I made up a master board. It will attach to two slave boards (the other two amps). This look a bit better in terms of layout and trace size?
http://img220.imageshack.us/img220/6727 … ardqe1.png
Also how important are my grid settings? I had to make it finer to make some of the traces and components fit. Will that be a problem?
SpikedCola:
Also how important are my grid settings? I had to make it finer to make some of the traces and components fit. Will that be a problem?
While doing the schematic, sticking to a 0.1 grid is the standard rule.
While doing the layout, thinks are less clear. I’ll just say what I do.
For component placement, I try to use a 0.1 grid to make the board look organized.
When routing heavy amp traces, I tend to use that grid also. In my past projects, heavy amp was ~100mA. I believe that is nothing compared to your current challenge.
For digital signal lines, I drop to a 0.05 grid with 0.025 alternate. I use whatever works between those two.
For ananalog signal lines, I would probably follow the same. I have not built a heavy analog board, so I have no experience to base a comment. I am just assuming.
As the board layout comes together, I’ll switch to whatever grid I need to fix routing problems or to make things look better.
After writing all of that, I realized the simpler answer would have been no. It doesn’t really matter if you use a finer grid to make it all fit. With an analog board (or fast digital), following best practices is more important than using a “standard” grid.
What is the voltage/current rating on the SMD cap you have connected to the huge power trace? (upper left hand corner, can’t read the number).
It also looks like you have the positive side of the two large rightmost caps connected to the ground trace on the bottom…
Shifted:
It also looks like you have the positive side of the two large rightmost caps connected to the ground trace on the bottom…
That’s correct, and their meant to be…
Yes! Much better. Still a couple of issues to address:SpikedCola:
I made up a master board. It will attach to two slave boards (the other two amps). This look a bit better in terms of layout and trace size?
(1) You can’t use 25mil square pins for high power audio or DC
(2) You can’t place inputs and outputs of an amp on adjacent pins
(3) You can’t sum three amplifier modules into one as shown
Start by removing all the 25mil square pins and using
proper screw terminals rated to at least ten amps.
For a 50Watt amplifier module you will draw about 75Watts
from the DC supplies. At sixty volts you have to deliver
over one amp without local heating or high inductance,
both of which reduce reliability.
Keep the input signal and it’s ground well away from
the output signal and power ground.
In the original design the three amplifier ICs were summed
with 200milliohm resistors, to a common load terminal. The
cables and connections to the summing point will need
to be much lower impedance (such as the fat trace/tracks
on the original board). If one (or two) go to a higher impedance
the remaining amplifier will be overloaded.](http://tinyurl.com/9casb2)
I have one thing to add to the discussion. Universities don’t teach EE students much about wire resistance or inductance. When I graduated with my BS degree, I had some idea about the need for decoupling caps in certain situations, but there weren’t any in-depth discussions as to why they were needed. And that goes the same for designing a circuit board. All of that comes from experience - not university training, in my experience. Those of you that have done this professionally for many years tend to take it for granted that the OP would know that stuff.
bigglez:
Yes! Much better. Still a couple of issues to address:SpikedCola:
I made up a master board. It will attach to two slave boards (the other two amps). This look a bit better in terms of layout and trace size?(1) You can’t use 25mil square pins for high power audio or DC
(2) You can’t place inputs and outputs of an amp on adjacent pins
(3) You can’t sum three amplifier modules into one as shown
Start by removing all the 25mil square pins and using
proper screw terminals rated to at least ten amps.
For a 50Watt amplifier module you will draw about 75Watts
from the DC supplies. At sixty volts you have to deliver
over one amp without local heating or high inductance,
both of which reduce reliability.
Keep the input signal and it’s ground well away from
the output signal and power ground.
