ON the menu, choose "Library" then "PCB Components".
Then find a component that is similar to the one you want.
Choose "Edit" and then edit this to match how you want your component to be.
Then choose "Library" then "PCB Components" and "Save" - DO NOT HIT OK YET.
Before hitting OK, change the name of the component to match the one you want.
That is simple component creation basing it on an existing component.
Another method would be "File" "New" "PCB Component" and either use the defaults to manually create one
or use the various wizards following a datasheet.
Having made a component you then need to make it into a part.
A part is the linking of a symbol and a component and adding additional manufacturing information.
So you will also need a symbol.
Make one using the above method or the block wizard.
THis can all be done in the design editor.
however to make the part you need to use the library manager.
Open a library, add a new line, name the part, copy the name and add it to the definition column, fill in the description etc.
RMB that line and edit the definition (the defintion "defines how the part is made out of both symbol and component").
In the definition, choose the component, add the stem name (I.E. "R" for resistors, "U" for IC's etc).
change to the symbol tab, add a new gate & double click in it, select your symbol.
in the pins tab, if your symbol terminals match the component pins exactly then highlight the pin column, rmb and assign terminals.
it fills them in.
in the rightmost column put "0" in every field.
Save it.
recreate your parts index.
You now have a part and can add that to a schematic & transfer it to a PCB.
Try the self teach document, or the express DIY document available on the Zuken site.