PCB design dilemmas

[temol]

I'm trying to design a PCB for a fairly simple schematic - it's a hi-gain jfet preamp. I want to make a single sided board, with board mounted potentiometers, input and output at the edge, etc .. just elegant. I would like to have a specific potentiometer layout. And this is where the problems begin. Elegance versus design rules, clerance problems, jumpers, etc .. Each time I finish with crossing traces running through the entire board. I need some advice on this. For example - the reasonable path length from the input to the transistor in the first stage and its proximity to other paths. Proximity of the input and putput traces.  I will show you an example. For the sake of simplicity I omitted most of the components, leaving only the input, output, potentiometers and three capacitors. But it is easy to see what the problem is. This is a complete schematic.


And this is my simplified board.


It does not make a huge difference  whether the tone control is in the top or bottom row.

T.

[italianguy63]

Personally, I think that is overly ambitious for a single-sided board.  It would be much easier to do double-sided and not have a be-jillion jumpers... It is easy/cheap enough to have double-sided boards fabbed.  My .02.

MC

i.e.  Put the pots on one side, and the components on the other.

[~arph]

Yes, and even with a double sided PCB you will probably have a hard time with a compact form like that. Are you doing through hole or SMD?

[287m]

- you want all pots in same side as other component, right? Why not as Marc suggest, and show the beautiful guts? 
- in your simplified, why ground line in both side right and left? just in one side is okay. And you can ground plane too, for fast etching. hahaha

T, trust me, jumper isn't crime.

[temol]

It's not about the cost. I just usually do the PCB myself at home. I even made double-sided PCBs but soldering double-sided board with non plated holes is not the easiest task.
I do not see any problem with moving potentiometers to the other side of the board, I think I like it even better. But still the same problem..



287m - ignore the ground line.. I just wanted to get rid of the yellow lines connecting the components. It's just an example board. There is going to be a ground pour in the final version.

~arph - through hole.

T.

[GGBB]

Most of the boards I have designed at this level of complexity are either double-sided or use at least one jumper. Additionally, having pots near their circuitry helps a lot and is also a good design principle. In your case, you have input and gain crisscrossing output and volume. The left-to-right knob layout is opposite to the right-to-left in/out layout and therefore introduces design problems. You'll be a lot farther ahead if you make both the same - have the input near the gain pot and the output near the volume pot.

Another thing I have learned is to think of ground as its own thing, not as multiple second connections for the in, out, and power jacks. You've located ground pads for in and out as if they each need their own like they were connected to jacks. Usually they are connected to a switch which doesn't have a dedicated ground connection for both in and out. Also, don't make ground "trap" everything. It doesn't have to surround the entire board. The ground pads don't have to be beside in or out, and don't have to run directly to the outer edge of the board (and you technically only need one). As an example, in the version where the gain and volume pots are in the bottom row, run the ground from vol pin1 up and around pin2 to the right edge, then you can run the in directly to the gain pot, and the out up and around gain pin 3 and over to vol pin 2.

[~arph]

I usually do a ground pour first and let all grounds connect via the pour. Then as you lay out the pedal, only wire some ground connections if isolated islands occur. (which you usually can solve by rerouting other tracks too). But this is probably a better strategy for a double sided board too. (as I do a ground pour on both layers).

[rankot]

I usually make single sided PCBs and poured ground. Like this (it's modified orange squeezer):



I like to have all the jacks, pots and switches mounted on PCB, because I hate wiring. Since I can't buy long legged pots here, I extend legs with leg trims of resistors or diodes.

[287m]

my workflow routine

get request or i want the pots position, ex
Tre-Mid-Bass
Gain-Pres-Vol
whatever IN and OUT and 9V position, but mine prefer 9V in top and ground pads near in, just in case need shielding
So, i imagine first. Then said to myself, OK. its doable.

and since im just Perfboarder, i just layout with ground line
ground plane is for my friend, the etcher. hahaha

example, some my friend request who want component in vertical
the DLS3-ish https://1.bp.blogspot.com/-Gtw7GZ545xA/WgL_sjfGn6I/AAAAAAAAApI/ba-R9en4E0gxC5w68RI1SS3OxAb9yhargCLcBGAs/s1600/DLS3.png
and 5150, currently not finished, because the fvckin 5458 and J201, https://1.bp.blogspot.com/-V7NLt2gH07c/WgMBkNOb1jI/AAAAAAAAApU/BREG_yjxBEErBvNdHxmUda1DnSACuaMHgCLcBGAs/s1600/5150f.png

