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

Eurorack Power supply PCB
MUFF WIGGLER Forum Index -> Music Tech DIY Goto page 1, 2, 3  Next [all]
Author Eurorack Power supply PCB
msboude
Hey guys, newish to the forum so go easy!

I built this mock up of a Eurorack power supply. It's a plain-jane +/- 12v ps. Just wondering if there would be a desire for folks to get their hands on a copy of the pcb for a DIY skiff. Getting ready to build this in Eagle Cad, wanted to take a temperature check on if there would be any interest? This would be just the pcb and a parts list for Digikey. Would be done some time after the first of the year, as you know the holidays are busy.

Thanks for honest feedback! Any suggestions welcome!

msboude
P.s. would you prefer it to be powered off of a 16v ac walwart, or a transformer with a center tap?
julian
I think a wall wart would be a much better idea - less space required, and more suited to beginner diy work.
av500
keep in mind that in Europe AC wallwarts are a rarity by now...
msboude
Thanks for your input guys! I think I do like the idea of the walwart, since the people actually wanting these, will want them for smaller boxes. Hammond makes a nice 16v Walwart that I actually have powering my doepfer lc3 case...

I think I have an idea of how you could use the board for both a walwart and/or a transformer with center tap. I have some more reading to do, but I think I found a good schematic that shows how it can be done. Would just require leaving some items off of the board and connecting some signals with wire, through-hole.
msboude
Okay, so yes, this can be multi-use. There will be 2 ways to hook this up, one is with a center-tapped transformer and the other with an AC walwart.

There will be a power input terminal block marked AC1 AC2 and GND. With an AC walwart, you will just hook one wire to ground and the other to AC1. Works great!

Just started the board on Eagle last night, it's been a few years since I have used it, so I am refreshing my brain. sourcing parts now.
EATyourGUITAR
remember to spec 2oz copper when you order the custom PCB. the fuses can be on the PCB. make the traces nice and wide. consider how much current will be flowing and use a trace calculator to determine the TDP in watts. you need to decide if your case to case power port XLR has the shield for RF or 0v or both? if RF are you connecting it on only one side? is that ground lift done at in the cable or in the back of the connector? do you have a port for chassis ground on the power PCB or is this done at the bus board? or is the chassis grounded through the cable shield and the XLR hardware? a diy kit that does not discuss this needs just a little bit of extra work before it is really something that will benefit everyone involved. don't forget that there are a lot of really good power diy kits and also free options like the one you posted. make sure you are really adding something that is better than what is already out and possibly also cheaper and better documented. you will be very successful and the community will thank you.
msboude
Awesome feedback!

Fuses are on the pcb for both AC1 and AC2, they will be blade type - check!
I planned to calculate trace width and use 2oz pour.

Won't need to plan for xlr shielding and such, as this will just be the board and the components with two power terminal blocks 1. (AC1 AC2 GND IN) 2. (+12 -12 GND OUT) . How you ground it from there is up to you.

I would be happy to add a 2nd ground to the output terminal block (+12 -12 GND GND) For case grounding.

By all means, please keep up the feedback!
msboude
Progress!

This board will be constructed as a pos/neg adjustable power supply using the lm317 and lm337 regulators and two on-board trim pots. You have the flexibility to change the output voltage to your liking. Since it is an adjustable supply, it would make a nice desktop power supply for testing circuits as well as a eurorack power supply.

it will have eurorack standard pins for a flying bus board, as well as a terminal block for power out and an added ground for case ground.


calaveras
wallwarts are fucking ass.
They have proliferated due to how regulatory certification works for consumer electronics. If the device doesn't have an AC inlet, just a low voltage DC inlet, it isn't held to as high a standard.
But most wall warts on offer these days are trash.
They don't output the stated voltage under load at any where near the amp rating.

I haven't built a power supply from scratch in years, but for old school lead sled linear supplies it's not that hard to make 12v out of 120. The hardish part is the bipolar 12v and 5v.
But there are voltage converters for that right?
(cough, long day. Worked 3 different gigs so I am a little punchy)

Anyway, it occurs to me that you might get a few more interesteds if the power supply was configurable for both 12v+/- and 15v+/-. Depending on the whims of the builder. I know there are a lot of nerds into that Fraque Rack thing.
msboude
you can still get transformer wallwarts.. although most are switching supplies now.

Here is a link for a 16v 2.5A Hammond wall wart, it's what I currently have running my Doepher LC3.



For this board, you will be able to use a center tapped transformer if you wish, as well as a wallwart.
msboude
ignore
msboude
More progress tonight on this one.

50ml trace width. Hand routed. Now time for quality control.

I do know that I need to connect the traces to the other side of the eurorack power connector pins, I just gotta update the part in eagle.

I decided to leave off the extra ground on the output.

av500
msboude wrote:
More progress tonight on this one.

50ml trace width. Hand routed. Now time for quality control.

