Amplifier PCB Layout Guidelines?

[ron.eddy]

Originally posted by mzzj

It depends where you compare it.
Try fitting SMPS and a mic preamp on same board if you like challenges

Yea, by no means am I saying that there is no need for care with PCB layout, just wondering was all.

Where you are going to connect those bypass cap gounds together?

I was going to connect them to the main chassis ground via jumper wires. I was under the impression that the ground lead length is not as important as the signal lead length, which I have kept under 5mm as per AD797 datasheet recomendations, so should I also be worrying about the ground trace length as well?

I usually start with bypass cap placement, then feedback resistors and after that rest of the stuff where it fits. Dont be shamed to use jump wires on 1-side board, its way more better to use couple of jumps than run signals around the board in loops trying to not use jumper wires. Some people seem to rate pcb layout by amount of jumpers used, thinking that less is better.

This is the exact kind of advice I am looking for. Personal experiences and what you all like to do first, second, whatever. Thanks for the input.

- Ron

[flg]

Some general concerns are: Ground as much as possible in a star fashion to 1 point. Different current paths to ground rather than sharing the same path, especially the higher current paths. 1 giant ground plane is ussually acceptable as 1 point. Keep signal paths short like you suggested, especially low level and or high impeadance paths(OpAmp inputs). If any radiaded noise will be picked up the longer traces act somewhat like more turns on a transformer and the noise voltage will be higher. Lower impeadance areas of the circuit are less sensitive to noise pickup(Outputs) keep this in mind when you have to make a decision between the two. I ussually get the Rs associated with a high Z area very close to the pin. This leaves the ussually lower impeadance side of the resistor with the longer trace. And diffinatly keep inputs away from outputs as much as possible. I'm little surprised these SMPS guy's don't step right up and teach us all. They are some of the most difficult circuits to layout cleanly. They have all the difficult parameters to deal with on the same circuit. As for the guy with the mic pre on the same board with a switcher, He should be proud, I wouldn't even bother trying!

[ron.eddy]

Thank you for that advice, I used it, along with the other advice to make a new layout for the circuit. I was able to reduce its size by 50% in the mean time. This is odd because I have been looking at this circuit for days and not knowing how to improve it and now with just a couple pointers it is already making much more sense.

SMPS circuits have high frequency to worry about, making it pretty difficult, is that correct? (Excuse for my unfamiliarity with these circuits)

[ron.eddy]

Another question I have involves the ground plane. My grounds in this circuit are kept separate, so as to facilitate their connection to a high quality ground point. With that said, is there any benefit to still using a copper fill on the board and attaching it to the metal chassis (which of course will be grounded)?

I plan on doing it anyway because it will be easier to etch then, but is there any benefits from it? In the picture below you will see the copper pour is not connected to any of the "HQG" connections.





Thanks, Ron

[pinkmouse]

If you use a copper pour, make sure there are no isolated "islands" left on your board, and the copper should always be connected to earth. Power ground is fine, but if you really want to get fussy, you can run it separately back to chasssi star ground.

Star ground all signal earths, and if you have enough copper left, then you can use a ground plane for power grounds.

Swap C9 and C7 around so the smaller cap is nearest the IC pin. that will help with stability.

If this was one of my designs I would have done things slightly differently. I would have started my design at 90 degrees to yours, and run two power rails right up the middle of the board then I would have built the circuit as symetrically as possible, stating with PSU decoupling then moving out, as Mzzj suggests.

Here's a design I'm working on at the moment that shows some of these aspects:

[mzzj]

Originally posted by ron.eddy






I was going to connect them to the main chassis ground via jumper wires. I was under the impression that the ground lead length is not as important as the signal lead length, which I have kept under 5mm as per AD797 datasheet recomendations, so should I also be worrying about the ground trace length as well?

Page 13. fiq. 35. 5mm for ground trace lengt. Try wide ground track under chip and bypass caps over and under chip.

[ron.eddy]

Originally posted by pinkmouse

If this was one of my designs I would have done things slightly differently. I would have started my design at 90 degrees to yours, and run two power rails right up the middle of the board then I would have built the circuit as symetrically as possible, stating with PSU decoupling then moving out, as Mzzj suggests.

Actually, that is exactly how I started out doing it, but for some reason I was running into a lot of trouble with the transistors. So I separated the +15 and -15 to different sides of the board and then laid out semi-symmetrically from there, starting with PSU decoupling. I changed around those caps as you said and they actually fit a lot better this way.


Below is what I have so far (Without the pour), and as you can see the +15 side is above the AD797 and the -15 side is on the bottom. The input is in the center very close to the input pin of the op-amp (I don't know if this is a good idea or what, maybe someone has some input on that???), the output is on the left side in the middle (vertically):

[ron.eddy]

Originally posted by mzzj


Page 13. fiq. 35. 5mm for ground trace lengt. Try wide ground track under chip and bypass caps over and under chip.

Ah, I see. I read that wrong the first time I looked at it. But I was wondering, out of curiosity, why the length of that ground track would be so critical, as it still has a ways to go before the signal going into the ground trace actually gets to earth. I mean, realistically, it is going to be seeing the small trace, the wire to attach that ground to the chassis, then the wire from the chassis to the outlet, then the wire from the outlet to earth. Does the ground trace on the bypass caps have to be that critical given these circumstances? I guess I do not understand fully.

I think I got the caps close enough now to the power pins, but since the lead separation on the bigger of those two caps is 5.08mm, there is no way to get the total path (caps and all) under 5mm, no matter what I do.

On a more general note, when any of you start laying tracks for a circuit board do you break the circuit into functional blocks (i.e. input section) and then base the circuit around those, or do you go more by the schematic and electrical connections? (i.e. as long as they are connected it matters little where on the board they are located (with some exceptions of course))

- Thanks a bunch,

Ron

[pinkmouse]

Hi Ron

I may be a little confused, but I still don't see a star for signal grounds.

The important thing with the supply bypassing for the IC is to get the small caps as near to the power pins as possible, the position of the bigger ones isn't quite so critical.

It may seem silly, but to me, the problem with your board is symmetry, or lack of it. It just looks wrong. The basic circuit is the same for each side, left and right, so why is your board so different from the left to the right channel?

I use a combination of laying out functional blocks aand following schematics, (sort of! ). If you look at my board, you can see the complete blocks for the CCSs on the right, as they are fairly self contained modules, as is the relay driver section on the left. The other bits are just initially roughly laid out to follow the schema, but then moved and adjusted to suit track lengths, clearances, and other design criteria...

[ron.eddy]

The star ground is not on the board, it is actually going to be right next to the mounting position of the board attached to the chassis. I only did this because my grounds were all broken up on the board and were gonnna all need jumper wires to get to ground anyway, so I will just jumper them all to a high quality ground individually.

I see what your saying about the symmetry. I will probably attempt another go at this board tonight or tomorrow to see if I can make one more symmetrical. This is a single channel of the amplifier, so with single sided and given the schematic I could not find a way to make it symmetrical other than a few items (The output transistors, the +/15v inputs, etc). But I will try your suggestion of power and ground up the middle.

Thanks for the advice,

Ron