CS4397 DAC - Output Stage layout. Advice sought and comments welcome
Oct 8, 2008 at 12:01 PM Thread Starter Post #1 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
I thought I might try the output stage for the CS4397 posted here. So, I thought I would put my new Eagle skills to work and do a board.

I have recreated the schematic here:
os17schre3.jpg


And, here is my layout:
os17in6.jpg


The board is 40mm x 60mm and will require two for the complete output stage.

I have assumed BC550C for Q1, Q3, Q4 & Q6 & a BC517 for Q2, and used the Murata 2200R inductors from Digikey.

You might note that for the output cap I have provided the option to use either a large(ish) film cap (c2) or an electrolytic bypassed by a smaller film cap (C9 & C10). Is this a sensible option and implementation?

This is my first board layout, so all comments welcome.

Cheers
 
Oct 8, 2008 at 2:16 PM Post #2 of 31

Pars

Can Jam '10 Organizer
Joined
Oct 28, 2003
Posts
4,127
Likes
55
No comments on the design, other that to say that if this is for an I-out DAC, its input impedance will be rather high (not familiar with the CS4397).

Some comments on the layout:

1) Q2: add a variant using the same package as Q1/3/4/6 (personal preference)
2) Beef up the trace widths some.
3) Normal convention (at least what I have seen) is for ground plane on top and traces on the bottom layer. Home etching would really be difficult with this as well (any component that covers its pads such as caps, etc. must be soldered from the bottom; you cannot do thru plated holes on a home etched board, so must accommodate these connections thru vias). Any reason you reversed this?
4) I would move the power inputs away from the signal outputs, and try to get them closer to where they go on the board. Really beef these traces up also.
 
Oct 8, 2008 at 2:38 PM Post #3 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
Thanks Pars. The CS4397 is a V out DAC.

My intention was to get some boards made rather than etching some. So, I hadn't really been thinking about the solder pads being on top on a home etched board. I take your point. If there's no need to have them on the top, I'll just move them to the bottom layer.

I'll make the other changes you have suggested also.

Cheers
 
Oct 8, 2008 at 3:19 PM Post #4 of 31

00940

Headphoneus Supremus
Joined
Nov 6, 2002
Posts
4,493
Likes
45
At first sight, I'd replace Q4 by a led and use it as reference for another CCS instead of R8.

Also, at the bottom of R6, you have tracks crossing at less than 90°. It's rather bad practice.

I'd have to think a bit more about it but it seems to me that you'd also want Q1 and Q6 very close to each other (touching even)
 
Oct 8, 2008 at 3:42 PM Post #5 of 31

Pars

Can Jam '10 Organizer
Joined
Oct 28, 2003
Posts
4,127
Likes
55
Good comments 00940, particularly the thermal bonding on Q1/Q6.

There appears to be something wrong relating to Q2. The base and collector both appear to be connected to V+ when per the schematic they should not be. I'm trying to figure out the blue trace running from the bottom end of R6 to pin 2 of Q2? The bottom ends of R4, R6 and R5 are also connected together (red trace) for V+?
 
Oct 8, 2008 at 4:21 PM Post #6 of 31

cobaltmute

Headphoneus Supremus
Joined
Jul 2, 2008
Posts
1,612
Likes
13
R6 is tied to V+ on both ends, which is not correct per the schematic. The "bottom" end of it should only got Q1 and Q2.

Polarity is backwards on C6 compared to original.

I don't have the knowledge to explain this right, but Q1 is drawn in facing the wrong way, so the connections to it appear to be wrong.

Q3 is the same as Q1.
 
Oct 8, 2008 at 5:04 PM Post #7 of 31

Pars

Can Jam '10 Organizer
Joined
Oct 28, 2003
Posts
4,127
Likes
55
The net or connection in the schematic between V+ and R6 must be connected to the perpendicular connection to the base of Q2 even though there isn't a dot there. That is not correct as they should not be connected.

C6 is wrong in the schematic... the + side should connect to ground and the - should go to -12V.

The BC550 pinout is C-B-E if viewed from the top with the flat facing down. This is correct on the board layout for both Q1 and Q3, so they are fine. Q1 collector goes to R3; Q3 collector goes to R1 and base of Q4.
 
Oct 8, 2008 at 10:53 PM Post #8 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
Thanks heaps guys. Your responses are very helpful.

I'd rather not mess with the part selection (except for C6 being upside down), apparently the circuit is well regarded so I'd rather not change it.

The pinouts for the BC550 had me confused for a little while so I'm pleased to see that that they appear to be correct.
 
Oct 9, 2008 at 5:41 AM Post #9 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
Here is the latest version.

os21ui8.jpg


I have changed the orientation of C6, the package of Q2 and the position of R5. I have increased all of the traces to 1.27mm (50 mil), and moved the majority of the traces to the bottom layer and shifted the ground plane to the top.

The large C2 cap is in the way for moving the power connection pads closer to the circuit. I would prefer to keep the option of the large C2 cap. Any ideas?

