Our Aleph 2 PCB - Critique please!

[TwangBar]

I and a few other fellows have been working on the Aleph 2 amp (for longer than we would like to admit!). It has been a long slog, what with looking for appropriate heat sinks and so forth.

Anyway, we are now at the stage of ordering our PCBs and would greatly appreciate any comments on our layout (as well as any tips on ordering the boards).

What you will notice is that we are mounting the driver board directly to the caps which will be located at each corner of the board. The transformer (Plitron 1000VA) will be situated in the middle of the four caps directly below the PCB. Also, the output boards will be run at the same time - you can see them on each end of the layout.

If the image isn't great, I can email the dxf or PDF.

Thanks!

BTW: We will be getting pricing soon so if anybody is interested in going in on the order...

[Mark A. Gulbrandsen]

Pretty neat. I'd make the speaker + connection pad large enough for at least 12 ga wire, preferably even larger than that!! Also the fiol trace for same.....and the other side of resistors R-22 to R-27 shuold be very heavy as well. These traces carry the full brunt of the output signal. Too small of trace for the speaker + been a common mistake on may of the PCB's I've seen here. What ounce will the traces be...at least 2 oz I hope and preferably 4!! Silkscreened, solder mask, and what else???? Did I hear you say Gold platinbg too?????
Mark

[Peter Daniel]

The ground path form closed loops, I don't think it's good. You might get hum because of that.

[Scribble]

Id be very interested! but depends on price obviously.. hope they turn out well!

BTW im in Australia for shipping wise.

Does any one know of anyone in australia who does any aleph or zen boards?

Thanks,

[Mark A. Gulbrandsen]

Peter,
I guess they could open up the ground on the right side between the two pads there....put in a couple of more pads to have the option of a continous ground or not. I agree though it may cause some problems in some cases. Also don't know if I'd mount an unshielded toroid right unde the board. Going that route you might end up a bit noisier.....A toroid in a can would probably work out though....
Mark

[fcel]

Twangbar,

1. I'm not sure why you label Q1, Q2 & Q3 as M1, Q2 & M3 and Q4 and Q5 as Q1 and Q2. Why not label them like the original schematics says to avoid any kind of confusion later on.

2. I can't really tell from the picture but you might want to have a little more pin spacing for Q1 and Q2 (per your dwg) so that it's easier to solder. I guess same comment on M1 to M3. May be have the trace "staggered" for the center pin?

3. Again, I can't tell from the picture but you might want to have a wide enough spacing to install a pot for R19 for trimming later. I think the chances of having the bias for both channel to be exactly the same is very slim. So a provision for a little trimming later on is a good idea, I think.

4. If you intend the output boards to be "join" together with the driver board, then why not have the G, D, S and sense trace from the output boards go all the way to the driver boards? That way, you don't need any wires.

5. I personally like "terminal block" because it gives me the option of easier swapping of boards later (without desoldering) and for troubleshooting purposes (i.e. if you have to take out the boards from the chassis for any reason). Do you want to consider that option? If you do, make sure about hole spacing for the appropriate locations.

[MWP]

Why not use a ground fill?
The loops youve created in your ground tracks is not a good idea.

[Soucie]

Hi guys;

I'm one of the guys who did this PCB layout. Someone else did the core layout and I prettied/fixed it up and added the big caps. It's very late for me so I'll make a couple of quick comments right now to get things out of the way. I'll go through the replies more thoroughly tomorrow.

1. the FET boards are intended to be sheared or cut off the main board by us, thus saving the seperate board costs. Then cut the FET boards into 3's (or 2 and 4's...FET's that is). We have 4 sinks just like the real Aleph 2

2. this layout was made a single sided board for cost but I will probably convert it to double sided after all. The point about the small ground loop on the left is valid but the tracks are wide. It's easily changed. The "ring" is more by layout/cap topology so it probably needs a few opinions from people. I was contemplating the ground fill method with a ground plane on the top side(thus eliminating the loop, but passed initially because my arm was getting tired from wrestling Orcad(pro layout software). It's a dog IMHO. But nonetheless I'm sure I can make it work with some effort.

3. this picture(not the actual layout) has several false anomolies from the Orcad to DXF to god knows what to JPG conversion. Plus the input connection tracks fell off for a still unknown LVS reason. I have to rework it.

4. transistor labelling was done by "the other guy". It's based off the Orcad schematic he entered and gave to me. Easily checked and changed

5. forget the gold plating, we are on a budget;-) We'll go for thick copper with solder mask and silkscreen

6. the speaker wire holes fit 12 gauge. I'll double check.

7. pin spacing between Q1 Q2. It's a standard footprint that I have soldered to easily before and is supplied by Orcad(a pro CAD tool). Are people really having problems soldering to this size pin spacing(FET or not)? I know some people don't solder very neatly with their Weller solder gun:-O ba-da-boom....sorry
Opinions anyone??

Ok I think I hit most of the ones that needed clarifying. Keep it coming! I'll look into the other ones such as the trimpot.

Anybody know who the PCB supplier was for the last large order batch of Aleph 2 PCB's? I'll ship the boards pretty well anywhere if they are of use to anybody. Get's our order quantity up and the PCB cost down! And I have a Paypal account if people want to get in on this(plus money orders).....we'll talk....

Thanks
John

[Soucie]

Since I'm here I might as well throw out a question. Does anyone around here have any experience with Orcad PCB layout software from Cadence? I have a few basic questions on some things that are causing me problems. The manuals aren't the best.

John

[marce]

Capacitor ground pads for C1-4 look awfully close to where the boards are going to be cut, even if board is scored and cut with a "pizza slice" pcb cutter you havn't much room for faux pas's.
Ground plane on top would be best option, allow the current to find its own optional low impedence route back to the psu source point.
Dont use Orccad, but do use Cadstar and Pads so may be able to help a little as a lot of the basic techniqes are the same from 1 package to another (Slap the parts down and join the dots )