PCB Layout tutorial

[add4]

I have spent a few hours playing on eagle and i'm always stuck with the same issue : i can't lay all the component on a board and connect everything without jumpers, on a single layer.
I practiced on small boards, that works more or less ok. but boards with more than 10-15 components are just too hard to do for me..
I practiced by copying the layout of some of brian's pcbs, replacing the same component at the same places, and routing it, to understand how he does it.
But it's still not progressing, i really feel stuck.
If Brian, or any of the guys with experience in that field, could make a small tutorial, or explain how he does it, what is positioned first, methods to solve current trace conflicts, give guidelines, anything, i really would be extremely interested in that.

Peace.

p.s. i know about r.g's book .. i asked it for christmas, and it's out of print at the moment ... 

[LaceSensor]

What's up with a jumper or two? Keep working at it.

If anyone has eagle libraries I wouldn't mind trying my hand at it...

[add4]

It's usually much more problematic than a jumper or two
and it's a question of getting it right too. the main problem is that when i rearrange everything to fix one problem, two others arise..

The way i try to work so far is :
1: place the critical components : the more connections they have the most critical they are
2: work from them building up blocks of circuit.

The main problem with that approach is the connection between blocks of circuits which is not easy to do at all

There was a link to Brian's own libraries on the forum :
http://www.madbeanpedals.com/forum/index.php?topic=3133.msg27085#msg27085
on the post where he shared them, Brian said his libraries were an evolution of the gaussmarkov ones..

What's up with a jumper or two? Keep working at it.

If anyone has eagle libraries I wouldn't mind trying my hand at it...

[jkokura]

I'll try and work something up on this for you tomorrow. It's too late for me tonight, but I'll work something out in the afternoon or evening tomorrow.

Realistically though, it's a lot of personal style and trial and error that taught me. And perseverance - don't giving up.

jacob

[LaceSensor]

cant see any download on that link to the libraries...

[add4]

you should be registered on the circuitworkshop.com forum to see the attachments.
I didn't posted it here earlier because i don't know if Brian would be ok with it, but i guess that if he did post it on another forum, he would agree to have this file on his own forum too...
I just attached the mad bean library and the gaussmarkov library too which is also openly downloadable on his website.
hope you enjoy

cant see any download on that link to the libraries...

[add4]

That would be great! thanks in advance..
i don't plan on giving up, but i feel the frustration of not succeeding a few times in a row..
maybe i'm asking too much too, i'm trying to do pcb mounted pots too, which introduces a lot more constraints on the pcb design.
but still ... some rules, general ideas, and tricks for the design would be great.

I'll try and work something up on this for you tomorrow. It's too late for me tonight, but I'll work something out in the afternoon or evening tomorrow.

Realistically though, it's a lot of personal style and trial and error that taught me. And perseverance - don't giving up.

jacob

[jimmybjj]

here is a book on the subject. Not eagle specific but still a pcb layout book.

http://www.smallbearelec.com/Detail.bok?no=679

[add4]

Thanks for the information jimmy, but as look at my original message on the subject:
"p.s. i know about r.g's book .. i asked it for christmas, and it's out of print at the moment ... "

I'm aware about this book ... but i thought it would be interesting to share additional informations about this, not necessarily a ripoff of this book... i don't even know if it's any good and helpful as a learning tool...
but i thought that having some free, additional informations about this fro the experimented layouters would be very interesting.
If you have an opinion about this book, i'd be curious about it too..
Peace

here is a book on the subject. Not eagle specific but still a pcb layout book.

http://www.smallbearelec.com/Detail.bok?no=679

[jimmybjj]

My apologies, I didn't catch that last line.

[add4]

No apologies needed :p thanks for bringing more informations in!
i was really only trying to be sure that the topic wouldn't be closed after someone mentioned that book..
since it isn't available at the moment, and that i'm sure a lot of other people have interesting experience into that..
and i'm sure lots of people also would love to have that kind of help
Thanks for helping again

My apologies, I didn't catch that last line.

[bigmufffuzzwizz]

I'll try and work something up on this for you tomorrow. It's too late for me tonight, but I'll work something out in the afternoon or evening tomorrow.

That would be very helpful, especially with the last steps. I hope to see this one day! 

[jkokura]

uh yeah, yesterday ended up being busier than I expected. I'm just checking in at lunch time today. I will try and get to this ASAP.

jacob

[jkokura]

Ok, here's my go at things. This is an informal tutorial, and will need to be rebuilt/redone to be a true and proper tutorial. I'd love to find a good video screen capture program and then do a series using my copy of eagle. Maybe a better way to consider this post is as a series of tips.

1. Make sure your schematic is correct. Doesn't help to have a mistake in there to have a problem with making your board. I once wrestled with a layout for HOURS, then I went back and found I had forgotten to make a connection, which once I had fixed solved all my problems.

