Hello

I am trying to construct a simple EQ based on a guitar effects pedal design.

I have some questions about the design, layout, and a bit about using EAGLE. I appreciate any tips you may have. I will try to be descriptive to make it easy for you to provide help

The schematic I am going by is below. For completeness, I have also included my eagle files, though these may not be necessary (unless someone wants to check them out!). There is also a screenshot of both, to save you the effort of downloading and loading the files.

I have followed the schematic exactly and built the file in the CAD program. I have replaced the potentiometers with just pads so that I can wire them off-board. I have also included bypass caps for good measure, though I am not sure if I've put them on the schematic properly (according to good practices).
Question: Does my off-board-component strategy seem sensible?
Question: Is my use of bypass capacitors appropriate?

Also, I am planning on running this from a dual 9V supply, so I have provided pads to wire in the battery connectors (offboard), and pads to wire in a switch. The switch is a DPST and makes two connections, one for +V and one for -V, and the middle "ground" is left connected.
Question: Is my use of a DPST switch appropriate here?
Question: Is there a way to use an SPST here?

And finally, on part placement and routing. I have spent a couple hours moving components around, trying to find an "optimal" positioning, but I'm kind of clueless here. Beyond trying to put parts near where they connect, I am not sure what to do. So far every auto-route I have tried only gets around 70% of the traces routed.
Q: Any tips on part placing and routing?
Q: If I have left-over air wires and want to put flying jumpers (or real air wires, whatever they are called), is there a way to provide for a place for them to attach, or do I just kinda tack them on to existing pads and legs?

I hope this post isn't too unwieldy, please throw in whatever info you can.

 

And here are the EAGLE files.

 

I have some questions about the design, layout, and a bit about using EAGLE. I appreciate any tips you may have. I will try to be descriptive to make it easy for you to provide help

Hello, lowprofile. If this is a 1st attempt at schematic/layout, I'd say you've done very, very well.

Cadsoft's Eagle is not particularly easy to learn; there is quite a "learning curve". It helps a great deal if you start off by going through a tutorial. Sparkfun.com has a very good tutorial for Eagle, and it really does not take all that long to go through.

The schematic I am going by is below. For completeness, I have also included my eagle files, though these may not be necessary (unless someone wants to check them out!).

It is a very big help to include the Eagle files. Some of us have Eagle installed, and we can go through making checks, adjustments, etc. I've done so with your schematic and board files; EQ-v2.* are attached.

There is also a screenshot of both, to save you the effort of downloading and loading the files.

.png image files are really the minimum requirement in order to eliminate questions. Without images of your schematic, there will be little to no progress. You have done well by providing both.

Note that you exported the images as .jpg - .jpg is a "lossy" format, and is not very suitable for line graphics like schematics. Please use .png format when exporting; these types of files are not lossy, and the resulting files are both compact and very clear.

I have followed the schematic exactly and built the file in the CAD program. I have replaced the potentiometers with just pads so that I can wire them off-board.

The names for the pot pads are rather long, which will make it somewhat difficult to position the labels on the board, yet keep the board small. I have made the names of some of the pads shorter, yet still descriptive. You might change the pot pad names to something like "P1L", "P1W", "P1R", etc.

I took the liberty to move things around a bit in your schematic to eliminate much of the "white space". This will help when you export images or make a printout, as the text and images of the parts will be proportionately larger than they would be with the white space. I've also attempted to arrange things in the schematic so that the signal flow is easier to follow.

I used the SMASH command on a number of items in the schematic (mostly the pot pads) to arrange them in a fashion where they are easier to read; the pads were moved apart a bit so they did not look all "bunched up". I also SMASHed many resistors and caps in the board so that the names and values would be readable (not overlapping).

I have also included bypass caps for good measure, though I am not sure if I've put them on the schematic properly (according to good practices).

Sure, the schematic placement is fine. You need more caps for the opamps though.

Question: Does my off-board-component strategy seem sensible?

Sure, why not?

Question: Is my use of bypass capacitors appropriate?

