(Please don't think ill of KiCad because of the resolution you see above. The poor resolution is an artifact of the screen capture process. Furthermore, as you work with KiCad, you should get into the habit of using its extremely user friendly mechanism for zooming in and out, and for panning. These will give you nice, crisp graphics to work with.)
What that shows is a place to connect a battery ("CONN_2", lower left), and then, clockwise around the circuit, a switch, a resistor, and an LED. Of course, there is a wire from the place for connecting a battery, and the wire goes all the way around, eventually coming back to the connector.
The diagram is "imperfect" in many ways… but is the result of a beginner's use of eeSchema to design a circuit, and will suffice for now for our needs.
Here's how I drew that….
To start designing the schematic, click the first big icon on the central project manager window, the one for "eeSchema".
Once upon a time, the first time you invoked eeSchema, you got a "beep" and the following "Not Found" warning….
If that happens to you, just click "Okay". The situation isn't dire… the system is just warning you that there is not yet a file with the schematic in it. Perhaps obvious, but better too many warnings than not enough?
First we'll put an LED, a two pin connector, a switch and a resistor "on the page"….
Be sure the "pointer" icon on the right hand toolbar is selected.
Put the crosshairs in the working area.
Press "A" (for "add component". You can use a lower case "A", "a", but I think the upper case version is more clear here.) ("Component" is a word being written out of Kicad, replaced by "schematic symbol", but as of version 4.0.4 "component" lingered in the tooltip for this.)
Type "led" into the "filter" (formerly "name") edit box. (You used to have to then press enter.) Find a suitable symbol. (The default result from entering "led" is pretty good, if all is well, but explore your options, if you wish.) Click the "OK" button. That should put you back on the page, with a tiny LED "stuck" to your mouse pointer.
Use your mouse wheel to zoom in to an appropriate level. (Don't get too frustrated with the unusual interface until you have mastered it. Different isn't necessarily bad! The KiCad people have "broken the rules" for reasons which, to me, seem good.) (If you need later to find a schematic symbol by using "Select by Browser", things like LEDs, resistors, are in the "Device" schematic symbols library.)
Press "R" as often as necessary to Rotate the schematic symbol to the proper orientation. (Refer to the finished schematic, above.)
Move the LED to the approximate right place. Click to "drop" it there.
Save your work
KiCad, in common with most computer applications, has certain elements of your recent work saved only in the computer's memory, and does not have everything you've done stored on your disk or thumbdrive at all times. If "things go wrong", or you have a simple power failure, your work since your last "save" will be lost.
Feel free to save your work frequently. In eeSchema, the button on the top tool bar (left hand end), and the menu entry under "File" talk about saving your (whole) project, and give you an option of saving a single sheet.
For the moment, your whole project is a single sheet! Don't be put off by the extra stuff.
You can also use the common "save" keyboard shortcut: ctrl-S
(A little aside about the (old) "no file" warning: KiCad uses a sophisticated… but not overly so… system of simple files to pull together all of the elements of your work. As you start working in each module, the file(s) where that module's result will reside are set up. That's why you may get the "file not found" prompts the first time in any project's life you enter a particular module… although I think that "feature" is now a thing of the past.)
Carrying on with schematic design
Press "A" again.
Type "conn_02" (Old:"conn_2"), press enter.
Drop the connector in roughly the right place.
Press "A". Type "spst". Press enter. Drop the switch.
Press "A". Type "r". Press enter. Drop the resistor.
By now, the "Add component" button on the right hand toolbar is probably the one selected. We need the pointer button selected. You could just click on it… or, if you press the "escape" key once… or maybe twice… you'll find that the pointer button becomes the one selected. This is a small example of the fact that there are many ways to do things… and in some cases, the one that "works" is very inferior to another one that you may be failing to look for, learn. If something you "ought" to be able to do seems hard… look for an easy way!
Take zooming and panning. Yes, there are buttons for "zoom in" and "zoom out". And you can use the pane's scroll bars.
Or… just turn the mouse wheel one way to zoom out and the other way to zoom in. The "scene" will pan to put whatever you were pointing to when you moved the mouse wheel at the center of the new view. With a little practice, "zooming around", if you'll excuse the pun, becomes easy and intuitive. Be sure to make the effort to master zooming, because until you do, being in the wrong place, or at the wrong zoom level will inhibit your productivity and raise your blood pressure… and distract you from the things that are hard!
One last comment on zooming: Use it! It is much easier to select things, move them, get them in the right place, etc when you zoom in as far as you can. You can even zoom in to "pick something up", zoom out to move it to roughly the right place, and then zoom back in again for final part placement, or whatever it is you are currently doing.
Schematic symbols present- now arrange…
Right! Zoom out, so you can see all 4 of the schematic symbols we've put "on the page".
We need to pick one as the "anchor", towards which we are going to move the others. We'll use the LED. We will move it down to the lower right of the page; put it just above the [co1leg legend].
(It may pay you at this stage to open a second copy of http://kicadhowto.wikidot.com/se1sch1 this page in a separate window, so you can use that to display the finished schematic, shown above, while you work on creating your copy of it.)
How to move things
Right click on the schematic symbol you want to move. Depending on exactly where you click, you will get one of the following. (Apologies for the fact that the illustration shows a resistor when you are probably wanting to move an LED. They are moved the same way.)
If you get the first pop-up menu, just click on "Component…", and you will find yourself at the second one! (Remember when you see "component": KiCad uses the term very narrowly… to mean "schematic symbol".)
Better yet… instead of using the mouse click, notice the "M" beside "Move". If the pointer button is selected, you only need to put the cursor over the schematic symbol and press M, to pick the schematic symbol up. You may get the "Clarify Selection" step, but that's no big deal. You'll eventually get used to where to click to get what you want.
Once you have done the above, and picked up the LED's schematic symbol, you can move it around. You just move the mouse. If you picked up the wrong thing, press the escape key, and the schematic symbol drops back where it started. If you moved it and clicked, thus putting it down in a new place, ctrl-Z will undo the move. Remember you can zoom out and then back in, on a different part of the diagram, while the schematic symbol is "stuck" to the cursor. To reach the parts that other CAD packages reach differently.
You may sometimes find that after a change, particularly if you've deleted or moved something, that "debris" remains on the screen. A quick slight "zoom out/ zoom back again" will redraw the page, clearing away the little scraps.
N.B.: Sometimes it is critcal to have the pointer button selected. You'll be surprised how often the button selected changes "by itself". Anyway. While you have the pointer button selected, if you put the cursor over a schematic symbol and press the delete key, the schematic symbol is deleted from the schematic.
You can also press the "R" key, to rotate schematic symbols, which you will also need to do with some, to get the schematic symbol as we want them. You'll need to rotate the LED, and do that now.
You can, of course, reach our goal by many routes. In my case, I next set about moving the resistor schematic symbol to a better spot. I made sure that it was the pointer button that was selected in the right hand toolbar, and then right clicked on the resistor schematic symbol.
Put the resistor above the LED. Do it very precisely, so that the little circle at the bottom of the resistor schematic symbol is exactly over the little circle at the top of the LED schematic symbol. Then drop the resistor. The two will be connected. (If you fail to line them up properly, the two little circles on the line's ends will still be present.)
Then move the switch until it connects to the top of the resistor. (Again, if you positioned them just right, the circles on the ends of the lines will disappear.)
Finally, move CONN_02x01 to where you see it in the illustration.
That's it! On to the next step…