It should auto fill every time you export Gerbers, unless you have that option turned off. It’s a checkbox in the Gerber export window somewhere.
2 Likes
WOW 
I will be coming back to this post frequently.
this one has me the most cautious since the two boards face the opposite direction. both with the alignment of connectors as well as the pin placement. rotated these 3d objects in my mind palace a thousand times but won’t feel confident until i witness it actually working.
3 Likes
To check alignment you could always plot and overlay the two images in photoshop / image editing software of choice. This can always be done on paper overlayed and held up to a light or window, (old school cad technician trick)
For refilling zones, there is a checkbox in kicad DRC checking dialog box.
3 Likes
I use a trimmed down version of this:
2 Likes
It’s a classic… I think there’s some of that kind of nonsense in the litany of dumbarsery thread…
4 Likes
I am aware of footprints for pots with both orientations, 1 2 3 , and 3 2 1, and it has caught many of us out. I can remember @analogoutput making a post about this comparing the many kicad footprints, you have to match the pins in your schematic to the layout of the footprint.
Am I correct in thinking you are planning on installing your components on the same side of the pcb as the hardware? If so, have you checked the height of all the components. I have noticed some vertically mounted resistors that could be very tight. I have included a photo of a thonk conn, with a resistor from my stash to demonstrate. This may not be an issue if you source small resistors.
It would also appear you may have some missing connections as indicated by the remaining rats nest lines, These may well be connected via the pin headers but is something I would recheck.
The footprint you have selected for the transistors is very fiddley to solder, a wide version is in the standard kicad library.
I have also just noticed R49 & D10, and R47 & D12 may be transposed, I think this is just the labels.
2 Likes
See
and the subsequent two posts. I always use my variant of the Alpha footprint. This I why I said
So could the electrolytic capacitors — of which I see zero. Really? No 10uF bypass caps near the power header? No 10R resistors or Schottky diodes on the rails either — well, that’s a choice and if you’re confident there will be no shorts and no power reversal that’s fine. But the 10uF caps are really recommended — mounted horizontally if they’re between the boards or board and panel.
They look like +12V and ground. I do see what looks like a header connection for +12V, it’s not obvious to me there’s a header connection for ground, though.
These kinds of leftover ratsnest lines, and the consequent nonzero unrouted count, bug me, so I use GND1 on one board, and I created power symbols +12V_1 and -12V_1, to make totally separate ratsnests for separate boards.
Hear hear. I still let the tight footprint through sometimes by accident and kick myself. Though I haven’t actually had trouble soldering one since one of my first PCBs when I went through about three pairs of transistors soldering and unsoldering until I got it without issues.
Here
you could avoid some very convoluted routing by putting some traces on the other side. Not really a problem, more an aesthetic thing. I also would connect C11 directly to pin 16 via a single straight trace but that’s probably fine. And I’d use wider traces for the power rail, as you did on the other board.
4 Likes
Thanks. As of the last two posts, I now know to use alternate power lines. These bug me too to no end and thought based off of an answer I got on Reddit to just ignore these. The other thing that bothers me is that the circles on the mouse bites register as silk screen points that I want to get rid of.
Good to know thank you. the pins on my transistors are really close together.
Finding out crucial last minute information like this is basically the only way I learn 
. This will definitely be accounted for. First module I’ve ever ‘designed’.
Where should I place the Schottkys in this case? near the bypass caps?
Also, this brings up something I forgot along the way too. My inputs are exactly these:
Are these sufficient to protect the MCU from accidental input voltage or should I add Schottkys here as well? I mean, I guess reverse polarity is to be expected on the CV input. My gate input is one you’ve posted here, @analogoutput, so I know that’s good 
1 Like
I don’t know what OP1 is or what its power voltages are. I assume it’s your TL074 with ±12 V power in which case it’s fine. If it’s an MCP6004 with +3.3 V and ground then the + input needs to be protected (but then you can’t get -4.95 to +5.55 V so presumably not, but if so:). For MCP600x the datasheet says under Absolute Maximum Ratings:
Analog Inputs (VIN+, VIN-)†† … V SS – 1.0V to VDD + 1.0V
so in this case the voltages on the input pins should not be outside the range -1 V to +4.3 V. Assuming Vin comes from a jack where potentially ±12 V could be connected, protection is needed.
