# Eagle Schematic and Board layout design for simple opamp module questions

Hopefully I'm not doing anything illegal, I posted a very similar question a few days ago, but this one is different.

Here is what I've been working on the past couple days, trying out different software finally settling on Eagle. Its a simple mic+opamp module that I want to get printed.

Schematic: Board:

I'm not looking to do SMD, just want to create a board where I can solder on DIP/through-hole components. (I have done copper pour ground on both layers BTW)

So the questions I have are:

1.Should I be using curved traces?
2.Are the green rings the copper rings where I can solder?
3.Is there anything missing from the board layout? (I'm sure there is...)
4.This is where I'm concerned: are the part sizes going to be OK? Are the distances the between the holes for parts standardized or do they differ?
5.Have I chosen the right part for the interface pins? I just want 3 holes that I solder wires to.

Thank you!

EDIT (7/28):

@Steven, I re-did the PCB design on one layer upon your recommendation. It turned out to not be all that hard, and it was good practice. What do you think? Although I think I did something awkward here: I put two resistors underneath the opamp IC, beause I figured I could use SIP sockets to elevate the IC and fit the resistors under it. Is this OK?

• I thought you said you weren't a noob... :-) – stevenvh Jul 26 '11 at 17:31
• Your LM358 doesn't have a refdes, so it's impossible to know what the power pins belong to. Also, it's more common to append the A and B to the refdes; now it suggests that they're two different parts of different types. – stevenvh Jul 26 '11 at 17:59
• I'm a little unclear on what you mean, but I assume you mean in the schematic? I guess I could put in a label, but everything hooks up fine with no errors so no biggie. – Shubham Jul 26 '11 at 20:52
• @Fake - Sorry, force of habit. I thought everybody calls it a refdes. It also shows as {refdes} in PCAD until you assign one. And admit that reference designator simply is too long! – stevenvh Jul 27 '11 at 7:45
• You still use PCAD? – Connor Wolf Jul 27 '11 at 8:43

## 3 Answers

1. You're using a strange mix of curved, straight and 45° traces. The point is purely aesthetic for a design like this, but I would try to stick to 45° traces.
2. Yes, they're the solder pads.
3. Not if your PCB netlist matches the schematic's.
4. You'll have to choose actual parts first and check the drawings in the datasheet, or, if you have parts already, measure them. This goes especially for the capacitors, resistors are more forgiving about this (though you'll want to use as much as possible the same pitch for them).
5. If you don't want to place a header or connector there I would place them a bit more apart. You can use a 1-pin header as component.

Also try to be consistent with the symbols in your schematic. You mix American resistor symbols with a European potmeter symbol. (Personally, I don't like the American symbol at all; a schematic with lots of resistors IMO looks messy and frenetic, while the same with European symbols radiates rest & relaxation :-)).

edit
A comment on the double-sided board. This is a design that easily can be done on a single layer. It's worth practicing the layout part of your design. You'll learn how just swapping two components may simplify your routing significantly. For instance the red trace from R6 to the IC can be swapped to the other side by simply placing R6 between R4 and C4. Things like that. It will help you later on when you have more complex designs with hundreds of nets. And it can be fun, too. I like this kind of puzzles a lot. It's like playing planarity.
The problem with this double-sided design is that there are pads which are not accessible for soldering, because they're under a component on the component side, like with C3 or M1. If you don't have plated-through holes you can't be sure the wire is properly soldered to the pad. Worse, if the component's package sits on the pad you can almost be certain that there won't be a solder connection between pin and pad.

• worrying about who is the primary user of the symbol seems trivial to me. Every symbol on that schematic is instantly clear to me. – Kortuk Jul 26 '11 at 17:42
• @Kortuk - so you wouldn't mind that all resistors < 1k would be the zig-zag line, and the others boxes? Wow, you're weird! ;-) – stevenvh Jul 26 '11 at 17:45
• as many I would prefer they were all the same symbol on a schematic unless there is a reason, in this schematic I assume the capacitor that is "american" is polarized and is easy to recognize that way and the two box one is a non-polarized coupling capacitor. that seems to make seeing the schematic a bit easier to me. I am used to both symbolds. On resistors if they chose to change symbols when function changed I would have no problems. Changing with no reason would be a bit befuddling and I would look for the reason wasting my time. – Kortuk Jul 26 '11 at 17:52
• yea I would prefer if the resistor symbols were the same. I dont like how the pot is a box, but it doesnt really bother me all that much as long as I can recognize what it is. I just picked the fist trim pot I could find in the eagle parts list, maybe I'll change it later. But anyways, thanks for the answer! – Shubham Jul 26 '11 at 18:05
• @stevenvh I see, I will try to do this with just one layer. So this is a top view of the board, right? I thought this meant all the solder pads would be on the bottom? Why wouldn't I be able to solder on C3 if its just a through hole? – Shubham Jul 27 '11 at 17:15

