Build Your Own Clone Message Board

I tried to use MB board as a guide to see if I could reproduce it in Eagle. I know my layout isn't as tight and I'll need to make the traces thicker. I ran autoroute and it gave me this below. I know most of you hand route. Since it's an existing layout, not sure why there are so many crossing traces, even after I ran ratsnest. Should I undo the autoroute, or alter this layout?

I'd rip it up and route it all by hand. Currently you have a double layer board and that's not something you'll likely want to DIY etch (though it can be done). By doing it by hand you'll start to develop a skill set that not many have (which gives you flexibility in the projects you do), and you can make a board that is single sided and can be etched with very little trouble. I'm sure the autorouter is a powerful tool, but there are alot of parameters to change to optimize it and that would take more time/skill than doing the routing by hand. Also judging by the lack of traces going to two of the leg of each of your transistors, there's an error on the schematic that need to be fixed.

You can eliminate several traces by using a ground plane on the bottom layer and a +9v plane on the top.

But yeah, you should route a circuit that small by hand, in my opinion. The air wires show you exactly where to run the traces, so it's not like you have to look at the schematic or even remotely understand what the circuit is doing in order to make a viable layout.

The thing about Eagle's auto router is that it only works well if the user has placed the components on the board in a logical way. And if you have enough experience to place them properly, you probably also know how to route it. So it's kind of a worthless feature for our small circuits.

DipTrace, on the other hand, has both an auto router and auto parts placer. It optimizes placement for the shortest possible traces and then routes everything. Pretty cool.

+1 for routing your own traces. I can also see that you seem to be missing some traces off of the 1M resistor, lower left corner, and the 47u electro cap lower right corner. Also the one trace that does come off that 47u seems to touch the right hand pad of the 1K resistor that is right there, you might want to check to see it it is supposed to. The other thing I notice, is there is a number of spots where traces are coming too close to pads for my comfort, and definitely too close for home etching, like that blue trace that goes across the top from leg 1 of the fuzz to leg 1 of the vol is too close to the 9V pad, and the other pads of the vol pot.

This is a link to the first in a series of tutorials on Eagle, it is really great and well worth going thought the whole thing. It will take you through routing traces, pouring ground planes, etc. http://www.youtube.com/watch?v=qG0O9LKH-_E

Thanks guys. Sure enough, I double checked the schematic and turns out I had quite a few errors. Ran the erc and it pinpointed the issues. I didn't have some components connected, even though it looked like they were, or I had pins overlapping. Anyway, I'm error free now, so I hope to work on this over the weekend. I did the layout like Bean's to use as a guide to help, but I wonder if I shouldn't just do my own. That way I'll have a finished product that's actually mine to do whatever I want with.

As always, thanks for the help.

Ok, so I'm working on the layout now and like the idea of both pots being at the top. All the other pads will be around the edges. Do you guys use any other conventions for the layouts you do? Do you start with the trannies in the center since they have the most connections? Start from the pot pads since those placements are predetermined? What would you recommend?

I usually place the in/out pads, 9v/GND pads, and the pot pads first. But be prepared to end up having to move it all around a bit.

There's no wrong way to do it. I just try to think about what is going to be the most efficient for the person who ends up building a pedal with the board. It's nicer to have the power hookup at the top of the board if you do top-mounted 9v jacks. It's usually better to have the effect in and out pads at the bottom because it's closer to where the footswitch is.

Try cutting out a piece of cardboard and putting inside a pedal, and then think about how you would want to wire it up; where you would want the pads to be. I can do some of that in my head, but I usually end up having to use physical models to get everything just right.


On the 1-layer vs 2-layer thing, it depends on what you intend for the final product. If you want to have the board fabricated, there is no reason not to have two layers, even for a very simple layout. The fab hour is going to go with two layers anyway to accommodate the through-holes. Might as well make use of a power plane and some routing on top.

Ok, I thought since I'm learning routing, ground pours, 9v layer, etc, why not just do a Bazz Fuss layout. Baby steps... I did BF layout a few weeks ago, but I've learned a lot since then, so I just decided to do a completely new layout. Here are the ground pour and 9v layers. It looks right to me. Any critiques?

I just noticed I have a trace from R1 to 9v, and I have a 9v top layer, Since one leg of R1 is the only thing getting 9v, prolly just need to either delete the trace or the 9v top layer all together.

You don't need the trace if the top layer is +9v pour.

You can see if a pad is connected to the net (name for the pour) by looking for the tell-tale "cross" on the pad.




