You can always flip and rotate a symbol.
3 Likes
Ah, a simple rotation… why always the simple things XD
Thank you again 
EDIT: Added filter and the Soft/Hard sync and FM, with help from @Caustic 
3 Likes
Personally I would also suggest adding the octave selection, really very practical
On my VCOs that don’t have it I miss it a lot
R42 must be changed, i don’t remember exactely maybe 2K (i ll searched and come back 
)
EDIT : I found it, between 1K and 4.7K
(By the way, R42 shown there is specified as 220 ohms but it really should be higher; 220R results in too much current through the voltage reference U4, potentially causing bad behavior and possibly damaging U4 permanently. If you used 220R this would be a good time to replace it with something between 1k and 4.7k. For more on this and other mods see 1222 Tuner VCO Module - #203 by antoine.pasde2 and 1222 Tuner VCO Module fixes/improvements - #6 by eric .)
3 Likes
I really appreciate that advice! I saw that earlier and was in the middle of a video so couldn’t respond. I am not sure how to implement this into the schematic I’ve got already…
Is this part of the performance version? If so, I didn’t look at that one, I was looking at the simple 3340 and just added the extra bits that were omitted, added some filtering / decoupling
Like nothing really extra, just trying to get a workable file so I can etch this, rather than perf board like my last one, or stripboard. I’m rather fond of how my last etching project turned out so I wanted to do it again
2 Likes
Okay, so I worked on a pcb design and got the rats nest sorted… it’s a messy boi but dang it, I’m gonna try it and see, the only obvious thing wrong is 2 resistors, I forgot to hide the reference and change the value to F.SilkScreen, so there are 2 resistors that show R1(100k) and R6(1.8k) [This has been fixed, next step is optimization]… otherwise they’re on order and I’ll post updates here as to how it goes! If I can get this board sorted, then boom, another kicad file to add to the community
My first ever from scratch in kicad too, so… idk maybe it’s not 100% s*** rofl
(also need to shrink it’s size and other optimizations of course)
4 Likes
I would put the reference on the silk layer. It makes the board so much easier to debug.
You can do this easily for every resistor by making a custom library with a custom resistor footprint that has both the value and the ref on the silkscreen layer. I can walk you through this tomorrow evening if you like.
5 Likes
AMEN
As someone on here pointed out, you want the values when you build and you want the references when you troubleshoot, so for resistors it makes sense to put he value in the box and the reference outside.
My custom footprints also set the silkscreen text size to 0.75 mm because having values and references both on the silkscreen can get crowded…
Suggestion for your power header: Label the orientation! I always use 10 pins so have a footprint that says +12V on one end and -12V RED STRIPE on the other. And shows the box header orientation notch.
7 Likes
Hey thanks for the information guys!
Yeah I kinda thought about that a little too late 
I got in a rush and ordered the prototype a bit too fast. But what I can do is fix it and it’ll be good for next time.
That’s a good idea, my reference is a square pad for -12v, other than that, it’s not labeled… oof…
Like copying the components I use into a custom library and setting the global to be ref/value both as silk screen? (I’m just using logic and guessing here…)
If the prototype works as intended ( can’t see why not ), then I’d like to shrink it down and round out the corners and such, make it pretty basically. But I left it bigger so I could diagnose it if something isn’t working…
Anyway, cheers you guys for being so kind and trying to help this noob out 
EDIT: I managed to find it! Holy crap
Granted, I’ve got to remove the duplicate stuff, but otherwise that worked a charm
3 Likes
booom!!!
ahhhhh now to shrink it down and round it out, beautify it ((And add the power reference that I forgot again…))
EDIT:
EDIT 2:
Fixed more of the text, re-oriented the pot text (was wonky before and hidden) and added Tip and Sleeve reference text for help since it’ll be wired for the prototype
EDIT 3:
Removed the ground traces and replaced for ground plane
6 Likes
Okay, so unless something is wrong EDIT: There is something wrong… found a few things on the schematic that went unnoticed with the help of discord and a friend there by the name of Tarn, spotted a problem which led to spotting a few other mistakes (junctions that weren’t suppose to be there), so there is problems already, JUST A HEADS UP
I realize it isn’t perfect btw, but hey, I hope this helps someone else 
If something is wrong though, then of course here are the files and everything so far.
4 Likes
You have at least one unrouted connection:
This would appear to be an unconnected island in the ground plane. If you shift this diagonal trace
down or to the right it might open up a connection to the connected island to the lower left.
You spoke of etching so I expected a single sided board, but you have traces on both sides. Or are the red traces all going to be wires? If not, and you really are going double sided, then a ground plane on the red side would very likely fix your island, too.
Also, preferences vary, but for power rails and other relatively high current traces, I like to use a 0.75 mm wide trace vs. the 0.25 mm I use otherwise. Look into net classes, that’ll help automate that.
4 Likes
Yes and there were some schematic problems that I overlooked too… here I’ve fixed those issues that I could find, I haven’t increased the trace width for the power, but there again, I’ve reached mental limit again (hate that so much because it’s causing blunders and goofs ><)
EDIT:
Okay, I managed to get rid of the rats nest by switched the ground plane to the front as you suggested @analogoutput
I was going to etch it, but it’s overwhelming as it is, so I’m just trying to trudge ahead and keep on going.
