I have this circuit I've designed with a lot of help in this thread. It was designed in Eagle. It's a condenser mic power, preamp and HPF for a guitar.

Here's the simulation schematic.


Here's another layout utilizing the dual op amp.


Here's the layout mode in Eagle


I ordered some PCB's using Gerber files from OSH Park for the first half of this circuit that I got from the university of washington, just the preamp without the HPF. These cost $12 for 3 prototypes. I was amazed at how cheap and easy it was to order PCB's.

I am prototyping this now, although it is challenging to get it in the 1590A box I want (3D printed the box for ease at this point). A printed PCB will make it much easier to cram all the stuff in the available space.




2 months ago I didn't know the first thing about Eagle, but with help from people here I have completed and simulated the circuit. This is the next step. I'd like to work up the Gerber files for this circuit. Here are some questions and limitations I am running into:

1) The pots I'm using are Alpha 9mm, I can't find those in Eagle. What is shown are the standard pots.
2) I need to figure out how to size the PCB layout area. It needs to fit within a 1590A. See pictures.
3) The LED isn't showing up on the layout, maybe because I selected the SpiceSimulation LED?
4) The output jacks are wrong, I'm using a low profile jack that Eagle doesn't have.

Thanks!

 

1) The pots I'm using are Alpha 9mm, I can't find those in Eagle. What is shown are the standard pots.

You can create your own components. It's sometimes easier to modify an existing component.

2) I need to figure out how to size the PCB layout area. It needs to fit within a 1590A. See pictures.

If I understand you correctly, you just move the board dimension layer.

3) The LED isn't showing up on the layout, maybe because I selected the SpiceSimulation LED?

Pick an LED that matches the footprint of what you plan to use.

4) The output jacks are wrong, I'm using a low profile jack that Eagle doesn't have.

See #1.

Your prototype layout isn't very aesthetically pleasing. Having components aligned and either vertical or horizontal looks neater:

You show a ratsnest for the board, but not the actual layout. Layout for the circuit above, even though I handwired the prototype.

I make my boards using toner transfer and use copper fill to reduce the amount copper that needs to be removed.

 

Here's my first attempt at using the layout feature. I got all the components humanly optimized... then hit the autoroute button and it spit out this. 2 layers. I have no idea if this is good or not.

Of note:
1) The board size is 32.5 x 70mm and will fit within a 1590A box with the pots on top and the components on the bottom of the board.
2) 3 sets of pads: 9v, Mic In, Signal Out. Eventually I could mount the Mic and Out jacks to the board.
3) R2 is a dual 9mm pot. R6 is a single. But I struggled mightily in creating custom components in Eagle and the best I could do at this point. Terminals 4-6 on R6 are not connected.
4) Grid spacing is 1.25mm.
5) I don't know if the component sizes are correct, although I did distinguish between the electrolytic caps and the smaller ones.

Please critique. Thanks!

 

1) When there is space, use it. In other words, give all traces space where space allows it.
2) I would use wider tracks (12-15mil).
3) Make power tracks wider (25-50mil). Ground tracks should be extra wide.
4) I would not route tracks in between capacitor and those 6-pin pads.
5) I would not route two tracks in between DIP pads.
6) R8-R10 need repositioning. All nine resistors should align up better.
7) Pay attention to capacitance effect. Two tracks running along side each other creates capacitor coupling.
8) I would renumber all your components so that there is some kind of sequential order.
9) You will find in general that it is easier to route tracks when horizontal and vertical tracks are on separate layers. Use vias when you have to.
10) Finally, PCB layout is called artwork. It should be a piece of art that you can look at and be proud of it.

 

Here is an example of using space where available.

The tracks in A are cramped. B uses the available space. (Also, you can use 45° corners if preferred.)

In the next example, A introduces current loops while the nodes in B are at the same potential.
More to the point, B is more easy to modify if you have to make changes on the finished board.

 

OK, making progress. I fixed the single pot and had previously hooked up the connection points wrong to both pots. Fixed.
The autorouter defaults to 6mil. I can't figure out how to change that, nor how to bulk change traces. But I did manually go in and change everything on layer 1 (Red) to 12mil just to see what it would look like. I probably could fiddle with this all day. Good suggestions.

 

YouTube is awesome, found this very helpful guy who showed me how to group change width.

Both layers are now 0.4mm (15mil). And it has caused a bit of congestion in the resistor bank on the left... I'll have to move a few things around.

 

you should setup the minimum clearances for the nets. this will prevent you from placing tracks too close to other things. there is tons of space, what is the reason that tracks and pads are so close together? look at that mic trace going around output pads or TL072. don't hesitate to rotate parts around to make connections shorter... (for example R8, R13).

also relocate R8,R9,R10 so they line up with other parts.

 

Do this in the rats nest view. There you will be able to better visualize what components can be moved or rotated.
After doing that, lay down the power and ground tracks first.

Post your Eagle files and I will have a go.

 

Yeah I spent a lot of time in the ratsnest view before I figured out how to autotrace. But yes that's the best place to move/rotate parts.

I increased the min clearance on everything to 15mil and made my grid finer so I could manually nudge traces. This has all traces at 15mil (.4mm).

 

that looks much better. i also like to add couple of pads for mounting. small boards may fit snugly into some enclosures but usually this is not an option and i certainly would not want board rattling when one of the parts is a microphone. are you sure that 100k pot in the lower right corner is wired correctly? i see nothing on the middle pad which is normally associated with wiper. i think this is R6 in your schematics and terminals 1 and 2 should be connected to each other. to see if there are any other issues run DRC.

 

There are blue tracks that are hard to see at the centre pins of the pots.

Generally, if you have a choice of which layer to place a track, it goes on the bottom layer.
Thus, for a simple PCB layout as this one, power, ground and all tracks first go on the bottom layer running in one direction (horizontal in this case). Ground should be a flood plane on the bottom layer.

Then you try to place all other tracks on the top layer, using vias as needed.

 

Yes 1 and 2 are common on R6

 

DRC says No Errors. What's the next step? I ran the CAM data. Is it ready for that? I sent off some Gerber files I found to OSH Park a few weeks ago and got prototype boards for $4 each. Anything I should be worried about on this?

 

I adjusted all the names and added the values, added a description and version number at the bottom.

 

Just posting this here, if missed from previous thread:

Active Filter Cookbook; 2nd Ed.
Author: Don Lancaster
ISBN-13: 978-0750629867
ISBN-10: 075062986X

 

Just posting this here, if missed from previous thread:

Active Filter Cookbook; 2nd Ed.
Author: Don Lancaster
ISBN-13: 978-0750629867
ISBN-10: 075062986X

Yeah, someone else mentioned that one. I picked it up used recently, been digging through it!