or Connect
Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › Questions about drawing single sided PCBs
New Posts  All Forums:Forum Nav:

Questions about drawing single sided PCBs

post #1 of 22
Thread Starter 

Hey guys,

    I have some questions about drawing single sided PCBs...I have searched the web for answers but most are tutorials with limited or no quality answers to my questions... for some reason I've become obsessed with making my single side PCBs as small as I can get them, and using a ground plane to simplify things and eliminate ground traces. So, to start this off, please look at the picture and tell me if you will, what is the problem with example "A" against "B" as far as the best possible circuit...please keep in mind that I will probably not understand your explanation right off and will have to study your answers and research them...

 

 

 

post #2 of 22
Quote:
Originally Posted by vixr View Post
 

...single side PCBs...ground plane ...

 

Those two ideas conflict.

 

Part of the reason a ground plane has an effect on a circuit is that it provides a capacitive coupling to ground for the traces that go past it on other layers. On a single-sided board, there is no "other side" to provide the other plate of the capacitor.

 

It's fairly tough to make useful ground planes on a 2-layer PCB.  We did try on PPA v1 and v2, for example, but mostly what we achieved is fairly thick power busses, not proper ground planes.

 

This is one of the reasons I went to 4-layer boards with PIMETA v2. It gives you the ability to dedicate 1-3 layers just to power and ground. I still ended up sharing some layers with signal and power, though.

 

Quote:
"A" against "B" 

 

It depends on what the circuit is doing, but general principles tell me that A is probably better.

 

In "B", the solder pads potentially weaken the trace. Solder "should* fix the thinning of the traces due to the drills, but that assumes no manufacturing imperfections. The lack of plated through holes due to making a single-sided board increases the risk that these drill hits will cause a trace break. Ideally, you'd put all three resistor solder pads off on a short spur from the main trace, so that no single drill hit can tear the main trace off the board.

 

You should also be using thicker traces. Those look to be maybe 20 mil? That means to have a drill that doesn't break the trace, you're going to have to use a 10-ish mil drill, and position it within a few mils of ideal to avoid taking a chunk out of the side of the trace, rather than put the hole in the middle of it as intended. Using big thick traces gives you a lot of slack to play with when it comes time to drilling holes.

post #3 of 22
Quote:
Originally Posted by vixr View Post
 

...for some reason I've become obsessed with making my single side PCBs as small as I can get them...

 

This is not an obsession, PCBs should be as small as possible, unless there is a special reason for them not to be. This reduces track resistance, inductance and capacitive strays (all of which can have unintended consequences) and costs. Generally speaking smaller is preferred by the end user. DIY PCBs are not usually designed to any constraints, but this is not the case with many commercial products. Often the space available is dictated by the case, which may be determined by cosmetics, mechanical engineers and such fripperies. Pots, switches and ports may be givens which have to be accommodated.

 

It's good practice to at least think about how the board is going to be housed before starting a design. Power supplies (transformers and magnetic components) need to be kept at a distance from sensitive (amplifying) sections. Inputs need to be kept away from outputs. Power tracks (class B amplifier) may need to be kept away from signal tracks, but a line taking power to a relay that is constantly (or nearly constantly) active probably has no impact on signals.

 

Quote:
Originally Posted by vixr View Post
 

single side PCBs... ...using a ground plane to simplify things and eliminate ground traces.

 

You can't 'eliminate' ground traces. You can flood fill the areas through which they pass, creating 'thick' tracks, but effectively they're still there. You have to be careful when you flood fill, because you can create connections that effectively destroy a carefully thought-out (star or other) grounding scheme, but flood-filling is useful, if for no other reason than that it saves etchant. It's not a good idea, though, to start with a flood-filled board and depend on it to make the ground connections, for the reasons already stated. Draw the tracks so that you understand how the ground currents return and optimize the component placement so that the returns do not interfere. This is part of how to get a good layout.

 
Quote:
Originally Posted by vixr View Post
 

"A" against "B"

 

At "B" the track (between the resistors) can be replaced in your imagination by 2 resistors. The lefthandmost track sees all the current going to the two righthand (real) resistors. In "A" the track can be replaced by 3 (imaginary) resistors in an inverted "T". The track to the upper resistor sees none of the current going to the righthand resistor, but one (track) resistor (the lefthand) does see both. These currents all generate signal voltages across the imaginary resistors. If the branch were moved to the left so that it comes off at the point where the lefthandmost resistor makes contact, then the signal voltages developed across the tracks leading to the other 2 resistors would be invisible to each other. Whether these signal voltages are significant is moot, but it is considerations such as these which determine which layout (or even if another layout) is more suitable. In general power is supplied to the thirstiest limbs of the circuit first, working down to the least thirsty, with decoupling at each stage, so that the lowest power areas do not have large currents pulled through or past them by areas with higher power consumption, although this can be moderated by the PSRRs of the stages or sections.