Additionally, I was thinking of connecting the output stage as in the following diagram. I'd be taking signal ground from the DAC rather than the output stage. Does that seem reasonable?
connectionsnw6.jpg


Cheers
 
Oct 9, 2008 at 7:08 AM Post #10 of 31

error401

1000+ Head-Fier
Joined
Oct 11, 2006
Posts
1,244
Likes
11
Quote:

Originally Posted by fordgtlover /img/forum/go_quote.gif
The large C2 cap is in the way for moving the power connection pads closer to the circuit. I would prefer to keep the option of the large C2 cap. Any ideas?


I wouldn't worry about short power traces that much. The decoupling caps are close enough to be effective for dynamic currents and the absolute voltage is totally unimportant. You might reroute things so the power supply traces go directly to the power caps, with traces from the caps to the components. This is how the current should flow, keeping the impedance aligned so that occurs is a good idea.

Quote:

Additionally, I was thinking of connecting the output stage as in the following diagram. I'd be taking signal ground from the DAC rather than the output stage. Does that seem reasonable?


Not sure what you're trying to show with the diagram, but what you're describing I don't think is a good idea. Use the output stage ground, which is where the current needs to return to (the dynamic load current will be sourced by the decoupling caps, and that is where it must flow back to). Using the DAC output ground risks polluting that ground with signal currents (which induce a voltage, obviously) flowing back from the load into the decoupling caps on the output board.
 
Oct 9, 2008 at 8:54 AM Post #12 of 31

error401

1000+ Head-Fier
Joined
Oct 11, 2006
Posts
1,244
Likes
11
I like that layout a bit better. I think you can get rid of at least one, and probably both, top-layer traces if you move and rotate R8 between C5/C6 and C2 and route the power traces between its leads, though there aren't any important ground current loops that're getting diverted here I don't think (depending on where you put your output ground pad). C5/C6, R4, R6 and Q3 will probably all have to shift slightly to make room, but I think it should fit.

I would advocate the connection in the new diagram, it should produce better results. Make sure you place the ground pad on the output stage board such that it has an unbroken straight line path to the decoupling caps (the power supply 0V should too, which your current layout does), which means on the current layout that you should put it in between the power traces. Are you using a separate power supply for the DAC?

Edit: I was absent minded about moving the power pads and for some reason concentrated on impedance. These probably should be on the other side of C2, close to C5/C6 as Pars suggested initially so they have minimal influence on the output signal trace running right over top of them. The output is a low impedance trace so it's unlikely to make a difference, but it never hurts to keep other stuff away from it. That is, if you can afford the board area increase, it's hardly a critical issue.
 
Oct 9, 2008 at 12:40 PM Post #13 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
I've moved the power pads and have all routes on one layer
smily_headphones1.gif
.

How is this looking?
os25rk5.jpg


Does C2 need to be 10uF, or would a lower value be OK.


I will need to use a separate PS for this board. Although, I don't yet have one. Would it be OK to run both board from a single dual PS, such as two TREADS, or would it be preferable for each board to have its own PS?

I assume this output stage won't draw much current.

Cheers
 
Oct 9, 2008 at 2:11 PM Post #14 of 31

Pars

Can Jam '10 Organizer
Joined
Oct 28, 2003
Posts
4,127
Likes
55
That looks good. You might consider making the board larger and spread things out a bit... I know when I do layouts it seems like I get antsy to pack everything in as tight as possible. When I actually go build it I wish I would have left more room
rolleyes.gif


Have you considered putting two circuits together... i.e., make a stereo board instead of two mono boards?

You should be OK on a single dual power supply. I did have one issue with the buffers I placed on the rbroer I/V stage that I use in that with a single dual supply (o22 modded), I got really low stereo crosstalk that I traced back to the 2SK170 buffers through the rails. Looking at how Pedja Rogic uses them in his tda1541 DAC, he uses sep. 7812/7912 regulators (TO-92) per channel feeding the 2SK170 buffers to isolate them from the rails. For now I just use it without the buffers and it works fine.
 
Oct 11, 2008 at 10:31 PM Post #15 of 31

fordgtlover

Headphoneus Supremus
Joined
Nov 29, 2006
Posts
2,757
Likes
46
I'm actually going to make the board a bit smaller to get a better deal on the board making from Olimex. I've had to reduce the board from 60mm wide to 50mm to fit 2 boards on one panel. Unfortunately, I have had to delete the big C2 cap. I found that most 10uF caps wouldn't fit anyway.

Hopefully, stuffing the board won't be too much of a problem.

Yes, I had always planned to make it a stereo board, but wanted to get one channel laid out and then just copy it for the second. This is almost finished.

I'll try a single dual PS based on a simple LM317/337 arrangement. Hopefully, it will be OK. Otherwise, I might need to use a single transformer and a power rail per connection. I'll perfboard this while I wait for the output stage boards to be made.

Thanks one again for your help
smily_headphones1.gif
I'll post the board when I get them.
 

Users who are viewing this thread

Top