2. A Layout is truly never finished. You can always tweak, always move parts to make it simpler, cleaner, more aesthetically pleasing, smaller, wider, whatever. The point is, don't kill yourself for the small stuff. Songs are the same way - at some point in time you have to call it 'done' and use it. You can go back and revise later, but once it's good enough start using it.

3. Parts can be turned many ways! I got stuck on a layout because I kept trying to leave my resistors 'up and down' when I should have been trying all sorts of directions. Don't forget to try 'sideways'

4. Check out the 'package' feature. Sometimes, you need to make a resistor reach to 4 holes instead of the usual three, or sometimes it could be a diode that moves to 2 holes and stand on end. Don't be afraid to make a part stretch or squish a bit, it can really help with a layout.

5. Remember that the PCB is always in REVERSE. When you do a layout you always have to remember that the enclosure is backwards usually. That means that if on your pedal you want the knobs to read "level, tone and gain" left to right, you need to make your pots on your enclosure left to right "gain, tone and level". It's in reverse. If in should be on the right of the enclosure, then on the PCB it should be on the left, and so on and so forth.

6. Here's the steps I usually take when I build:
a) I know the width I want to work with every time. I use prearranged drilling patterns in specific enclosures all the time. So that means that everytime I load up a schematic ready to do a layout, the first thing I do is edit the width of my enclosure to 2.3 inches. If you want to use a 1590B size width I believe it's 2.15 that you have to get down to, but 2.1 would be a good size to go to if you want that enclsoure to work for you.

b) I set up my ground plane right away. In the bar at the top I type in "poly gnd". Then I start at the top left and just inside the boundaries I trace the internal dimensions of the PCB, whatever the height and width is. This can be adjusted later, so don't worry about that at all.

c) Sort your In, Out, Gnd and Power pads next. I usually will stay 150 mils inside the boundary with my pads. This leaves room for your ground plane to go all the way around the edges unless a trace takes it's place. I also will have up to 3 different gnd pads on my boards. One is for the switch, one is for the DC jack, and one is for either the in or out jack, the other of which connects though the enclosure. It's cool to have the +/-9V pad up at the top of the enclosure for me because I put my DC jacks up top, but if you have your DC jack down by your switch it would be better to have it on that side.

d) I put my pots into place at the same time as the Pads. I use PCB mount pots all the time on my layouts. I also like to have the pots stick up from the PCB, not under it because of how my jacks on my enclosures go. That's me though, you don't have to do it that way. However you DO need to think about how you want your PCB to sit on or around your jacks in the enclosure. I HIGHLY recommend PCB mount pots for layouts. Pay attention to the way that the Pot's pad numbers orient. Also note that you need to make sure the pots are the right distance from each other and that they will properly sit inside the enclosure. Many knobs have 3/4" skirts, so putting the pots 750 mils from each other would make it impossible to use those knobs, you have to move to 775mils at least. Also don't put a pot so that it would have to fit in a hole too close to the edge of the enclosure, because if the pot can't get in a hole on your enclosure...

e) I will usually start moving parts over one at a time and I usually start with the input section. Hide the layer with the part values, take a printout of the schematic with the part numbers on it, and start with the part right after the input. It's usually a resistor to ground or cap in line, or a series of them. Whatever they are, move them over to the area by the input pad and begin to lay them out in a way that makes sense. Hit ratsnest a lot, and the layout will start to emerge as you turn parts and maneuver them around.

f) Sometimes I get to a dead end, and I'll then switch to the output section, or the tone section, or whatever. You can start at a pot lug and then move on from there, or from another pad (Power, Out) and work on that part. Sooner or later you're going to work it out.

g) All of this seems obvious, but truthfully it's not the hardest part. The hard part is when you've done all this and it's still not working. At that point, you have to start getting creative. When you get to a point that it's getting toooo crazy and you can't make it work, save it as a layout version and start over again. Sometimes you get to a point where you've done all you can, and you can't make it work. Usually it's because a trace needs to be made and there is NO way to make it. If that's the case, consider adding jumpers. To add a jumper, you need to create two 'via' pads, which you then name to the same name as the connection on the board. Once that's done, you can arrange them on the PCB however you need, and then just leave the airwire on the PCB unconnected.

h) Sometimes you just can't do a layout on one layer, at least not in the size of PCB you want to use. Any layout is theoretically possible if you have unlimited space, don't care about using jumpers, and so on, but in that case you may as well not be using Eagle, because you could use perf, or turretboard, or whatever. Eagle is helpful for making tight layouts that you etch.

i) Finally, you can try and go with a two layer board. There are places you have them made if you really want. To do so you would... wait for a true tutorial or figure it out for yourself!

Jacob

[gtr2]

Nice work Jacob!  Your post should be a sticky in the members tutorial!

Josh