Oscillation may be knocking at your door.
  • You started copying Robo's layout, but then deviated and made some changes. Generally, the placement will be due to routing considerations (and some aesthetic) so you're introducing routing requirements which may not be beneficial.
My general recommendation for getting into layouts is the same for building, start small. A nice boost or Rangemaster type thing. Get used to the process and learn how to route effectively (audio path > power).
 
@Synchrony Pedalworks - you have to reverse the polarity of the C101 capacitor. Also - there's no filtering cap connected to 9V - (pins 1 and 8 of the charge pump). You have C101 on the negative rail, but no el cap on the positive rail.
Another issue - potentiometer footprint overlaps with solder pads of the potentniometer above. They're too close.

One more: marked area. Does not make any sense now. Positive supply connected to anode and cathode of the D101.
Should be - positive (PWR) to LED and Anode of the D101 only. Cathode to 1 and 8 of the charge pump. As on the schematic.
1749299779559.png
Probably because of the 9V label on both sides of the D101. Remove one label or change right one to Vcc+ for example.

1749300099694.png
 
Last edited:
Synchrony Pedalworks said:
@neiltheseal , @temol , and @szukalski - these are great suggestions. Thanks! Let me go back and give it a try without the auto routing and see if that cleans it up. @neiltheseal - your comment about the ground pour helps clear up my confusion, so thanks!
Click to expand...
If you are doing it without autoroute, try hiding the GND net. That will make it easier to focus on what you really need to connect, if you are doing a ground pour at the end.
 
You have taken on a rather difficult task for a beginner - the layout should be nice. I would rather try to follow the schematic, of course trying to maintain "elegance". Now you have a lot of long traces, which can be easily avoided by moving some elements.
 
@temol, @szukalski, and @neiltheseal - Thanks again for all the help. These comments are really helpful, and I am starting to see the picture more clearly. I recognize that the project is probably more ambitious, but I was going to give it a go for a couple more attempts. Let me know your thoughts. I made several changes...
  • Moved several components to reduce the length of routes
  • Renamed the 9V to VCC+
  • Changed polarity of C101
  • Copper pours on the top and bottom layers for ground
1749395116657.png

1749395272857.png
 
There's still something wrong around diode. Routing should look like this

1749396871258.png 1749396947668.png

It looks like you don't need to use the Vcc+ flag at all. Because pins 1 and 8 of the charge pump are not connected anywhere (except diode). You only use -9V. So the 9V flag is only on the anode side of the diode. On the cathode side there is no flag. Show current schematic.
 
You must log in or register to reply here.
Back
Top