I see Steven has already answered the questions you asked, so I'm going to answer the ones you didn't ask.

This looks familiar. Didn't I give you a circuit for this before, but now you've changed a bunch of parts around without understanding why they were the way they were? I'm pretty sure I specified a true rail-rail opamp, which is why biasing it at 1/2 the supply made sense. The LM358 needs something like 1.5V headroom on the high side, so is only usable from 0 to 3.5V with a 5V supply. That means it should be biased at 1.75 volts, not 2.5V. You can fix that by changing R5 and R6. Better yet though would be to use the right opamp.

The parallel combination of R5 and R6 are going to load the output of C5 a significant amount, especially if R7 is set to its maximum setting of 10 kΩ. There is no need for such a low impedance. You can easily make R5 and R6 100 kΩ each, for a total of 50 kΩ load on the microphone output. If you insist on sticking with the LM358, then make R5 180 kΩ and R6 100 kΩ.

You are asking for a gain of 100 from the first stage and 11 from the second. You want to keep the maximum gain per stage down. If you really want the gain of 1100 as you have now, give each stage close to the square root of that. R3 of 330 kΩ will give the first stage a gain of 34. That should be enough if the second stage has a gain of 34 too.

For no apparent reason, you decided to reduce the feedback impedances around the second amp by a factor of 10, but didn't adjust the capacitor accordingly. R4 and C2 form a high pass filter with a rolloff of 16 Hz. That's reasonable. However, R1 and C1 will now roll off at 160 Hz, which is well into the audible range. There is no reason the two stages can't be the same. Make R1 10 kΩ and R2 330 kΩ, just like in the first stage.

• Yes you gave me a similar circuit before, and I had to change around the parts because I had a limited assortment of parts, and to get the parts from your schematic, I would have to order them and wait a few days. So I just went ahead and breadboarded it, and it worked ok and I just made some adjustments in software. Then I soldered it. Check it out: youtube.com/watch?v=CPCE1GDdkBU – Shubham Jul 26 '11 at 19:49
• This posting is just for the PCB design. After I get a few samples printed, I can start playing around with the part values and opamps. Olin, I appreciate your advice, schematics, and insight and it has not gone to waste. I placed an order for the parts from your schematic last week and am waiting for them to arrive. – Shubham Jul 26 '11 at 19:51

I re-did the PCB design on one layer upon your recommendation. It turned out to not be all that hard, and it was good practice. What do you think?

You removed the silkscreen! Labels are great. See this article from Sparkfun about PCB design for manufacturability for a more thorough description. Simply put, more silk is better.

Although I think I did something awkward here: I put two resistors underneath the opamp IC, beause I figured I could use SIP sockets to elevate the IC and fit the resistors under it. Is this OK?

Um, perhaps? Planning to mount a high-speed opamp in a SIP socket may or may not be good depending on your application, but I'd be hesitant to do this from a mechanical standpoint unless you really need the space, which you don't. Use up that blank space at the top right of the board, and just run the traces outside of the space.

If you were doing double-sided design, then you might consider putting SMD parts on the backside, but I understand that PTH and single-sided design is comfortable and cheap for many people.

• The silkscreen and labels are still there, just disabled those layers for the picture so the work is easier to see. Don't really have a specific application, just want this to be a module I can use whenever I need analog input from a mic. – Shubham Jul 28 '11 at 21:36
• @Shubham: If your application is audio, the parasitics of mounting the opamp on a socket should be inconsequential. Looking more closely at your schematic, I see that the part values are also quite large, so I should have known this... – Kevin Vermeer Jul 28 '11 at 21:38
• Yes exactly, I wanted to do this on a single side and compact so I can keep the cost down as much as possible. Thanks for the input, always appreciated! – Shubham Jul 28 '11 at 21:39