MUFF WIGGLER Forum Index
 FAQ & Terms of UseFAQ & Terms Of Use   Wiggler RadioMW Radio   Muff Wiggler TwitterTwitter   Support the site @ PatreonPatreon 
 SearchSearch   RegisterSign up   Log inLog in 
WIGGLING 'LITE' IN GUEST MODE

My 1st PCB!
MUFF WIGGLER Forum Index -> Music Tech DIY  
Author My 1st PCB!
l3v3l6
I just received 10 prototypes from JLCPCB of the first PCB I've ever designed. It's a 3340 VCO, designed with no particular form factor using Molex headers for attaching outputs and pots. I haven't put a microscope to it, but the board looks really clean and the sockets and adjustment pots fit just fine. Some of the boards have a bit of a nubbin off a corner where the cut was not quite clean, but not a real big deal.

Many thanks to everyone on this forum for providing help and advice over the months while I worked on this project.

Now to populate this thing to see if it actually works!


veets
Congratulations! I mean to try myself that someday. Hope it works. Be sure to provide updates.
Monkizzle
Go! Go! Go!
kassu
Looks nice!

May I ask why there are 2 transistors in the sine shaper? It looks like the JFET type.
l3v3l6
kassu wrote:
Looks nice!

May I ask why there are 2 transistors in the sine shaper? It looks like the JFET type.



Yes, JFETs. Two MMBF4117s.
Borogove
Looks great! SOLDER ALL THE THINGS
kassu
l3v3l6 wrote:
kassu wrote:
Looks nice!

May I ask why there are 2 transistors in the sine shaper? It looks like the JFET type.



Yes, JFETs. Two MMBF4117s.


You need yo solder only one. In my schematic there were two footprints in parallel to give the choice between SMT and THT, but only one is supposed to be populated. Good luck!
MickMad
JLCPCB prints pretty good PCBs, I often order from them.

Congrats on making your first PCB, I really hope for you that everything will work on the first try smile

What CAD did you use to draw it?

In any case, I got some suggestions for you:
-don't use odd angles on the tracks, either lay them horizontally or vertically, and if you need to turn use 45° angles (avoid 90° where possible)
-try to lay as many tracks as possible on one layer, while reserving the other layer for ground
-when a track has to go on the bottom layer, make sure that it crosses tracks in the top layer perpendicularly
-use copper pours to fill unused space with ground connection
-use wide tracks for power lines (I use as much as 0.8mm thick tracks depending on the situation)
-avoid placing components identificators inside the component boundaries, once you place all the components you won't easily identifiy their names
-place components as close as possible to the pins they're connected to; example: place all the resistors that connect to the inverting input of an opamp near the opamp.

There are MANY more guidelines to follow but these I suppose are the basics to proper PCB layouts. The last one in particular is very important, because grouping the relevant components together and placing them in a logical way can help a lot when routing the PCB. giving a cleaner look.

I repeat, I really hope your first PCB is a success!
l3v3l6
kassu wrote:


You need yo solder only one. In my schematic there were two footprints in parallel to give the choice between SMT and THT, but only one is supposed to be populated. Good luck!


Thank you for pointing that out! d'oh!
l3v3l6
MickMad wrote:
JLCPCB prints pretty good PCBs, I often order from them.

Congrats on making your first PCB, I really hope for you that everything will work on the first try smile

What CAD did you use to draw it?

In any case, I got some suggestions for you:
-don't use odd angles on the tracks, either lay them horizontally or vertically, and if you need to turn use 45° angles (avoid 90° where possible)
-try to lay as many tracks as possible on one layer, while reserving the other layer for ground
-when a track has to go on the bottom layer, make sure that it crosses tracks in the top layer perpendicularly
-use copper pours to fill unused space with ground connection
-use wide tracks for power lines (I use as much as 0.8mm thick tracks depending on the situation)
-avoid placing components identificators inside the component boundaries, once you place all the components you won't easily identifiy their names
-place components as close as possible to the pins they're connected to; example: place all the resistors that connect to the inverting input of an opamp near the opamp.

There are MANY more guidelines to follow but these I suppose are the basics to proper PCB layouts. The last one in particular is very important, because grouping the relevant components together and placing them in a logical way can help a lot when routing the PCB. giving a cleaner look.

I repeat, I really hope your first PCB is a success!



Thanks for the list of suggestions. Many of those I had already known and kept them in mind when laying out the board.

Is there any particular reason for keeping tracks strictly horizontal or veritcal? I knew about not using 90° angles and avoided them.

I did give a little bit wider space to the power supply nets.

The bottom layer was a solid pour for GND. Most of the traces are on the top layer, with a few on the bottom when necessary.

It was really challenging to get the satellite components as close to the TL074 as possible. I'm sure I could of done better, but this is just my first attempt at PCB design.

I went back and forth about where to place the component names. I see your point about the name being hidden once the part is in place, but noticed that many folks do place the part name inside the outline. This does save space that would otherwise have to be allocated for locating the text, although in this design there is lot's of empty space anyway.

I used Autocad Eagle for the design.
MickMad
l3v3l6 wrote:

Thanks for the list of suggestions. Many of those I had already known and kept them in mind when laying out the board.

Is there any particular reason for keeping tracks strictly horizontal or veritcal? I knew about not using 90° angles and avoided them.

I did give a little bit wider space to the power supply nets.

The bottom layer was a solid pour for GND. Most of the traces are on the top layer, with a few on the bottom when necessary.