i know, its not nice, but im fine with that
===
BTW, just see you in rusian forum
in progress to head to head 2 Krank?

~~~~~~~~~~~~~
Woah Rankot, nice!

[Marcos - Munky]

Febri, those layouts are nice, really. Just a suggestion, avoid those 90 degree traces. See rankot's layout and do the traces that way. It may not make any difference if you do perf, but for pcb if the traces have 90 degree turnings, they can lift of the board with just a little excessive heat.

Rankot, nice layout! If you did it in eagle, could you share the 3pdt library you've used? Mine have even spacing between pins, which doesn't match the 3pdts I have here.

[PMowdes]

Why one sided?? 

PCB fabrication isn't any cheaper if you go one sided, you are just making a rod for your own back by not using the other side of the board

If you use someone like Elecrow for fabrication you can get a 10 boards fabricated and delivered form china for less than $10, so cost shouldn't come into it

And as for ease you wont see any difference when populating the board with components

You should be able to get your pots and switches where you need them with out too much trouble if you use both sides of the board.

I always start with the dimension layer, make sure it fits your enclosure.  Then place the pots and switches and off-board wiring pads how you want them.

I'd steer clear of board mounted jacks and footswitches where you can, they are almost impossible to remove once they are soldered in place

[temol]

GGBB - I'll try to move gain and vol pots and see if it helps. You got me thinking about ground pads from IN and OUT. Those ground pads are helpful when testing the board, but then I do not use them anyway after putting the board into the enclosure. I (almost always) use shielded wire, with shield connected only to the jacks.

PMowdes - why one sided? Because in only one day I'm able to: design the board, etch it, put the soldermask, drill the board and solder the components.

Thank you all for the input!

ps. my design routine - check available enclosures, take smallest possible that does the job, insert enclosure outline into Eagle, draw the board outline, put the pots, supply pads, jack pads.. and so on..

T.

[GGBB]

GGBB - I'll try to move gain and vol pots and see if it helps. You got me thinking about ground pads from IN and OUT. Those ground pads are helpful when testing the board, but then I do not use them anyway after putting the board into the enclosure. I (almost always) use shielded wire, with shield connected only to the jacks.

Here's an example of one of my single-sided layouts - 5 pots and LED board mounted on reverse side - 1590B friendly. Control layout (on pedal) is right-to-left. In and out in the bottom corners, Vin and power ground in the top corners. Additional grounds for in (near the in) and footswitch. Input and gain close together, output and volume close together. I use that configuration for nearly all of my layouts, but often don't use the in ground. Most of my layouts are for 3 or 4 pots, but I have done one six pot pedal (compressor) the same way (but needed one jumper on that one).

[temol]

and 5150, currently not finished, because the fvckin 5458 and J201

What about them?
btw - Killer sounding preamp!

===
BTW, just see you in rusian forum
in progress to head to head 2 Krank?

Yeah.. but I'm slowly leaning towards TrueVALs design, a bit simpler to layout.

GGBB - neat layout! Thanks for posting.

T.

[LiLFX]

A single sided board for a compact layout of this complexity AND high gain is a bit ambitious. I'd got with a two layer board. The big thing that a lot of pedal guys don't think about when routing their board is signal flow and EMI. Every conductor with a current flowing through it will have an electromagnetic field surrounding it that will radiate into the dielectric space. You want those fields to return to ground and not neighboring signal lines. Guitar pedals are considered to be forgiving of bad layouts because guitars are inherently noisy anyway so we tend to ignore additional noise, but I'm sure we've all built a pedal that squealed or misbehaved and we scratched our heads wondering why. Welp...they aren't that forgiving and proper layout matters even in a noisy pedal.

Route your board however you need to route it, but I'd make sure you allow ground to squeeze between traces and add a ground pour to the opposing layer as well. Stitch in some ground vias around your input and output traces .

[R.G.]

It is usually possible to lay out through-hole circuits on a double-sided plated-through PCB in the space under the components. That is, when the components are brick-walled side by side in regular rows. the space under the components can usually support the inter connections with 50mil pads and 12 mil traces and one trace between holes on 100mil centers. The layout pros refer to this as "one trace per channel", a channel being the free space between two adjacent IC leads or grid spacings.

That is by no means a statement that it is easy, or that all circuits can be made so.

Single sided PCBs probably have a limit of layout density that is more than half as dense, but less than the density of the double sided board,

The point of this blathering is that there is a cost of laying out a circuit, in time and effort. This is an idea from some design automation courses that I beat on in PCB Layout for Musical Effects. If you are near the edge of what is possible in a layout, you either have to work exponentially longer to make it all work, or you have to relieve one of the constraints and design rules. If you're running into the limits of your design rules and skills on a single sided board, and don't want to pay the additional time and labor to make it all fit, you may have to relieve a constraint to make it fit. In this case, the simplest constraint might be single sided-ness.  Or it might be the rule "no jumpers". Or the rule "only 1/4W resistors" or some other thing.

When a layout gets exponentially harder and you're questioning whether it is in fact possible given the limits you've put on your design, you're on the edge of learning something. It may be a new layout concept, some experience about what densities work, or just that you have been flirting with an unknown, but real impossibility. The details always matter.

[rankot]

Rankot, nice layout! If you did it in eagle, could you share the 3pdt library you've used? Mine have even spacing between pins, which doesn't match the 3pdts I have here.

Thanks, but I do all of my layouts in freeware PCB Creatror by Area Bay Circuits, because it's OK and flexible. Not too smart software, but I am used to arrange my components by hand. I usually use my basic layout with 3PDT, power supply parts and jacks already in place, then I choose position for pots and start populating from input to output. I always make single sided PCBs cause two sided with plated holes are produced by only one producer in Serbia and they are too expensive, plus they don't make less than XXX
I try to make PCBs without jumpers, but sometimes it is unavoidable.

[temol]

In my opinion "time vs effort" factor is very important, escpecially for DIY, single unit builds. PCB design (as many other design areas) requires experience..
When I design (or try do design...) the board, there is a breakpoint when I loose an interest with the current project. Mainly because I no longer see possible routing options and I'm tired of erasing traces, moving components for the fiftieth time. That's when I usually take a break for a day or two or I start a new project. Sometimes I have up to ten partially finished desings at different level of completion.
I suspect that the main problem is the urge to stack all components on PCB instead of gradually populating the board, working on smaller sections. Also stiffness in design limits me a lot.

T.

[temol]

This time I have a question about connecting shielded wire to IN and OUT jacks. Is it ok to connect shield like shown in the drawing?




T.

[temol]

Hi-gain lesson leared... I should not have placed the IN and OUT tracks too close (and parallel), even surrounded and separated with ground pour. This is the most probable cause of oscillations appearing with gain pot set at 15 o'clock. Of course I was aware of the possible problem. You can see the problematic tracks near the bottom edge of the pcb.



T.