eagle cad help

[mhartington]

So i got this schematic all built up in Eagle, thanks a lot to gaussmarkov for their awesome parts library. It really made building it much easier than the stock library. Only thing that could make me even happier is if I understood the board layout system. I still want to attempt to do it my self but I am asking for a hand from those who are much more experience than I.

If anyone is interested in helping, PM me and I'll give you the Eagle schematic. I got to give a big thanks to Galego for actually making the schematic. He's on this forum somewhere, hope he doesn't mind.

heres a link to an image of the schem
http://a.imageshack.us/img441/2018/fiftyone.jpg

[taang]

if i understand correctly (i am fairly new at eagle too), once you have a schematic in place, you can create a board with one of the buttons in the tool bar. with the board view mode, you basically have a physical representations of all the parts, with yellow lines to show the schematic "wires". then you have to arrange the pieces in such a way so that you can use the "route" tool to draw pcb traces.

it gets pretty tricky the more parts you have.

also there might be an automated way of doing this, but i have not found it (autoroute does exist, but i can't figure it out)

[DiscoVlad]

Here's a fish:
In the Schematic view click on the "File" menu, and select "Switch to Board". This creates a new board with the components in your schematic to one side.

And here's a fishing rod:
http://dmi.uib.es/~jguerrero/labSistemes/eagle_tut.pdf

[mhartington]

i know how to switch the from schematic to board layout, it organizing the parts and making the final PCB which I have trouble. If there is an auto rout feature that would be amazing and great to know.

[deadastronaut]

I would also know how to do this.autorouting..im just trying out eagle...

i'm actually in the process of doing that very circuit using circuit wizard...which is very simple and instant and.... autoroutes..

[mhartington]

I would also know how to do this.autorouting..im just trying out eagle...

i'm actually in the process of doing that very circuit using circuit wizard...which is very simple and instant and.... autoroutes..

I guess the Autoroute is a feature not available in the lite version of Eagle, but from what i can find out about it, its rubbish. Its good for simple designs and from there if its a simple design, just do it your self.

[deadastronaut]

hmmm. yeah im on the 5.1......free version. i was told it did autoroute...

checkout the circuit wizard...it does me ok...and its nice n simple..like me also..

http://www.youtube.com/watch?v=rYQLWRgC9jw

[aflynt]

I've got the lite version (5.10.0 for OSX), and it does have autoroute. Just click the auto button (second from the bottom on the right side of the toolbar). It's nice for quickly seeing how things could go when you're moving components around, but I find myself not really using it at all when actually running the traces.

-Aaron

[mhartington]

strange, i have the auto button too but when i hit it, i get a little prompt saying its not available in the light edition.

hmmm. yeah im on the 5.1......free version. i was told it did autoroute...

checkout the circuit wizard...it does me ok...and its nice n simple..like me also..

http://www.youtube.com/watch?v=rYQLWRgC9jw

This looks like a great program, wish i could use it but i work from a mac computer and theres no version of circuit wizard for mac

[aflynt]

strange, i have the auto button too but when i hit it, i get a little prompt saying its not available in the light edition.

Have you moved all the components within the board area first? I think it gives a message like that for me if a component is outside the bounds of the board.

-Aaron

[caspercody]

I have asked this question before, when first strating Eagle, how do you start to design the board portion?

Best answer I got was to first start with the ground, and power supply (because these parts have the most connections). And of course keep trying.

The move, and rotate buttons become your friends. Also the change option is very useful. Replace a small layout resistor with a larger layout one. And the ripup button is very useful. This allows you to remove a trace you put on the board, and now want to reroute it.

[edvard]

First, read through Gaussmarkov's blog posts on how to do stuff in Eagle.
http://gaussmarkov.net/wordpress/tools/software/eagle-cad/
I learned at least half of everything I know about Eagle from Mr. Markov's blog.