It was really challenging to get the satellite components as close to the TL074 as possible. I'm sure I could of done better, but this is just my first attempt at PCB design.

I went back and forth about where to place the component names. I see your point about the name being hidden once the part is in place, but noticed that many folks do place the part name inside the outline. This does save space that would otherwise have to be allocated for locating the text, although in this design there is lot's of empty space anyway.

I used Autocad Eagle for the design.


Well, technically nowadays there's not really a need for that; in older times, sharp angles like 90° ones could create what is called an "acid trap", which means that the acid used to etch the board would linger for more time in the corner area and eat away more copper than it should.

I still use 90° sometimes, for example when I lay a big power bus I tend to draw a thick trace going the lenght of the PCB and then I lay branches horizontally to bring the power line where needed.

There's also an issue that occurs when designing really, really high speed circuitry which is the signal reflection effect; it is definitely not an issue in low speed designs such as an audio VCO.

Practically, the horizontal/vertical thing boils down to two factors: reducing loop area when two traces are intersecting (one on top, one on bottom) and aesthetics. The former factor, when two traces overlap the return current path of the traces is not anymore straight below the trace (with the ground plane) but it has to go around the trace that it overlaps; the latter is just personal, for me it gives a sense of order.

Regarding the components placement, it comes easier when you use small SMD parts like I do, but in your case you could try placing the resistors/diodes vertically, it reduces the real estate occupied by them.
l3v3l6
I finally got a board populated, applied power and, wouldn't you know it, a puff of white smoke appeared over the power conversion area. Before applying power I had lowered my expectations and would not of been surprise if the board produced nothing in the way of audio frequencies, but pyrotechnics was truly disappointing.

It turned out to be a problem with the negative voltage regulator. I had made my own library part for the UA78L05 and MC79L05 I was using and copied the footprint from the UA78L05 to the MC79L05. The problem is that the pin connections are not the same and lethal current was supplied.

I was able to mount a replacement MC79L05 to the correct pads and applied power again. No smoke this time. I had not socketed the 3340 or the TL074 yet, so I checked my voltage supplies and all looked okay.

Socketing the ICs, I applied power, a CV voltage and started probing with my Oscope. Something was strange. I was getting approximate waveforms but they were at ~96khz. When I say approximate I mean they really looked kind of ugly.

Unhooking everything I did a complete reaassesment of the board, comparing it with a working model I had put together on prototype board. The prototype did not have all the features of the PCB but the basics were there.

For starters I had no GND connection to the 3340. In the schematic I failed to merge GND with the 3340 ground pin, so no ground was created for the board layout. That was easy to fix with a jumper wire. Also the circuitry between pin 11 and 12 was not right, so I ripped that out and rewired according to the AS3340 datasheet.

Then I was finally able to get some sound out of it. There's still some problems. Sine wave output is triangle and the PWM adjustment causes wild changes to the frequency (I think this may be due to my power rails being too small and how PWM shares power with the frequency adjustment).

Anyway, it has been a good learning experience. What I'm going to do next is start on a simpler board with just the basics and model it off of my working prototype, part for part.
EATyourGUITAR
l3v3l6 wrote:


looks like a paults disciple with roger's .com power header. this would work great in a time machine when synths were synths and PCB's were large for no reason at all. top notch for the style if that is what you like. probably not so good for making mass production and small format.
Schlumpfhut
Nice job w00t

Maybe - if you at some point in time are going to revise/change your design - you add a footprint for an MOTM-style power source for those of us who are building in that format.
av500
MickMad wrote:

In any case, I got some suggestions for you:
-don't use odd angles on the tracks, either lay them horizontally or vertically, and if you need to turn use 45° angles (avoid 90° where possible)
-try to lay as many tracks as possible on one layer, while reserving the other layer for ground
-when a track has to go on the bottom layer, make sure that it crosses tracks in the top layer perpendicularly
-use copper pours to fill unused space with ground connection
-use wide tracks for power lines (I use as much as 0.8mm thick tracks depending on the situation)
-avoid placing components identificators inside the component boundaries, once you place all the components you won't easily identifiy their names
-place components as close as possible to the pins they're connected to; example: place all the resistors that connect to the inverting input of an opamp near the opamp.


and make the solder vias for the caps and resistors larger, you have the space...
Alfrede
Hi l3v3l6,

your PCB looks quite cool. What you might know is that the Part mc79 has a negative Voltage. The 78 idicates a posetive Voltage. What software do you use for your Project? Personally i began with kicad an there are a lot of Parts with their Footprints. When you share your File we can have a look together where your fault is.

Greetz

Alfrede
l3v3l6
av500 wrote:

and make the solder vias for the caps and resistors larger, you have the space...


Are you refering to the sollder pad around the hole, not the hole itself? I was just using the default design values in Eagle.
av500
l3v3l6 wrote:
av500 wrote:

and make the solder vias for the caps and resistors larger, you have the space...


Are you refering to the sollder pad around the hole, not the hole itself? I was just using the default design values in Eagle.


yes, the eagle defaults are way too small for hand soldering, I had the exact same issue when I did my first through hole design in eagle...
FetidEye
eagle tips:

check out snapeda.com . all the Eagle parts you will ever need
also, The MusicThingModular Eagle library is pretty handy.
devinw1
I got burned by negative VRs too. Not only are the pins different (got that part right), but the case is live to DC voltage, not ground (like it is on positive VRs)! Be careful about that. thumbs up
MUFF WIGGLER Forum Index -> Music Tech DIY  
Page 1 of 1
Powered by phpBB © phpBB Group