 

I hope this somewhat wordy description has not added to the confusion.

 
w

Edited by wakibaki - 1/30/14 at 9:23pm
post #4 of 22

 

"C" is better

 

post #5 of 22
Thread Starter 
Quote:
Originally Posted by tangent View Post
 

 

Those two ideas conflict....

 

but mostly what we achieved is fairly thick power busses....

 

It depends on what the circuit is doing, but general principles tell me that A is probably better.

 

Ideally, you'd put all three resistor solder pads off on a short spur from the main trace...

 

You should also be using thicker traces. Those look to be maybe 20 mil?

Thank you sir for the awesome replies. Lots of ideas to research.


Edited by vixr - 2/1/14 at 2:42pm
post #6 of 22
Thread Starter 
Quote:
Originally Posted by wakibaki View Post
 

I hope this somewhat wordy description has not added to the confusion.

 
w

So much information...thank you sir

post #7 of 22
Thread Starter 
Quote:
Originally Posted by Avro_Arrow View Post
 

 

"C" is better

 

Thank you sir. Sometimes the parts have to be offset a little if other traces run under...But you already know that..  :)


Edited by vixr - 2/1/14 at 3:10pm
post #8 of 22
Thread Starter 

here is an example of a signal generator I wanted to build... the first uses a large ground "buss"

 

 

this one is the same circuit using ground traces...

 

 

which one will do a better job?

post #9 of 22
Thread Starter 

Also, wakibaki brought it to my attention that there is actually better ways to add the components that will make the device work better... I use the net function to identify the trace connections and then I place the parts in a way that keeps the traces short and the parts symmetrical...

 

 

 


Edited by vixr - 2/1/14 at 3:10pm
post #10 of 22
Thread Starter 

I need some more time to read all the info you guys gave me... Three of the Gods of DIY replied to me...lucky


Edited by vixr - 2/1/14 at 3:21pm
post #11 of 22

It would be better as a double sided board with a ground plane on the bottom.

It is not as hard as you think to do a double sided board at home.

My current portable amp uses a double sided board I etched myself.

 

Your listening and learning...and that's good to see.

post #12 of 22
Quote:
Originally Posted by vixr View Post
 

here is an example of a signal generator I wanted to build... the first uses a large ground "buss"

 

Actually, this isn't what I was referring to as a ground/power bus. Here's the PPA v2 layout:

 

 

The pink bits are where the red and blue traces overlap.

 

The power busses I was referring to are up at the top, where we have massive V+ and V- busses, because the space was there. Since it lowers the power supply's ESR, we did it.

 

Now, down at the bottom, you see the input signal traces going underneath a true ground plane, between the rear input pads and the pot. Here, the ground plane does the same thing that the ground shield does in a nice cable. The alternative would be either to have 6-ish inches of unshielded cable between the rear panel and the pot, or "encourage" builders to use shielded cable. Because we could do the right thing for the builder on the board, we did.

 

Now, to my real point about ground planes vs. power/ground busses: imagine trying to snake a ground plane anywhere into the middle of that board. We tried. It falls apart like rotten lace. When the amount of top-and-bottom signal traces gets this dense, you see the value of 4+ layer boards.

 

As for your board, the one with the ground plane — yes, that's what I'd call it — is better. The point we're all trying to make is that putting it on the other side of the board would be even better.

 

But, beware: with a true ground plane, you often want to cut holes in it around sensitive parts of the circuit, where you don't want coupling to ground. Op-amp input pins are a biggie.

 

Speaking of, what is U1, and why does it have 10 pins, two of which seem to be duplicates? And why are there no bypass caps?

post #13 of 22
Quote:
Originally Posted by tangent View Post
 

 

Speaking of, what is U1, and why does it have 10 pins, two of which seem to be duplicates? And why are there no bypass caps?


My guess is it's a 555 timer with a jumper under it.

post #14 of 22

hi vixr

 

some great advice already given. to expand on tangent/avro 's comment of the ground plane being better on the other side is that you really don't want to "cut up" a ground plane if at all possible. It is always necessary to some extent and sometimes even purposeful to force the ground current flow in a particular direction. when you fragment it too much , the risk is for generating ground loops. this becomes a much greater risk with larger boards. I am not necessarily on the same page as waki with small boards being better but I do feel that signal path needs to be kept as short as possible. board layout is a true gift and one of the arts that remain in this otherwise highly engineered field, my tendency is still to be true to the flow of the circuit drawing which is usually not the best for optimizing layout and utilizing busses as noted above. 

 

looking forward to learning more along with you 

 

..dB

post #15 of 22

By the way, this is what I mean by "short spurs":

 

 

This puts the drill hits off to the side of the main trace, rather than piercing it.

 

This is only for hand-etched and drilled PCBs, and it's done only to protect the main trace connecting these three parts. For a professionally-made PCB, especially a 2+ layer one, there's no need to worry about the pierced traces. The solder, hole plating, and component lead heal the break quite well.

New Posts  All Forums:Forum Nav:
  Return Home
Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › Questions about drawing single sided PCBs