Eagle PCB Software

[Jaicen_solo]

Ok guys, those of you who are reading my ABC thread will know that I want to design a 3 into one exclusive switcher. Unfortunately, it uses a number of IC's which i'm unfamiliar with, and since I need to get a PCB made quickly, I want to use Eagle to design a nice professional looking layout.
What I need to know is if anyone has any guides for using the program. I can't seem to get any of the components on the schematic other than the 74 series IC's. Where do I find resistors and diodes etc?? Help!
I wish I could go back to multisim. 

[jrem]

do an 'edit/add' to add a device to the schematic, then look in 'descrete' for resistors, caps, and stuff.  Look in  'linear devices' (not linear tech, that's a company) for op amps,  'transistors' for um, well . . .

my big hint . . .   watch the +/- 's on op amps and b/c/e on transistors CAREFULLY . . .     make sure the device you pick in the layout has the EXACT same pin configuration of the device you're using.   Email me off line if you want more info, or find the Eagle bbs . . .

[Andi]

Depending on your version, resistors, caps and inductors may be in "RCL".

[gaussmarkov]

ditto:  most of the components that you need are in the libraries linear and rcl. some diodes are in diode.  there are several transistor libraries.  if you want a cermet-like trimming resistor, look in the pot.lbr library.  when you are adding a component to a schematic, try using the search function to find the specific one you want.  you can use an asterisk for wild card searches.

generally speaking, you have to make substitutions.  to do this, you want to have the component that you are using match the one you plan to use in dimensions and pinout.  for example, you won't find the 1N914 diode in the diode.lbr library.  but that doesn't matter:  any diode the same size will do the trick for layout.  the important characteristics are the physical size of the diode and that diodes have anode and cathode leads.  you can change the "value" of the diode on the schematic so that it reads 1N914 after you place it on the schematic.

you can find package dimensions in datasheets.  the package names in eagle often state dimensions and you can match them.  but note that datasheets for things like film capacitors may not tell you the actual size of the capacitors that you will use.  they list maximum dimensions that are often much larger than the real deal.  the only way that i know to handle this is to have the components on hand when you design your layout.  then you can measure them yourself. 

you may need to create components that are just pads for hooking up voltage supply, grounds, inputs, and outputs.  the supply1.lbr and supply2.lbr libraries have such components but they do not create pads on your board layout.  this is what i did.  if you would like my versions of these, send me a pm with your email address.  it's a small library.  or maybe someone else knows some existing components in eagle that do this and will add that info to this thread.

the only other thing that comes to mind has to do with the length of your leads.  for example, you may want the leads of a resistors to span various distances.  look at the package options inside of a resistor device like R-US_ in the rcl.lbr library and you will see how a single device in eagle can be configured several ways on the pcb.  i always draw the schematic first and then create my layout from the schematic.  when you are drawing the schematic, don't worry about which package you use.  you can choose later when you are designing the board.

and i wasted some time with the autorouting feature when i first started using eagle.  i have not found that very useful and recommend against playing with it if you are pressed by a deadline.

hope this helps!   

[Andi]

Aye - I found the Autorouter quite fun to watch but not terribly useful - my guess is that it works well for complex digital designs, but not for audio. I tend to run the 9v and ground tracks first, then fit around them. Remember you can switch to the top layer to represent jumpers that  hop over other tracks.

[jrem]

hmm, I use the autorouter . . .      put the parts on there as best you can, make the top layer N/A, run the auto router, then use the ripup tool (icon, not the script) and rip up the trace for the component you want to move, move it, then auto route again.  After a couple of hours you can get a complicated board with only one or two unrouted wires.

I've done it the other way (non-auto, when first starting out with Eagle) and have found that the auto router helps keep all the dimensions, clearances, trace widths, etc in line.  YMMV.

[Gilles C]

I agree about using the Autorouter first. It helps when you're now sure about where to put some traces.

I also find it helps to work on small blocks, and then connect them together.

Gilles

[DavidS]

Something that has made me alot happier with Eagle is creating my own component library. By default, the pad and drill sizes for most of the essential components are set to "auto", what this means is that the pads are smaller and the drill sizes larger than what us really useful for making a board at home. Read the tutorial on building your own components (included in the docs you can download along with Eagle), but the fastest way to get things done is to copy the existing parts into your library and just modify the pad diameters and drills to better, fixed sizes. Takes a little bit to get the hang of, but very nice!

[gaussmarkov]

on second thought, i agree that using the autorouter is a good learning tool.  everyone should play with it.  and i missed the option to turn off the top layer.  that's cool.  i will have to try that.  and Gilles suggestoin about working in small blocks.  that's a good one too.  i often forget to do that but it's really effective.

[jrem]

Something that has made me alot happier with Eagle is creating my own component library. <snip> building your own components (included in the docs you can download along with Eagle), but the fastest way to get things done is to copy the existing parts into your library and just modify the pad diameters and drills to better, fixed sizes. Takes a little bit to get the hang of, but very nice!

too much of a bitch when you (I) go from machine to machine.  I just use the DRC (I think, not on this machine) to set up my dimensions, clearances, min drill size, etc, and rock 'n roll.  Also, I tried the create libraries, but then again, dragging them to other PC's is just one more thing.  Using stuff that is there is easier, and making it fit just takes a note in my project log book.  But we all do what works for us . . .

[DavidS]

I didn't get the results I was looking for using the DRC, just couldn't get those drill sizes down to what I liked!

[gaussmarkov]

here's another thought on using eagle:  i now use the command line for certain things.  generally with software i end up learning keyboard shortcuts because i think they can be faster and more accurate.  with eagle, i layout the entire schem with a mouse and then i assign the values to resistors, capacitors, etc. typing in value commands like "value r1 1M" rather than pointing and clicking on R1, switching to the keyboard to type the value and then clicking or tabbing to the accept button.  here's another example,  when i start to lay out the board, i don't use the mouse to drag the components onto to the board one by one.  instead i zoom to fill the screen with just the board and, following the schematic, use a sequence of typed move commands (e.g. "move r1") to bring the parts onto the board (for initial positioning with the mouse).