I do know that I need to connect the other traces to the other side of the eurorack power connector pins, just gotta update the part in eagle.

I decided to leave off the extra ground on the output.


1) you don't need to route GND explicitly, instead make a GND pour polygon over the complete TOP and BOTTOM layers. then you can also get rid of a lot of vias and have almost all traces on the TOP side.

2) use the eagle DRC command to check your design for obvious errors. the Eagle default rules are very conservative, but in case of a PSU board that'S actually not too bad

3) why can't you connect to the other pins on the 16 pin connector? just draw a net there like you connected the first row
av500
4) pin1 of your 16 pin header is top right, but it should be bottom right at the -12V, I would suggest you put a fottprint and silkscreen for shrouded header there
msboude
Thanks for the reply! Will get the header pins straightened out and marked.

I didn't use a ground pour as it's a split supply and I wasn't sure how that changes things. I have used polygon pours on single positive supply boards before, but I have never designed a dual supply, so I wanted it laid out as it was drawn up and designed. No vias were used.

edit, I just noticed my outputs are mislabeled. Will get that straightened out as well.

I appreciate your input!
av500
msboude wrote:
Thanks for the reply! Will get the header pins straightened out and marked.

I didn't use a ground pour as it's a split supply and I wasn't sure how that changes things. I have used polygon pours on single positive supply boards before, but I have never designed a dual supply, so I wanted it laid out as it was drawn up and designed. No vias were used.

edit, I just noticed my outputs are mislabeled. Will get that straightened out as well.

I appreciate your input!


ah right, vias are all through hole legs - I guess I do to much SMD smile

you dual supply still has a common ground, so I don't think it changes anything. having a GND pour on top and bottom makes for the lowest resistance in the GND path and is less copper down the drain in the fab - after all you pay for it smile
msboude
av500 wrote:
3) why can't you connect to the other pins on the 16 pin connector? just draw a net there like you connected the first row


Because I didn't assign pins to the symbol on that side. ha!
msboude
Cool! will look into ground pour some more on split supply. I see what you are saying now. Thanks for your advice man! I appreciate it!
FetidEye
Nice Treehouse!

The shrouded headers as used commonly in eurorack are in the standard library of Eagle : "con-harting-ml". use ml16
you can enlargen the pads if necessary.

It is good practice to add some text like "red line here"

and you might want to use other LED and small capacitors footprints. (with clearer polarity markings)

There is also a thing about not making 90 degree turns with your traces.
Use the Miter tool!
msboude
Fedideye - Thanks for your reply!

This morning I had a chance to rip up and rerun some traces to remove 90 degree angles. I also changed the output terminal block silkscreen lettering to match the outputs of the terminal block.

Thanks for the tip on the eurorack header, will look into that tonight! I made a note to add good markings for the eurorack header polarity, led, diodes and caps. This will be done after the board is totally done. I still want to double check my measurements for parts and pad hole sizes before I layout the silkscreen layer.

Getting close!
msboude
Alright.. some quick updates for those following (sound of crickets) ha!

Updated the eurorack pin outs for correct polarity with a large white line on the silkscreen layer indicating the -12 pins. Connected both sides of the pins to each other, before, only one side of the pin outs were connected.

Updated all caps to 50v, vs the 25v versions I was using before, allowing plenty of overhead without losing much space.

Updated the rectifier diodes to 3 Amp forward current, allowing for plenty of overhead there.

Ran some calculations for heatsink temps. Looks like max temps these regulators can handle is 240 degrees F (120C). Based on 18v rectified, with the low profile heatsinks I'm using (Ohmite FA-t220-38A), these regulators should be running at around 148 degrees F (48C) when running a constant 1A at 12V. You can pop in a larger heatsink the FA-t22064e to get them down a tad to 139 F (59C).

Traces are 50mil, they were calculated to need a minimum width of 38.4mil for 1.5A, so there is some headroom there as well.
emmaker
Don't run PCB traces or ground planes under a metal heat sink.
msboude
Alright! I will redirect as much as possible..

I take it that it is due to the heat?
KSS
Where to begin? Speak up and it's possibly discouraging or seen as a d**k move. Stay silent and yet another half-baked PCB hits the scene. If it weren't a power supply silence could more easily be chosen. If it didn't represent something so central to the synth experience, it wouldn't be worth the tons of time typing all the things wrong here is gonna take..

First, no, not heat. emmaker is warning against the short circuit that will happen when a 12 or 15 or 24 or 30 v potential is separated by only a solder mask. It will short. If the heatsink has legs with inherent spacers of sufficient height then you can ignore the comment for this kind of supply. Spacers are a good idea anyways as the airflow needed to achieve the temp rating you calculated is likely not met if the H/S is tight against the PCB. Unless you put convective cooling holes in the PCB itself, and these are not really too good either. But they're better than nothing with this kind of H/S flat to the board.