If you have the schematic correct, then you shouldn't see an airwire between 9v and the resistor at all on the board, and therefore you wouldn't have drawn the trace.

The hardest part of Eagle is learning to "let go" and let it worry about the connections.

Thanks CJ. I noticed the same thing (see my post right before yours). If you know you're gonna send a board layout to the board house, you're gonna have your traces along with your ground pour on the bottom layer, and your 9v power plane on the top layer. That makes perfect sense to me. My question is when placing components on the board, how can you do it so the GND and 9V airwires aren't showing up since you know they will have their own layers. Seems to me, if they would not show up, be ALOT easier to do the initial layout, assuming you're using 2 layers.

The airwires are just there to show you how the components should connect. They don't care about being on the top or bottom. You can turn off the layer they are on (forget which one it is) so they all go away if you want. And, once you have the net named appropriately (GND or +9v, for example), you can place the parts on the board and then use the RAT command, and it will fill the polygons you drew (the planes) and also connect all the parts that connect the power/gnd nets. So those airwires will dissappear automatically when you update. It's hard to explain but easy to show. I wish I could find some really good software for recording screen actions so I could do a proper tutorial.

Also, it's important to keep in mind that unless you change it on the board layout, all parts are by default placed on the top layer. You can route them on top or bottom, but they are actually physically on top. If you want to swap one to the bottom side, use the Mirror tool. Click on a part in the layout with Mirror and it will flip it down to the bottom. 99% of the time, you won't do this for through-hole parts, but it comes in handy for board-mounted pots or with SMD parts you want on the bottom.

Oh, ok. I'll try that. I hear Camstudio is a good software to use for that.

Diptrace, what's that CJ?
Edit: http://www.diptrace.com/nonprofit.php

Is this worth learning alongside Eagle too?
I'm a CAD noob and always starts from a schematic so what to do?

Diptrace seems pretty cool. I haven't actually run all the way through a full schematic and layout, but it seems like it is easier to make new parts with Diptrace.

But I'm already up to my nuts with Eagle.

Lol. No doubt. I have spent prolly 100 hrs reading and viewing tutorials for Eagle. I feel that I'm really making some headway, but the initial learning curve is steep. But once you know it, man, it is so powerful. I avoided it because I thought I had to own the professional version to do pedal design. WRONG. The free version works great!

After deciding to do the GND and +9V pours before doing my layout, I was able to do this layout in about 10 minutes (before routing the wires). SO MUCH EASIER, so thanks, CJ and DF for the great insights.



Can you guys tell me what the dealios at the bottom of the board by the pads are?

That means they are too close to the edge of the board, based on the design rules you have set. Run the DRC and it should pop up.


Keep in mind that since you've got the pours set up for both 9v and GND, you can put D1 and C4 literally anywhere on the board (since they directly connect to both 9v and GND). Wherever you move them, it will work.

You have the top and bottom clearances set differently, by the way. I can see that there is more clearance around the pads on the top than bottom. This isn't necessarily wrong, but it's just not uniform.

That occurred to me. Crap! How do I reset the DRs again? I know I did it before...

Reset them? I'm guessing: Tools>DRC>Load>default
Checking: Tools>DRC
And from there you can also edit the rules in the tabs..

less than 2 weeks into Eagle, I'm already trying to dispense advice
I finally made friends with ground/power pours before routing.. finished a board last night.. woo-HOO!

I don't recall doing it that way. I tried that and didn't see anyway to adjust the border.

Here's a zip of goodies for you. It has my current library and DRU file that I use to make all the MBP boards. The library has been stripped down a lot this year, so if you want more parts selection you can d/l my older one from Culturejam's forum http://www.circuitworkshop.com. This library eliminates a lot of redundancy (instead of 10 different dual op-amps with different names, it just has one default dual op-amp for example) and many custom parts I've created as well as re-sized pads which work much better for both manufacturing and etching. My DRU is also in the zip which is pre-configured for manufacturing. Anyone, please feel free to use this stuff as you like for making PCBs.

Doood, thanks Bean!

Change design rules:

In the Board Editor, go to Edit > Design Rules

The main things to look at are Clearance and Restring tabs. Those set the minimum distance between adjacent copper (Clearance) and the width of the pads (Restring).

Once you get it set the way you want, you can save that configuration and then load it each time you start a new board.

Or, you can save yourself some bullshit and use madbean's DRU file.

Lol! Awesome. I also corrected the schematic since a few components weren't connected. I'll post the final layout later.