Board layout

[studiostevus]

Hi Guys,
I am breaking my head over the best board layout for Pedja Rogic's I/V for TDA1541a as published here. (public domain, so I assume to publish my board layout for private use here)....

I would like to try to etch the board at home. As it would be my first home made PCB, I would have liked to use single sided, but this seems impossible with this design. What do you guys this of my current double-layer layout? Any improvements?

draft1.jpg

[amc184]

To be brutally honest, it's pretty bad. It'd take too much time to go through every fault with it, but here are a few notes:

- To start with, the circuit this board is based on is incomplete. I would probably put the power supply on the board, but even if you don't, you'll need some local decoupling capacitors.
- Do the component footprints you've used actually correspond to the components you will be using? I noticed you've used a weird style header footprint and quite a large resistor footprint. You've used two different footprints for the TO-92 devices (BC547, BC557 and 2SK170). Don't just use the default one that whatever CAD program you use suggests, actually compare them to what you will use. When designing PCBs I only use footprints I've drawn myself.
- The traces are too thin. Since this is a line level board you probably don't need to worry about current carrying requirements, but you'll be etching the board and you don't want to have them lifting. Make them two or three times wider.
- The traces are routed and the components are placed without any logic. Ground traces are important, you need to route them using a star topology or as a ground plane. The same applies for power supply rails. The components can be just scattered around, but it's nice to arrange them in a pleasing pattern. They could also be far more tightly spaced than they are currently.
- Make the board practical. Remember things like mounting holes and connector positions. Make the board so that it will be easy to use.

Here's one of my boards as a example, it's a power amplifier, each board is a single channel:

[janneman]

Agree with the above comments. OTOH, you've got to start somewhere and I wouldn't want to show any of my first boards!
But you'll learn fast.
Some tips:
- turn X1 CW and move up;
- turn R6 CW
- turn Q6 CW and move up & to the left.

Keep it compact and logical, try to minimize trace lengths.

jan didden

[studiostevus]

Thanks for the advise. I have made a second version (started from scratch), but not sure this is significantly better, although it has a ground plane.

rogic_iv.pdf

[janneman]

Originally Posted by studiostevus

Thanks for the advise. I have made a second version (started from scratch), but not sure this is significantly better, although it has a ground plane.

Attachment 206016

Better for sure. But let's do a few more:
Look at the tracks for Q1! Why not move it under R4.
Look at C2. If that was below the TDA input, you'd have a much more compact design and less track length.
Why not put R1 next to R2?
Look at the traces from Q2 - it should be to the left of Q6 and both should be moved up.
You still have two different footprints for the TO92. Those for Q3 and Q4 will confuse you at the time you put the board together and virtually guarantee a mistake at one point.
Use the Q6 footprint.
Try to forget that you are dealing with audio and how it sounds.
Try to look at it as a geometric problem. Compact layout with short traces. That will automagically sound best!
And don't start from scratch everytime, that gets you only in a loop.
Move a few parts at a time, and you'll converge on a good solution.
And, you can ALWAYS improve a layout. At some point you got to stop worrying.

Details like ground planes come at the end.

jan didden

[amc184]

You need to have another look over the suggestions I posted yesterday. Your second try still has almost all the faults of the first. A couple more specific comments:

- Do you know what the size of your output capacitor will be? The footprint of this component is very important because the size of a 10uF film capacitor can vary so much. I'd normally use an Axon True-Cap or a Mundorf M-Cap.
- Your traces could still do with a bit more width, maybe 30% more.
- I see you've added mount holes, what tiny diameter did you use? They'll need to be at least 3mm in diameter, you'll struggle to find screws and posts smaller than that.
- Many of your traces are far to long. Look especially at the input trace from the TDA1541A, it's huge. Look at the two vias you used to jump under the trace between Q1 and Q4, why not just move R10 closer to C1?

The issue of the power supply needs to be resolved as well. You can't ignore this, it won't work without at least local decoupling. Presumably you will be mounting this inside a CD player, so I'm guessing that you were thinking of running it off the CD player's existing power supply. You need to check what supplies will be available, most TDA1541A based players will supply +5, +9, +15, -6, -9 and -15V, you need +15, +19 and -19V. If it were me making this board, I'd be including an onboard power supply, something like:
- Dual 120VAC to dual 18VAC transformer
- Filter bank
- Series +19 and -19V regulators (both LM317 or similar)
- Further +15V series regulator

[MJL21193]

Hi,
That doesn't look like a very complex circuit and if you are going to etch this yourself, you should try a bit harder to make it a single side board. Double sided homemade boards are not easy to do and it takes practice to line the layers up accurately.
Use jumpers if you need to but if you want to improve your layout skill, try to do it without them.

NPX_01124.JPG

Like janneman said, we all start somewhere and though he doesn't want to show his first efforts, mine are immortalized here on this forum (somewhere )

[studiostevus]

Hi,
Thanks again for the advice.

@amc - The output stage will be for a DAC, and powered by separate +/-19V and +15V Salas shunt regulators. This hopefully covers the power supply decoupling matter.

@MJL - you are right, it is not overly complex, however I dont think a single sided board is manageble.

@all - I will puzzle a bit further tonight, but I think I get your point to shorten the wires and look at it as a geometrical problem. What I find, however, is that the more I try to shorten the wires, the more of a spagetthi it becomes (wires tangled up around each other on 2 layers in the middle of the board, crossing layers and all), whereas allowing longer leads gives a bit more room to let wires run in a bit more aesthetic (and possibly less interference) way.

Btw - MJL's board looks very nice! How did you etch that?

[amc184]

This hopefully covers the power supply decoupling matter.

It doesn't. You still need local decoupling. Standard practice is to have two capacitors next to the consumer for each rail, a film and an electrolytic, with values of about 100nF and 220uF respectively. These ensure that the consumer receives a nice, low impedance supply.

I wouldn't use a third power supply to provide the +15V rail, I'd put a regulator on board. It'll only add a few components, and will be sufficient for the job.

I've attached a schematic of what I think you should include on the PCB. Highlighted in red is the 19 to 15V regulator, you could omit it, but I suggest you don't.

[studiostevus]

Ok, I did some more work on the board.

-added lm317 to bring down 19v to 15v and removed the separate input
-added decoupling caps. Not sure this is what you intended to say.
-the board has much shorter traces, although it has become somewhat messy

What do you think?

rogic_iv_sch.pdf
rogic_iv_brd.pdf