The Schematic
In this section we will make a schematic using only simple symbols and wires. You will learn one way of how to assign footprints to the schematic as this is required to start the layout.
Starting the editor
Open the schematic editor (EESchema) by clicking on the button for the schematic layout editor (leftmost of the large buttons. See screenshot)
If this is the first time you open EESchema then a window will pop up asking you how you want your libraries setup. Accept the default option. If the default option is not available then you somehow did not install libraries with KiCad. No worries this can be solved
An empty schematic will open for you. I have annotated the important parts of EESchema in the screenshot such that you know how i refer to the different parts of EESchema. In this tutorial we will mostly use tools from the right and top toolbar. All KiCad tools are reachable via hotkeys and we will make use of them (I generally have one hand on the keyboard at all times as i make heavy use of the hotkeys).
Zooming and Panning
First familiarize yourself with the basic interactions of EESchema. Use the mousewheel to zoom. The middle mouse button is used to pan. The default zoom behavior might need a bit getting used to as it centers your view around where the cursor currently is. This is a very powerful feature that allows very efficient navigation of the canvas. If you however find it is too disorientating then you can turn it off in the preferences dialog (Menu bar: preferences -> preferences -> Common -> Center and Warp on zoom)
Add Symbols
With that gotten out of the way lets start making our schematic. We will make a simple non inverting amplifier with the LM321 and a few connectors as the interface. Use the add symbol button 
in the right toolbar (or “place->symbol”) to start the symbol mode. A similar button is in the top toolbar but that one opens the symbol editor.
After that click somewhere on the canvas and the add symbol dialog will come up. Enter LM321 into the filter field and select the symbol from the result by single clicking. You will now see a preview of the symbol and symbol details in the dialog. Double click on the symbol name or click ok to add the symbol to the schematic.
Now the symbol should be attached to your courser. Move it around a bit to get a feel for this. Then place it down somewhere in the middle of the drawing area by left clicking. In the end your canvas should look something like this.
While you are in the add symbol mode you can call the add symbol dialog again with a simple left click. We do just that and add a resistor (R) and a connector (Conn_01x02).
I suggest you use the filter field (the one wher you entered LM321) to find these symbols and get a feel for how it works. For the resistor the searchterm resistor will get you the resistor but not as the only nor first result. But if you observe the results while typing you will notice that the correct symbol does come up after typing r (counterintuifely getting more specific with the search term in this case results in a less useful result – This is admittetly a weird quirk of kicad but well so be it.).
As a further hint: all basic symbols are found in the device lib. Connector symbols are in the connector_generic lib (the connector lib has more specific connector symbols like the ones for a usb connector). It might pay to just look through the libraries in general to get a feeling for what to expect where. And remember everything about the official library including its organization are documented in the library convention https://klc.kicad.org/
Look at the screenshot to see where i added mine. When you added both of them use the ESC key to end the add symbol mode.
Copy Symbols
We now need one more resistor and two additional connectors. We could add them in the same way as we did before but why not simply copy the things we already have. Hover over the resistor you placed and use the hotkey c to copy it (alternatively also reachable via the right click context menu). The copy will be attached to your cursor so place the new resistor just below the first one. Repeat this for the connector until your schematic looks something like this.
Move, Rotate and Mirror Symbols
The rightmost connector is facing away from the amplifier, so we want to rotate it. This is done by hovering over the connector and pressing the hotkey r. You can also mirror the symbol using x or y. Moving it around is done with m. Play around with these 4 hotkeys as you will need them when you start your real projects. You can even use the other 3 hotkeys while you move your symbol around (while it is attached to the cursor). All of these actions are also available via the right click context menu of the connector (handy if you ever forget the hotkeys).
After you played around a bit, place the symbols such that they look something like this.
Make the Connections
If you look at your symbols you will see that they have lines sticking out of them with a small circle at the end. The lines are called pins and the circle indicates that this pin is not connected. We will use wires to create the connections required. For that start the wire tool found in the right toolbar 
.