Bypass capacitors are always needed.

Also, I am planning on running this from a dual 9V supply, so I have provided pads to wire in the battery connectors (offboard), and pads to wire in a switch. The switch is a DPST and makes two connections, one for +V and one for -V, and the middle "ground" is left connected.
Question: Is my use of a DPST switch appropriate here?

Absolutely.

Question: Is there a way to use an SPST here?

No.

Some more comments:
1) C1 and C8 are shown as polarized capacitors in both the original and your schematic. Since the input and output signals are basically AC, and the polarity across the capacitors will constantly be changing, you must either use non-polarized capacitors, or the design of the EQ must be changed.

2) You do not have the mandatory 0.1uF/100nF bypass capacitors from +V to GND and -V to GND on each opamp. You should add them. I have used the "invoke" command to display the power pins for the three opamps; they are to the right of C9/C10 in the schematic.

And finally, on part placement and routing. I have spent a couple hours moving components around, trying to find an "optimal" positioning, but I'm kind of clueless here. Beyond trying to put parts near where they connect, I am not sure what to do. So far every auto-route I have tried only gets around 70% of the traces routed.
Q: Any tips on part placing and routing?

Have a look at the board. Just for grins, I auto-routed it, then started moving things around, changing packages for resistors to get more room for things, changing trace layers, etc. I also used the polygon tool to add a copper fill area/ground plane to the bottom of the board; this will help to keep things quiet. Many of the traces could be made much wider. I don't like to leave them so narrow. I'm not going to do all of the work though.

Q: If I have left-over air wires and want to put flying jumpers (or real air wires, whatever they are called), is there a way to provide for a place for them to attach, or do I just kinda tack them on to existing pads and legs?

They are simply called jumpers. There is a library for jumpers, called (oddly enough) jumpers.lbr - there are various types/lengths in there.

I hope this post isn't too unwieldy, please throw in whatever info you can.

You did fine.

[eta]
The TL072 is a good old opamp, and still widely used - but there are newer and better opamps available.
Have a look at the MC33078; a dual opamp that's pin compatible - far less noise, far greater bandwidth, rail-to-rail inputs and outputs, less idle current, and not THAT much more expensive.

 

And the topside will look something like this:

(SgtWookie's board)

 

Wow, I am very impressed with the help here! SgtWookie, you are a gentleman and a scholar! nerdegutta, I guess you used some sort of plugin? I heard that that was possible but it is impressive to see!

I understand about the caps, but I'm not sure what my options are **see additional note below**, I have only ever seen electrolytics (which afaik are all polarized) in those sizes. I guess that these are to remove any DC component from the input and output signal. I wonder how these vales were chosen by the original circuit author! From what I know, I guess they would have to be chosen such that their reactance is low enough to not affect the signal. I'm going to look at other similar circuits (guitar effect pedals) to see what other people use. Also notable is that the circuit did function (albeit with a lot of noise/popping) when I built it on a breadboard. I'd like to do things the right way so I'll look into this further.

I have some other design rule files that keep the traces bigger. I'll give them a try.

My choice in op amps comes from making a list of op-amps that would be acceptable for audio use, and then buying the one on the list that was available locally. Now that I have them, I'll use them, and see how it goes.

I was originally hoping to do this as a single-sided board, so that I could etch it at home, but now I'm thinking I can indeed do a two-sided board if I'm careful. I see others have done it! I'm going to go for it.

I have made notes on everything you've said because it's all great info. Thanks again.

*** some time passes ***

I've looked at more guitar pedal designs and the input/output capacitor values vary. I'm thinking I might squeeze through by using a 100nF ceramic on both ends, without fully understanding what I'm doing

 

If you go as small as 100nF, you may find that your output sounds tinny due to low frequency attenuation.

Digikey stocks these 10uF 35v bipolar (non-polarized) aluminum electrolytics for $0.30/ea:
http://search.digikey.com/us/en/products/ECE-A1VN100U/P1187-ND/227628

Google "eagle POVray" for info about the 3-d stuff.