a short eagle style guide - for the beginners

[duck_arse]

first - put a frame: A4 is good. you get a page-printable size, a box with auto file and date and space to write in. a bonus is the box for version control.
      if you end-up with a small diagram in the middle of a large page, select and drag the whole dia down to the area above the text-box. use the "Wire" command to draw bounding lines on the "Symbols" layer. before exporting to image, use the "zoom select" command to set your corners, then select "Area > window" when the option box appears.

- turn on "Grid" when you're drawing. I use 0.1" and multiple of 4, dots.
- turn on "Pins" in the layers dialogue. this will show you where the wires/nets are wanting to go.
- turn off "Names" and "Values" in the layers dialogue. this declutters during placement.
- fiddle the colours. set the background you want to stare at. then set the layer colours so they provide you with the maximum visual information.

- start placing. I put one resistor, one cap of each size, and one of each type diode/led/transistor/etc. I start with resistors. copy (and place, roughly) the first horizontal each time you want a horizontal, and the first-placed vertical each time you want a vertical. this puts the name and value in the same direction for each part, and also numbers them incrementally, so work your placements in a logical fashion.
  then do caps, same method. copy and place enough semiconductors and pots etc for your needs.
- add a symbol for ground, Vcc, Vdd, V/2 and your choice of + or - 9, 5, 12, V etc. copy the ground, and go across your dia placing them wherever they are needed. same with supply. for inputs and outputs and other fly wires, I "wirepad", copy and place.
- joggle everything into alignment, both horizontal and vertical, in nice straight lines. PLEASE NOTE - leave space between each parts "pins" circle, for the netting to follow. don't overlap the pins, welding the parts together.

- under "Options > Set.... > Misc", set "Check connects", "Auto end net and bus", "Auto set junction" all to on.
- start netting. you really just want to use "wire bend styles" 0 or 4 (on the top toolbar), which are both square. using these two modes means minimal net segments from pin to pin. this makes it easier to move a part in one go, with less cleanups.
  if you need to rotate a part, delete all connecting net segments between, rotate and re-net. this is the only way to make sure it's really right. if you have "junction" dots appearing on pins or in the middle of net segments, check your grid settings or check your parts alignment to the grid dots. the easiest way is just to grab a part and shift it out of alignment with those around it, see if a spiders-web of lines appear around the dot. delete all the segments between the offended pins, and re-nett.


transmogrifox's mosfet latch, modified, as an example.

- select the right parts, or edit your libraries, and save the parts you use over and over. if you want a 2N2222, find that part and use it. you can place a 2N3907 and use the "value" command to change it's type, after a complaint box, but DON'T. it's not worth the hassle of pinout cross-checkings.
- now everything is neat and aligned, go back into layers, turn off pins, turn on "Values" and "Names", and finish the diagram. save often, and don't forget to use the "Errors" function.

[edit: posted example dia]

---- one of our heavy-duty layout users might like to add that part - I'm too out of practise.

[Kipper4]

Thanks Duck. I really need some neatness in my schematics, this will help

[287m]

hohoho, thanks to auto set junction, save my time a lot! i dont know before
i think just diptrace have the feature, now diptrace fully used for 3D preview

thanks uncle Duck! 

[bluebunny]

Nice one, duck.  Have a beer.  Or whatever it is you anatidae favour...

[duck_arse]

(Anas superciliosa) - worms will do.

[do we have no stylish board layouters?]

[bluebunny]

Layouters of stylish boards, or stylish layouters of boards?  (I'm volunteering for neither post.)

[Kipper4]

I'm with Marc. 

edit ; Besides I've never heard anyone complain because PPR made a hand drawn adjustemnt to a schematic. Not that I'm starting to...........

I cant spell for toffee and my schematics are a nightmare. I know what I meant.

[bluebunny]

I find Paul's illustrations rather charming.  And you get stories about tractors thrown in too!  Sure beats watching telly...

[Kipper4]

I concur Marc. Someone should do a PPR schematic mod archive. 

[duck_arse]

colours and changing them.

the eagle schem editor colours default to red for symbols and green for nets, which may prove troublesome for some of our colour-blind members. here's a way to change the colours to what you are most comfortable with.

open a schem.
on the toolbar - "Layer settings" opens an options box thing, with the layer numbers, names and colours. select one of the layers by clikking it under "Name", then "Change".
click the colour swatch displayed between "Color" and "Displayed" to open a box of colours. select the swatch you think you'd like, then "OK".
if the layer number ("Nr") is highlighted on the left of the box, that layer will display in the schem. if not selected, select it now, or you won't be able to see it.
click "Apply" to see the changes in yr dia, and go back and change your selected if it is not satisfactory, otherwise clik "OK" and just put up with it.

there is a number of option colours provided by default, but you may want something else. I did. try as I might, I have found no GUI method of adding colours to the chooser box. it may be possible, I just don't know how/where. if you want to edit your settings file by hand (/home/username/.eaglerc on linux, probably \garble\cobblers\somewhere_else\eagle.ini on windows) you can. look for the section starting:
Palette.0.0 = "0xFF000000"
and go down to where the colours are all "0xB47F7F7F". change only the last 6 hex numbers to suit.

please note: it is my experience that eagle fiddles the colour info you enter such that the displayed colour does not match that provided by your colour chooser utillity. I don't know if this is real or just a trick of the light.

they are your colours, pick the ones you want. enjoy.

[Kipper4]

Thanks Mate.