Like with the add symbol tool nothing happens at this point in time. Move your mouse over the end of the output pin of the amplifier (The one at the tip of the triangle. The end of the pin is what is marked with the circle.) Use left click to start the wire. If you now move the mouse around then you will discover that a green line is following you. Move the mouse to the nearest pin of the nearest resistor and click again to end the wire at this point. The schematic should now look like this.
Now also connect pin 2 of the connector to the amplifiers output pin. (First click on the connector pin and then on the output pin. The output pin no longer has a circle but you can identify the end of it as it is where the other wire already connects.) KiCad will now add a circle where the old wire and the new wire cross. This circle is called a junction dot.
Now connect the rest up as shown in the following screenshot. Notice that we leave the V- pin of the amplifier unconnected for now. You can add additional direction changes while in the wire tool by left clicking where you want this corner. I used this for the connection of V+ to the connector (to get more space for the text above the other connector.) You can start or end a wire anywhere on another wire also by left clicking. A new junction dot should then be generated there as well.
We now only need to connect the V- pin to the wire representing our low voltage potential (The horizontal line on the bottom of the schematic.) There is however no way to do this without crossing some other existing wire (or worse going through a symbol). This is not a problem and will happen in nearly every schematic you ever make. Click on the pin and then on that wire. If you do it right then no junction dot should appear in the wire connecting to the - pin of the amplifier.
Check Connections with the Highlight tool
Now that we made a few connections we might want to double check what is connected. First lets double check that the last wire we just added really is not connected to the feedback connection. Activate the highlight net tool 
and left click on that wire. The result should look like the screenshot. To get rid of the highlight click anywhere on the canvas (where there is no wire).
Get Ready for the Layout
Add Annotation
Symbols in schematics are identified with a so called reference designator. There are different styles how this is done (= lot of competing standars) but most such styles use a combination of letters representing a group of components followed by a number. The KiCad standard library is configured to follow a common rule that is not really codified in an official standard. KiCad however has a restriction that any reference must end in a number.
At this point our reference designators still have question marks in them. Which means they have not yet been annotated. We use the annotate button 
in the top toolbar to start the annotation dialog (alternative: Menu bar: Tools->Annotate Schematic…). We do not need anything special so just accept the default and press annotate. If everything seems ok press close.
Now your symbols should have gotten unique reference designators.
Assign Footprints
In this part of the tutorial we show one option how symbols get their footprints. We also have a more detailed lecture about footprint assignment
Start the assign footprint tool with the button in the top toolbar 
(alternative: Menu bar: Tools->Assign Footprints…)
If you never started anything layout related before then you get a popup informing you that a default footprint library table was created. You can click ok.
The assign footprint tool is split into three columns. The leftmost colum shows all libraries available. The middle column holds the symbols placed in the schematic and their assigned footprints. The rightmost column shows the filtered footprint list.
Move the assign footprint dialog to the side such that you see both the schematic and the dialog at once. Click on any row in the middle collumn of the dialog. The symbol gets hightlighted and the view is moved such that this symbol is in the center.
Notice that the amplifier (reference U1) has already a footprint assigned. This is because the symbol is setup this way in the library. Most symbols you get with KiCad are setup this way and you can typically keep this default footprint unchanged (such symbols are called fully spezified or sometimes also atomic).
Now lets assign the footprints to the remaining symbols. We set the filter options to be “Use Schematic symbol footprint filter” and “Filter footprint list by pincount”. If we now click on the first connector we should see a number of connectors listed in the right column. You assign the footprint to the selected symbol(s) by double clicking on the footprint name in the rightmost column. I suggest to use JST_EH_B2B-EH-A_1x02_P2.50mm_Vertical for J1 and JST_PH_B2B-PH-K_1x02_P2.00mm_Vertical for J2 and J3. You can assign the same footprint to multiple symbols by selecting them at the same time (crtl or shift plus left click to add to the selection)
When all footprints are assigned then we are ready to click ok.
Save your schematic with the button in the top toolbar (or crtl+s). We are done for now.