What I do is lay out the parts more or less in the order they are in the schematic.
Hit the Ratsnest button every few placements to refresh the airwires; the less tangled the final product looks, the more successful your routing will be.
Then I place pots, input/outputs and power supply connections roughly where I want them, move and rotate parts to fit reasonably close together.
At some point I change the outlines to match the size of board I'm shooting for, which usually forces me to move parts around some more.

When that's done, I start routing.
I usually autoroute first just to get a rough idea of where stuff is going, to see if some parts will work better in different places, which calls for a ripup moving parts around and another autoroute.
When I'm happy that everything is placed where it should be and autoroute isn't going to do any better, I'll rip up and hand route; sometimes just a few traces if the autorouter did well or the whole thing if it made an even worse mess.
Remember when autorouting to disable the top layer and set the bottom layer to "*" (it's in the routing dialog that pops up).
Also remember when hand routing to hit Ratsnest often to clean up airwires and traces, especially if you use a ground pour instead of ground traces.

Hope this helps...

[DiscoVlad]

First thing to do in layout view is turn the grid on.

View/Grid... Set Display "on", style "dots", leave size and alt at 0.05, and 0.025, but change multiple to 2.
This gives a grid of 0.1" spaced dots (I find that using grid lines is too visually distracting). When moving components make sure you align the pads to these dots.

Another thing worth doing is set up some Hotkeys (Options/Assign... menu).
In board layout view you're going to be using the Move, Group, Route, Ripup, Split, and Ratsnest commands a lot, and the Package and Optimize commands a bit less.

It is generally a good idea to align polarized components (eg. transistors, ics, etc) in the same direction. For instance if all the transistors are pointed the same way, it's much easier to see if any are in backwards.

Similarly, with things like resistors, its best to stick to one package size and only change that if necessary.

Lay the components out in stages! Think of the circuit as a collection of building blocks.
eg. Move only the components onto the board that are between the input and first transistor. At first I tend to lay them out like the schematic though after a while you get a feel for placement.
The goal at this point isn't to cram everything into as small a place as possible, but to tidy up the ratsnest (those yellow lines between components) so that the lines cross in as few places as possible.

Once the first block has been laid out, do some basic routing. Don't worry too much about power/ground signals yet, but do the short connections between components that are within that block.

Then move onto the next stage and repeat... I tend to use things like Transistors, ICs, and Potentiometers as the demarcation lines.

After a few blocks, move each block (as a group) together, and route the connections between them. At this point you can start trying to compact the space used a little, but bear in mind that the power still needs to be connected.

Other things to look out for:
Try and put all the off-board connections along the same edge of the board.
Try to minimise Jumpers.
Make routing traces as wide as possible
Use DRC early (To set pad (restring) sizes... the defaults are quite small if you're manually drilling the board later 25mil is a good minimum), use DRC often.

Most of all, don't be afraid to scrap a layout and try again differently. It's unlikely that the first one will be perfect, and even then "perfect" is really the best compromise of space and component layout.

There is a very good explanation of some rules of thumb at http://www.alternatezone.com/electronics/pcbdesign.htm it's geared around Protel (Altium designer?) but the principles are the same no matter what software you're using.

[DiscoVlad]

Regarding the Auto-Router; Just. Don't.
For sure, they'll do a better job than an absolute beginner (some times) but their best use is to maximise noise and interference (which in 99.999% of cases you don't want), and they're no substitute for experience... Experience and understanding which you won't gain by using the auto-router.

[taang]

also, fun tip: you can type the name (like r4 or c18) of the component in layout mode (say, if you have the schematic open on the side) to instantly select that part. really helpful if you have a complicated schematic, if you want to layout the parts in order.

[edvard]

...
There is a very good explanation of some rules of thumb at http://www.alternatezone.com/electronics/pcbdesign.htm it's geared around Protel (Altium designer?) but the principles are the same no matter what software you're using.

I love this forum; you come here to give advice, and you end up with some to take back home...
Awesome tip, Vlad!