[AndrewFischer]

Quote:

Originally Posted by splaz /img/forum/go_quote.gif Anyway to change that btw ?

With Eagle,

View, Grid and you can change the grid to metric.

To change the width of an existing trace, click on the the change icon (wrench) then change the width. You should rip up the pour first.

If you plan to send out to have the board made:

Most PCB fabricators give their design rules in mils. Even if I go somewhere else, I try to layout my boards to meet Olimex's 10mil spacing. If you meet their 10mil rules, just about anyone can make the board.

 

[DaKi][er]

Please stay with mils for units, it is the standard for just about all the libraries included in eagle, all the parts you use and manufacturers specs

You'll soon learn the units and know how much 16mil is or 40mil and figure out appropriate trace widths and such, the only reason I use mm is when I want to measure how big a final board is or draw out a boarder at a certain size, then it is straight back to mils

 

[AndrewFischer]

I use mm in Eagle in three places. I use it in the Library when I'm adding a part with metric dimensions. If I'm making a board for Olimex, I use mm for the drill sizes. I use mm for the board outline.

I use mils or decimal inches for everything else.

 

[splaz]

Update, finally got some time to work on it.

Wanted to know mm just so I could do the heatsink.

Okay, this is the 317 regulator part of the circuit keeping in mind what you guys have suggested in terms of layout. I think this looks quite a lot better in many regards, major downside is it's only really intended for that heatsink, but most other similar supplies for this purpose don't bother with a heatsink, so I can go naked or with that heatsink, either way is good.

The resistor on the box cap side of the reg, I'm planning to be able to use one of those top adjust box trimpots so you can use either that or a resistor once I sort the pads out, but wasn't entirely sure if there is an optimal way to connect the trimpot.

ie. Is it preferable to short the wiper to the adjust pin or gnd, or leave one pin open and connect the wiper to either gnd or the adjust pin. Does it even matter.. ?

Also the part mounted vertically is the back emf diode, I'm assuming nothing wrong with having it upright ?

I figured there potentially may be issues with having them that way if they were say used in the rectification due to the long lead, however given this diodes function I get the feeling it doesn't matter. Sort of out of the scope of my knowledge either way but I'm going on gut instinct, which is often wrong, but I hope it's right this time.

Another thing I have to do is actually buy the heatsink as they have two tabs on the end of the arms that go into the board, they're nowhere near any components so not an issue, just have to buy one to measure where they actually are as the specs don't say, then I can alter the package to put in the slots for them.

edit: Oh yeah, of course there is naturally more to the circuit, however just wanted to get that regulator area done right as that seems the most critical and was harder for me to get right. Need to of course add in the other parts of the circuit and test points aren't in yet, just wanted to check that I'm on the right track.

Also, yet another questions from me...

The back emf diode for the tantalum right next to the reg, should that be closer to the cap ?

Okay, I think that's my annoying question limit for today.

 

[AndrewFischer]

Looking good

I haven't checked where the traces go, so no idea if you've got it wired correctly.

Better to short the 'unused' pin to gnd. It doesn't matter in normal operation. If the trim pot fails so that the wiper is open then you still have a connection.

Diode will work upright. Only downside is you can't tell easily which way the diode should go. Just double check when you install it.


Hints:

Now is a good time to look at the design rules for the fab you plan to use.

Make sure your silk screen outlines are wide enough. Eagle defaults to 5mils and that is too narrow for many fabs. Some of the fabs I have used with have a minimum width of 8mils. Olimex needs 10mils.

Drill rack. Really only an issue with Olimex, but it is best to double check your drill sizes against what the fab will be using.

Trace width and space. Shouldn't be a problem. Best to keep your widths and spaces >= 10mils.

 

[luvdunhill]

I have a few questions more than anything... I've been studying this article at TNT:

http://www.tnt-audio.com/clinica/reg...edance1_e.html

basically, it implies that the regulators have their best operating point at around 30mA. I have built a similar supply as yours and have included two 2.7k resistors after each regulator with decent results, due to the points made above.

Also, what about using something like this (http://www.diodes.com/datasheets/ds21227.pdf) for rectification? I have some on the way to replace a simple integrated bridge rectifier.. they are kinda odd shaped parts (GBU sized I believe?), but you should be able to accommodate for them with your custom PCB..

Finally, I am thinking about using a RFI filtered power inlet, which seems like a decent add on and brings this sort of topology close to the STEPS design (in topology only chances are, not performance). The particular part I'm considering is a Qualtek 862-06/003.

I'm not sure if I've been any help, but I thought I'd throw those ideas out as we're implementing similar power supplies.