Rerouted it and it seems okay now, so I’ve uploaded a 3.3 here:
4 Likes
I meant adding a ground plane on the front in addition to the back…
3 Likes
I didn’t think of that… omggggggg
I’d cry, but it’d probably short out my keyboard XD
Both layers with ground planes:
EDIT:
Fixed where I forgot to update the zip file to include mounting holes and a few other things that I ran out of steam on last night. I changed the title to include proto because I ordered the prototype of this one since I know the first one won’t work (due to the problems mentioned here and discord)
2 Likes
There’s even a shortcut for it. Create a ground plane, select it, and choose “Zones > Duplicate zone onto layer” (I think it’s called). That allows you to make a zone with the same dimensions on the other side.
4 Likes
Thank you for all your help! I hope I’m not being a pain.
I am converting this from a picture of a stripboard, I think having less than 12 hours experience in kicad has been the tedious part to staying positive and pushing through…
I say this to emphasize how grateful I am that you all have taken the time to be kind and educate me rather than belittle (has happened, though not here or the synth community thankfully )
It doesn’t show the rounded corners, but here’s their “Preview”
4 Likes
It should show the rounded corners. Try uploading the gerbers to tracespace.io .
If they don’t show there then you have a problem with your edge cuts layer. Have you run DRC?
2 Likes
I did, but the preview isn’t kicad preview, it’s from a company who screwed me so I didn’t want to say their name >.>
But PCBway’s preview is not the same
I downloaded the zip file from the order so that I could check it against kicad and it shows up fine in kicad, as do the mounting holes. No idea why they do that… that’s stressful because all this crap after ordering… anyway… hopefully it’s okay when it gets here.
This is only a prototype, so I mean it should be considered untested and should be used with caution until after it gets here and I’ve had time to test it.
If there’s nothing wrong, then the only real difference between the order and the file I’ve got on hand is taking off “AS” from the 3340 footprint text, adding “v3.5” below the description text to reference the file and that’s about it for now.
I mean obviously there’s a lot of improves and could optimize this all day, but as this is just something I wanted to complete so I could use the chips I’ve got on hand, I didn’t want to spend all the time optimizing, but no time testing. So… Idk, call it a WIP for now I’d say. But it’s definitely further than it was a few days ago as a simple picture XD
EDIT:
Did some major cleanup and shrunk it to 70x99mm
Fixed the electrolytic to the right footprint, changed the jack sockets to a header for the wires, cleaned all the stuff up to make it fit within 70x99mm
Basically trying to make the final version look nicer (if the prototype works)
3 Likes
So to update here, I’ve been going over this board with as fine a tooth comb as I could.
I’ve run across a few problems and I’m going to list them here, I haven’t culminated everything into a comprehensive whole yet, so please forgive me on the constant updates.
So for starters, the design is now on v4.1, and to explain why:
Up until v4.0, I had used freerouter, which worked fine enough, but it’s flawed but I used it to take some of the mental load off of me (the rats nest) until I could work out some other problems.
Notably:
- RV4 was suppose to be 10k, not 100k - I’ve fixed that both in the schematic and on the silk screen
- Text was a bit wonky here and there, that’s now sorted and everything has been reduced to .75mm
- There was one other thing that made this board expensive to prototype is that it exceeded 100mm on 1 side, so it has been compressed to fit 70x99mm (I’m proud of that part XD)
Which brings me to v4.1:
- Organized the schematic to look nicer
- Fixed the silkscreen to include the revision number on the board itself, to separate it from any possible previous versions
- I’ve manually routed the traces and vias, which was fun actually. all traces are now at least .5mm unless it auto shrunk on the angles, which I did notice happened. But as I ran the power traces first, I don’t think it did it to those, did not check that.
- I’ve also included silk screen text to label the in/out pins for the jack sockets so there’s no confusion as to what pins do what
- Basically I’ve nitpicked until my brain couldn’t find anything worth nitpicking anymore
And last thing is, I’ve ordered this as a prototype in black (hey, it’s $2, cost me $14, why not)
At this point, there’s nothing more I want to do to this board personally, not unless it doesn’t work, if that’s the case then I’ll fix it and just update this post, but I’m trying not to spam or post too much as well, so I’ve been trying to keep that edit button in mind as well.
As of now and here are the files/pictures related to that to keep you guys up to date.
(30/11/2021 5pm as of posting)
I would wait to use any of these files and let me be the one to blow something up, as I would rather take the blame if something doesn’t work, than say this is ready to use.
It is stiil a prototype but I wanted to share the progress as I never found any files already made like this.
EDIT!: I just found a single connection that wasn’t made (It’s not a huge deal, just bridge it) I wanted to point out [ This also goes for the -12v ]:
Edit2… I still managed to miss this ground plane not being connected through to the other side, it’s not everywhere, just the top right pair flagged, so I just added vias for later… but for the prototype, I’m going to just bridge those with a wire.:
Current status: Untested Prototype
4 Likes
IT WORKS!!!
Just had a great time jamming on it!
Includes the v5 and the jackies/knobbies boards in the zip file, read_mile file and everything is included!
The only difference between the board I tested, and the board in the files is that I fixed the through-holes for the panel mount 3.5mm sockets and other tid bits, but it’s all here in the read_me.txt if you want to know how much I put into this board.
Tested: Working!
EDIT: Be sure to check the distance between the 16-pin headers, this version has the possiblity of being too close together depending on the 16-pin header you use.
Thought it was worth mentioning
9 Likes