2

I am designing a control board for an analog audio amplifier, with a touch screen interface.

This is my first board I have ever laid out and routed and I was just wondering if people check my design look before I send it out to get it printed.

Quick rundown of the connectors on the board:

  • J7 is the 18v AC coming in from a transformer
  • J2 is a 20 pin jtag connector
  • JX is connected to a LCD / Touch screen module
  • J3R & J3L are control lines going to a digital potentiometers to control the gain and the volume

Below is the BOM

enter image description here

Screen capture of the board it's a four layer board with the top inner layer being a ground plain.

enter image description here

Let me know what ever you think. Like I said this is my first time laying out a board so I did use the auto router and the fixed it in some places. I would rather be brutally honest and tell me to redesign if need be, before I waste $66 on a board that isn't going to work.

George
  • 1,396
  • 4
  • 16
  • 33
JWL
  • 118
  • 6
  • A schematic would be very helpful.. Also, it seems like you can lay these out with a 2 layer board with bottom layer mostly being a ground plane. – abdullah kahraman Jun 16 '13 at 18:56
  • Yes, please add at least a schematic. Also take a look at http://meta.electronics.stackexchange.com/a/2520/10157 for other things you can do to make a design review go well. – Joe Baker Jun 16 '13 at 22:05
  • @abdullahkahraman Did you auto-route this board? – Nick Alexeev Jun 16 '13 at 22:56
  • One question, if this is your first time routing, why did you go in for a 4 layer PCB? Looking at the components you can easily do it within 2 layers which will make your board much smaller, components tight together and is highly likely to work. – David Norman Jun 16 '13 at 23:49
  • 1
    And one word of advice, DO NOT EVER USE AUTO ROUTER. A professional will never do that and it is a good learning practice. Just think of it as drawing, the more effort you put on it better the outcome would be. – David Norman Jun 16 '13 at 23:50
  • 1
    Why say "DO NOT EVER USE AUTO ROUTER"? Professionals use routers every day for ASICs, because they can far out-perform humans for large designs. – travisbartley Jun 17 '13 at 01:13
  • 1
    This question lacks a direct inquiry. JWL, we can give better support to you if you can narrow your question down and be more specific. Unfortunately, this site isn't made for "what do you think" questions. – travisbartley Jun 17 '13 at 01:15
  • @NickAlexeev This is not my question? :) – abdullah kahraman Jun 17 '13 at 07:17
  • 2
    @David: Nonsense. A auto-router is a useful tool. Like any tool, you have to know what it can do, when it's appropriate to use, when not, and how to control it properly. It is very rare that I don't use the auto-router on at least part of a board I am designing. Saying to never use this tool is bad advice and sounds more like a religious conviction in the first place. – Olin Lathrop Jun 17 '13 at 12:43
  • Okay well the harshness is what I was expecting. I have scrapped the above design and decided to try a fully hand route a 2 layer board. Once done I will update the question and be way more exact with any questions that i have remaining. Thanks for the insight. – JWL Jun 17 '13 at 14:05
  • @trav1s, You can see what auto route does. I have built countless PCBs but I have never used auto route because it is of no use. – David Norman Jun 18 '13 at 01:16
  • @OlinLathrop, as far as my experience goes, I have seen auto route just makes things worse. Although you can auto route a small segment of the PCB which is fine but not the whole board which is what I was aiming at. – David Norman Jun 18 '13 at 01:18
  • 1
    If you really think auto routers are of no use, then try to route 10,000 logic cells with >90% placement density over 7 metal layers. Oh, and make sure your routing doesn't create any design rule violations, timing violations, or signal integrity problems. And you have less than 5 minutes to do it. If you can't do that, you shouldn't say such sweeping statements, because an auto-router can. – travisbartley Jun 18 '13 at 01:44
  • @trav1s You are comparing apples and oranges (PCB autorouters with ASIC/FPGA autorouters), they are very different things with the same name. Of course you don't hand route an ASIC with 20+K nets, but I do hand-route a PCB with 3K nets and 1K components. If I had a PCB with 20K nets then I might be tempted to use an autorouter on that too. –  Jun 18 '13 at 02:34
  • 1
    Its more like comparing apples and slightly different colored apples. There are autorouters that can successfully perform for PCB, even for small designs, faster than humans. They have to be fed proper rules, constraints and commands though. My point is that sweeping generalizations like "never use autorouters" just isn't rational. Maybe it was 10 or 20 years ago but times have changed and the tools got better. You owe it to yourself to do the same. – travisbartley Jun 18 '13 at 02:45
  • @trav1s This is the internet. Sweeping generalizations are as common as trolls and cat vids. Even so, I have never used an autorouter that can do a better job than I can, or faster (factoring in the time to setup the rules, etc.)-- so I manually route almost every board that I do. And I have used some very expensive and capable autorouters. The one I have now, and used a couple of times, cost more than an SUV. While sweeping generalizations are hyperbolic, it is understandable in this case. –  Jun 18 '13 at 04:30

4 Answers4

3

Just a couple of random points. I didn't do a complete analysis, mostly because what I saw was serious enough to not warrant that.

  1. Switch to SMD ceramic caps. The lead inductance of TH caps makes them practically useless (talking about the normal 0.1 uF caps, not bulk caps).
  2. Might as well switch to SMD resistors, too.
  3. Power traces look very thin. Especally the lines going to the linear regulators.
  4. I have no confidence that you calculated the thermal dissipation of the linear regulators, or that you have a way to cool them.
  5. The vias look very large. Might be able to make them smaller to give you better signal routing.
  6. It is very hard to tell from the picture, but I think that you have vias so close together that they are forming slots/voids in the power/gnd planes.
0

You can use more wide tracks if you have no specific space constraint. Specially power and ground tracks must be as wide as possible. And ofcourse SMD capacitors are more suitable than TH and important thing is that capacitors must be place as close as possible to microcontroller and filtering capacitors to power regulator (if using) ,,, and their must be wide

Muhammad Ahmed
  • 25
  • 1
  • 8
0

You should also try to avoid right angle traces. This will cause an edge on the signal, if you were to hook an oscilloscope to it, which may cause issues

Watch this from sparkfun to cover many of the basics.

Funkyguy
  • 3,558
  • 1
  • 21
  • 45
0

The layout of the crystals doesn't look right.

  1. Per BOM, the X1 is in the R145 package (it's a cylindrical package). In the layout it looks more like HC-49 package.
  2. There a tips for the PCB layout for the crystal on the p.17 of the ST app note AN2867. More discussion on the layout for the crystal can be found in this thread.
Community
  • 1
Nick Alexeev
  • 37,739
  • 17
  • 97
  • 230
  • @JWL Did you auto-route this board? – Nick Alexeev Jun 17 '13 at 02:18
  • Yes, At the time I didn't know that it was such a bad idea to do that. I going to try to relay out the board with only 2 layers and hand route must of the thing. – JWL Jun 17 '13 at 02:45
  • 1
    Using an autorouter for one's very first board is indeed not a good idea. Autorouter has it's uses. But, beginners usually over-use autorouter. – Nick Alexeev Jun 17 '13 at 02:59