In the original design the three amplifier ICs were summed
with 200milliohm resistors, to a common load terminal. The
cables and connections to the summing point will need
to be much lower impedance (such as the fat trace/tracks
on the original board). If one (or two) go to a higher impedance
the remaining amplifier will be overloaded.[/quote]
Points noted. Ill make the changes when my flight gets in tonight. Thanks!Also, in terms of connecting the boards together, should the summing resistors be on the master board or on the slave boards? I was hoping to use a larger conductor (~14ga) to hook the outputs of the slaves to the master to make up for having separate boards, but Im not sure if it will work. Again, this is all a learning experience for me, so thanks for taking the time to help! (all of you)
The - end of the cap is hooked to the V- trace (-30v) so the polarization is correct :)Shifted:
It also looks like you have the positive side of the two large rightmost caps connected to the ground trace on the bottom…I havent actually picked components yet, I just guessed at the components I would be using, assuming I can change the package and board layout later on if I come across something. However, I think I may need to rethink that (and the other 0.1uF caps) as the original design calls for Wima 63v caps](http://tinyurl.com/9casb2)Shifted:
What is the voltage/current rating on the SMD cap you have connected to the huge power trace? (upper left hand corner, can’t read the number).
There will always be holes in a formal education.signal7:
Universities don’t teach EE students much about wire resistance or inductance.
As an undergradute in Engineering school I took
summer jobs in electronics factories to get hands-on
exposure. Also, the program I took had one year
of rotation between school and an industry sponsored
training school, where we learned drafting (technical
drawing), machine shop, electronics lab, and sheet
metal fabrication. Each was on a one week rotation.
For the next four years I spent my summers doing
“grunt work” in factories. I repaired a lot of valve/tube
oscilloscopes, tested and repaired a lot of analogue
multimeters (AVO mk 8s mostly), and also worked
in a calibration lab with national standards traceability.
The OP came here asking for help with a clone PCB
design, and was sidetracked by another round in the
PCB tool wars (of which I’m guilty of doing). After
the OP was given solid advice about basic electronics,
the OP bragged about ohm’s law, and turned around
and presented the same errors in the next version.
You can lead a horse to water…
So what do you suggest that we do next time someonesignal7:
All of that comes from experience - not university training, in my experience. Those of you that have done this professionally for many years tend to take it for granted that the OP would know that stuff.
seeks advice here?
I would hedge your bets on the summing resistors.SpikedCola:
Points noted. Also, in terms of connecting the boards together, should the summing resistors be on the master board or on the slave boards? I was hoping to use a larger conductor (~14ga) to hook the outputs of the slaves to the master to make up for having separate boards, but Im not sure if it will work. Again, this is all a learning experience for me, so thanks for taking the time to help! (all of you)
Use placeholders on each power amp to include the
local resistor. A better method is sum the amps off
the PCB (the speaker connector area would be good
location). With placeholders you can try it out with
the resistors on the PCBs later.
PCB errors are not forgiving. Better to have all theSpikedCola:
I havent actually picked components yet, I just guessed at the components I would be using, assuming I can change the package and board layout later on if I come across something. However, I think I may need to rethink that (and the other 0.1uF caps) as the original design calls for Wima 63v caps
parts on the BOM in the PCB editor first. This may
require downloading and reading many datasheets,
and creating accurate PCB layout footprints.
Probably the least fun part of any project for me!
Found a footprint for a (slightly ;)) larger connector. Also rearranged the inputs and outputs
bigglez:
There will always be holes in a formal education.As an undergradute in Engineering school I took
summer jobs in electronics factories to get hands-on
exposure.
…
After the OP was given solid advice about basic electronics,
the OP bragged about ohm’s law, and turned around
and presented the same errors in the next version.
…
So what do you suggest that we do next time someone
seeks advice here?
I wasn’t attacking you - or at least, I certainly didn’t intend to. I just wanted to point out that though Ohm’s law plays a part in the problems of the design, it’s not a 100% explanation. When someone asks for help, we should help them, not give them a hard time over what they know or don’t know, imho. I wouldn’t say the OP was bragging, but rather just informing us of his background.
… but this is getting off topic.
Those connectors are still way too small! 