 

[mono]

Luvdunhill, I have often used bridge rectifiers like the one you pictured, for misc supplies but not as often on a small current audio project. The gains in using them are very high current (in context, certainly diode bridges go much higher than that, but I mean for headamps), and sometimes board real-estate. That particular package with it's .2" pin spacing is even usable on perfboard since it has 0.2" pin spacing, though the perf holes may need slightly enlarged.

Otherwise they're nothing special really, would be more suitable for a budgetized gainclone as there's little point paying for a 8A avg/200A peak bridge when the supply only sees somewhere between a few dozen mA to an amp or two.

 

[splaz]

I have a rather hefty bridge in the parts drawers rated to a few amps that would make layout a lot easier. It's straight with widely spaced pins, 2 AC inputs in the middle + one side, - the other. Nice and easy. However then snubber caps would be a bit of a pain and it is way overkill.

luvdunhill, first link not working and the second, I had a read through that when I first learned of the no low esr after regulators, although I didn't quite realise how low it was. Hence the original 470uF on the output. Although I had originally intended to use a general purpose and not low esr, but at that capacitance the esr is fairly low anyway...

Diode standing up, that's the whole point of the "-" mark, that side is the way the anode points to if that makes sense. Can still be a little confusing as if you do it on the other side it needs to be flipped...

Design rules, I'll look into that if I decide to take the design to a fab, might try and implement a few of those but some of them may be fab specific and I haven't decided if I want to do that at this stage. Want to have a go at etching it first, make sure nothing goes ka-boom and if I feel it's worthwhile may do a small run.

 

[AndrewFischer]

Quote:

Originally Posted by splaz /img/forum/go_quote.gif Design rules, I'll look into that if I decide to take the design to a fab, might try and implement a few of those but some of them may be fab specific and I haven't decided if I want to do that at this stage. Want to have a go at etching it first, make sure nothing goes ka-boom and if I feel it's worthwhile may do a small run.

Try checking your layout with the 10mil rules from Olimex.

http://www.olimex.com/pcb/10mils.dru

Just about any fab can make a board that fits these rules. Its a good check to run if you are planning to do some sort of printer transfer too or other home process.

If you are thinking about DIY etching the board just to save money, I'd take a close look at the costs. It may be cheaper to send the board out.

I don't even buy Vector board anymore.

 

[splaz]

Well I think I've pretty much finished. Only thing is, how do people normally put the input/output pads in. Is there anyway to make the Vcc arrows have pads or not ?

Well heres the rectifiers, this seems a bit messy and well maybe I should just settle on one option rather than making it a bit more flexible. Is it even as bad as I think it is ?



Don't know if that's any good design rules wise as eagle kept spitting out problems mostly with that area, but I need to sort some things out with that as it was saying there was issues with the holes for C5 and C6... ?

Heres the rest of the board



I tried to make the components as neat and compact as possible, while still making the tracks fairly simple layout wise.

That's with all the test pads in, not input/output pads as of yet.

Didn't realise how hard this layout thing can get until doing this and this is pretty simple too.

 

[AndrewFischer]

Quote:

Originally Posted by splaz /img/forum/go_quote.gif Well I think I've pretty much finished.

Yup. Thing is the last 5% of the work always seems to take 95% of the time.


I modified the wirepad library. I changed it so the Value prints on the silkscreen instead of the name. That way I can have pads with identical names. No idea why Cadsoft didn't do it this way in the first place. I changed the font size and ratio for Olimex. Changed the drill size too. Small example:

Up to you with bridge vs. individual rectifiers vs. flexible. I use discrete diodes because I've got parts drawers full of them.

Try moving parts around to figure out what is causing the design rule errors. You may need to rip up the pour to see the problem.





Layouts get easier with practice. Eagle is quirky.

 

[FallenAngel]

Is there an updated schematic, I'm totally interested in building one of these and trying out how it sounds vs a virtual ground.

 

[splaz]

Thanks for all your input.

Quote:

Yup. Thing is the last 5% of the work always seems to take 95% of the time.

Too true, just checked the trimpot space in reality and although the pin spacing is fine all the ones I can get locally are longer, need to rearrange that. Decided I might want to go tangent style and have a resistor and trimpot in series for finer adjustment.

Now I'll be messing around with the pad library thanks to you...

Still haven't made up my mind on the rectification...

I think I know what the design rule issue is. I believe some of the tracks may be overlapping.

So close, yet so far.

 

[mono]

For the diodes I would do without the allowance for a 1A diode bridge, and place the 4 diodes parallel to each other (laid out, obviously not schematically). I'd also put a little space between each and an extra pair of holes to allow for a little longer and wider parts, at least 2A (DO-15), maybe even 3A diodes. 2A diodes are still only about 4 cents each @ Digikey, I don't see the draw in having a 1A bridge when there isn't a space constraint and the cost is higher.

 

[splaz]

True, had just started leaning in that direction, guess you pushed me off the fence while I was off balance.

More work to do...