I would say the bigger issue is that you are obviously new at this and there are many traces which arbitrarily wander, bifurcate and it's really a mess at this point. Sorry, but you did say you could handle honest feedback. Since I'm typing now, here goes. First, do you see the two places in the posted image which will most certainly be a problem as they are too close to each other? NE quadrant, you have a trace nearly touching the H/S peg or screw. And there's no reason at all for it to be close anyways. Same if you follow that trace to the Euro power connector, where it nearly touches the pad next to it. Again, why? There is no need for the 45 exit from the net9 pad heading to R5 . just do the same as the ground pads.

Net 11 can be nearly all red, and should be. Then once it and nearly everything else on this board is on *one* layer, move that layer to the bottom. This board needs very few red (top?) traces, and is not improved by having this present mix of top and bottom. Get the blue -V output trace out from under the red. And then turn it red. We're going for nearly all blue, with a few red traces only. From your current starting point, it will be easier to go all red first, then move to bottom (blue).

When you have a choice of one or another trace to move to the top to make things work, put GND/0v on the bottom, and -V and V+ on top. This makes your board both easier to trace for repair and potentially less likely to short out . It's not the first thing you need to be thinking, but it's good to have in your mind as you work.

Make the main horizontal 0V/GND spine trace much wider. Much. Wider. 200mils Rotate all the parts hanging off of it so they are perpendicular to it which will get rid of many unnecessary trace bends. Bring C1 and C3 towards the center. Why so far apart? Slide C2 and C4 East, rotate the fuses and make the board smaller in the spine direction length. Size is cost in PCB. Size and Holes are your touchpoints. Once the fuses are rotated the input conn can slide East also.

Consider using flat to the board parts. Most people do not like vertical resistors and diodes. I think they're fine and give a nice transistion to the SMD parts that will replace them eventually. You can fit an SMD part on a 100 pitch vertical TH pattern. But here, your rectifier diodes and traces are much more fiddly than they can be laying flat. Trade layer hopping for flat parts where you can. Unless you are doing this as a SMD prelude. Then I understand and have done similar. But really the diodes should be flat. OR at least reversed per pair so that if they are pushed into one another a body meets a lead. What i'm saying is either rotate the lower left Diode 180, which will shorten and straighten net6's red trace and also resolve the bend in the blue trace of net 3 going under the spine. Better still just lay this diode across the spine and eliminate the blue trace! If the spine is 2 or 300 mils, then a 500 mil flat pattern will have plenty of space. Two diodes across the spine and two parallel makes for easy layout and easy understanding during repair.

Your 317 Vreg protection diode in the north should be rotated 180. It's one of many that should be looked at for how this rotation can de-convolute the traces. Fuck pretty layouts where all the parts face the same direction. This is a power supply. Make it *safe* first and electrically awesome next. Then!, if you can make it pretty too, Ok. But first things first. As Hinton sez and it's true, engineering is not a democracy. or something like that. Point being physics matters more than feelies.

Both trims can be moved so the adjustment screw is more central. Net 12 can and should be a straight vertical line til it meets one side of the cap hanging off the spine, already rotated 90 earlier. Notice how the resistor under R4 and West of D9, and R4 itself too, can be moved East and rotated to directly attach to Net 11 on the East side of the regulator (Net 11 in SE quadrant of your layout). See how many traces this removes and resolves?

There is so much more, and hopefully this gives you a start into making a better layout.

If this were mine, I'd re-establish that 2nd ground and use a .156 x 4 pattern at the East. Doing this means your board is now interesting to larger format users also as that is one of the popular standards in 4 and 5U. Also many DIY PCBs have this connector. Another Euro Con South of the first for a 2nd flying bus will make this a 6U power supply, and doesn't cost you any more for fab. There's plenty of room in the SE corner. I'd get the LEDs and their limit R's inside the h/s footprint next to the trimpots to tighten up the layout, but others might think they're hidden that way.

Most importantly, the schematic is supposed to make the circuit *function* and *topology* more understandable to a Human. The reason for this is that it doesn't necessarily reflect the physical needs and reality of the PCB layout. And remember, the electrons and holes are not experiencing anything but impulsion and availability. Period. They nearly always don't give a rats ass whether a corner looks like it does to us. But impulsion and availability matter greatly. C10 and D10 don't need to be separated as you have them now. Put them on the same line next to each other. In other words, the lines of your schematic do *not* necessarily reflect the lines/traces on your PCB. We see. Electrons and holes feel. Guide them when necessary, otherwise give them as much free rein as you can.

I'll finish with this. Right now, while you're still new at this, change that GND trace and net to 0V or 0v. It is *not* GND, and the sooner you make this distinction the easier life will be. For both you and the rest of the community
MUFF WIGGLER Forum Index -> Music Tech DIY Goto page 1, 2, 3  Next [all]
Page 1 of 3
Powered by phpBB © phpBB Group