Man, those things are giant.
I just started playing with Eagle3D. Lets you see the board and the component placement in 3D renderings. Very cool. Missing a few components, but like this:
http://www.higginstribe.com/z8e/eagle3d-test.gif
I like this discussion. I have no experience with analog PCB theory.
Yeah, I think theyre a bit overkill 
Theyre rated at 19-36A
The OP has a bad habit of editing the original posts.TheDirty:
Those connectors are still way too small!Man, those things are giant.
We have now lost the continuity of changes made to
the original design by the OP. The original use of 25mil
square pin headers was a poor choice. The revised
connectors are better (but undocumented). They are
also too fat for the physical space, hit other part’s
outlines, and allow no room for fingers to grip them.
On the topic of conductor and connector specs, it has
less to do with the physical size and a lot to do
with the contact resistance. For a 150Watt audio amplifier,
driving a 4 ohms load (speaker):
V = IR, I=V/R, R=V/I, P=IV, P= IIR, I = (P/R)^1/2
I = (150/4)^ 1/2 = 6.123Amps (RMS)
For a sub one watt power loss in each connector:
R(max) = Rload/150 = 4/150 = 26milliohms.
Even allowing for 50W per amplifier, it’s connectors
and PCB traces would have to be less than 78 milliohms.
The original design used three amplifiers to drive a
common load (the 4 ohms speaker).
The output AC impedance of the amplifier IC is also
very low (guess at less than 10milliohms).
In the original desing three amplifiers are combined,
with 200 milliohm ‘matching’ or ‘sharing’ resistors.
For this to work at all the three amplifiers need a
very low impedance path to the load. How low?
Much less than 100milliohms!
The use of 25mil square pin headers was just wrong.
In the original article the author used screw terminals
for all external connections and chassis wiring. These
provide the low impedance and low resistance needed
to reliably deliver the heavy load current, heavy supply
current, and equalize the load over six amplifier ICs,
three in parallel, two sets in push-pull or
BTL (Bridge Tied Load).
Here’s an [on-line calculator for trace width.
Here’s the results to deliver 6.2Amps over two inches length:
http://www.stonard.com/SFE/trace_width_1.jpg](ANSI PCB Track Width Calculator)
While ive edited my original post, I kept different revisions saved in my eagle folder, so I can go all the way back to the beginning. Also, the connectors I chose werent exactly for the connector itself, just for the size of the holes (Im thinking of using wire-to-wire to tie the boards together), so this way I dont need to order special connectors
SpikedCola:
Yeah, I think theyre a bit overkill
I didn’t realize you were right close by. I have screw terminals, like the one in Bigglez link on the top of this page, or I’m sure you can get those screw terminals from Sayal Electronics on Gordon Baker Dr.
Sure, *you* can. But new visitors to your thread willSpikedCola:
While ive edited my original post, I kept different revisions saved in my eagle folder, so I can go all the way back to the beginning.
only see the current (edited) image and think the
comments below it are out of context.
It is better to post new revisions independently,
and leave a ‘paper trail’ for others. Posting here
is free.
Okay, but loosing the ability to 'unplug' a module for testingSpikedCola:
Also, the connectors I chose werent exactly for the connector itself, just for the size of the holes (Im thinking of using wire-to-wire to tie the boards together), so this way I dont need to order special connectors
or repair is important. Also, having worked on other’s
wire to PCB designs (commercial equipment) the wires
break off at the PCB interface unless handled very carefully.
EAGLE has PTH mounting holes that make good lands
for soldering wires, if you go that way.
Sorry, youre right, I should be keeping different revisions posted instead of updating. Ill do that from now on. Also, thats a good point about having removeable connectors, Ill look for a screw terminal connector in Eagles library and make the changes. Any other tips thus far?
Newest revision:
http://img218.imageshack.us/img218/6093/121mz6.png
Changed connectors to [these, they are rated at up to 6A](http://www.sparkfun.com/commerce/product_info.php?products_id=8084)