For the second input. if CM is always 1.65 V that’s all right, after the voltage divider it would be 1.65 * 100k/133k = 1.24 V.
As for the - input: Given infinite voltages on the rails, it will be the same 1.24 V. And then V_O, the output voltage on the op amp, will be 1.24(1+33k/100k) - V_I(33k/100k) where V_I is the voltage on the jack. But if V_I = 12 V then V_O is -2.31 V and if V_I = -12 V then V_O = 5.6 V. Both of these are outside the limits of the power rails, so in those cases the voltage on the - input cannot be 1.24 V. In fact it will be V_I + (V_O-V_I)(100k/133k). With V_I = 12 V, V_O can’t go lower than 0 V in which case the - input is at 2.98 V and with V_I = -12 V, V_O can’t go higher than 3.3 V and the - input is at -0.5 V. Those limits are safe, so no overvoltage protection needed there.
2 Likes
d’oh.
You’re correct, and I carelessly said “inputs” where the top schematic is the output 
. The 3.3v comes directly from the MCU and comes out as roughly ±5v.
I need to get the math fundamentals down so badly though. So far it’s all been empirical, which is wasting a lot of time in reality. I found these circuits on the Axoloti forum and tested them (only) with the appropriate application, so I know they work on that front at least!
There should be a series 1k resistor between the op amp and output jack. With that there it should be all right.
2 Likes
Horizontal-ized most of the resistors
Added bypass caps and parallel schottkys (above power connector)
Changed to larger transistor footprint
Reversed pot pin placement (created custom library with reversed footprint)
All power lines should be .75mm now
made separate ground and 3.3v lines for top and bottom boards
“silkscreen clipped by solder mask:” Line on edge cuts and arc on silkscreen. Not really sure about this one. When I first tried to do the mouse bites I knew I screwed up because the 3d view didn’t show a gap. It looks fine in 3D view now, so I’m going to assume it’s okay.
Assuming that the two errors don’t break the CNC machine at the PCB place (in which case I apologize to everyone here ahead of time), I think it’s ready as it will ever be… wish me luck…
3 Likes
Good luck 
looks good.
I see you have gone for parallel protection diodes, and this does protect your module, but it relies on somewhere else in the system to then handle the shorting of the power rails. This somewhere else is your power supply, or if that has no protection the ribbon cable. I have seen this done on a few modules. It is also common to put them in series, this does give a 0.3v drop on each power rail if using 1N5817’s so I always breadboard with these to check no issues are caused. Most use 10ohm resistors in series, while they give little reverse polarity protection, they do act as sacrificial components in case of unexpected power usage like a short. Maybe something to consider for any future designs.
Please keep us informed of your progress, it’s nice to see new designs come to life in the community.
2 Likes
Another issue is that this appears to be a Eurorack, not Kosmo board 
4 Likes
I know right. I don’t even own any bought euro modules/plan to buy any/can afford any. However I opted for the format due to very limited space in my tiny apartment and no woodworking skills to make a case. I 3d print out my little euro ‘cases’ in 2 pieces and use a module that spans both halves to keep the pieces together.
Visually I think Kosmo is a cooler format. I agree with Moritz that it is ‘large and imposing’.
3 Likes
you’re telling me i gotta solder stuff into this too?!
jk, still untested but I’m just gonna stare at these for a while.
thanks again for all the help everyone!
8 Likes
Looks awesome, cool logo!
3 Likes
thank you!!! 
made it a while ago on a whim and I’m pumped to see it on a real-life thing.
2 Likes
I need to get some sort of logo going for my PCB designs. I tried getting some of my sand art (like the snake in my profile picture) onto a monochrome image but there’s not much contrast to use. Just sand and… More sand.
3 Likes