Thank you! You gave me an alternative to the morning's crossword puzzle! "That (what you wanted) should be easy!", I thought to myself.
And it was... when you discover the trick. There's always a trick.
What you want, as you probably know, but for others reading this, is to create your own FOOTPRINT. (The term "component" has become confused over the years, meaning far too many things.)
The trick is that you are going to make the lines of copper on the PCB with some PADS!... rather strange pads, to you and me, but KiCad thinks they are pads. And KiCad is what matters.
Here we go... I'll do a whole porject, because so often, the context matters...
Started a project from scratch
Drew schematic... SPST switch, resistor, in series between a +12v power component to a GND power component, with 2 "Power Flags"- one on each of +12v and GND.
Then ran footprint editor.... see http://kicadhowto.wikidot.com/tfstart1 http://kicadhowto.wikidot.com/tfstart1
Used "load footprint from library" get a starting point. "Select by browser" helps you find something suitable. I used Discret/ R3, but any simple footprint with just two connecting points will do. (Be careful not, in the course of this, to overwrite the original with your changes!)
First I did what it took to save the unchanged old "R3" in one of my OWN footprint libraries... if you don't have one, see the tutorial at http://kicadhowto.wikidot.com/tfmf1main http://kicadhowto.wikidot.com/tfmf1main. And I gave it a new name.
To accomplish what is in the previous paragraph...
a) Use (top bar menu) "File/ Set Active Library". (If you succeed, you will see the library you though you specified listed as "active library" in the window's title line.)
b) Do "Save Footprint in Active Library". Don't worry... a chance to name it pops up as soon as soon as you invoke that.
So far, so very ordinary, for any new footprint.
So far, in the electrically significant elements which would appear on the board, we have two holes, with copper around their edges, and on the inner surface of the hole, copper connecting the top-side pad to the bottom-side pad. Fine. We need two such things for what we wanted.
Nearly there for our custom footprint! "All" we need are some "lines" of copper, connected to the holes.
Easy enough...
Ha! Or so I thought! Was going strong, 'til now. Thought I was nearly done. "Just" had lay down some "lines of copper"... do that all the time... when putting traces on PCB designs.
But. You can't. You can't put "traces" into components, the way you can put them on PCBs.
What you CAN do, though, is add some very strange "pads"....
Right click on one of the existing pads. Choose "duplicate pad", and drag the new one you've created off to the side.
Get into "Edit pad". Pressing "E" is a quick way; use any way you know.
Change properties thus...
Pad Type: Connector
Shape: Rectangular
Size X: 0.2 mm
Size Y: 25 mm
Be sure Orientation is 0, as I suspect is already is.
Those are the critical ones. You can, of course, choose any dimensions. And you can change them, pad by pad, later, as needed.
When you've laid down enough of this sort of "pad", go back into "Edit pad", and change Orientation to 90, and create what you need of that sort. (One sort will be vertical lines, the other horizontal.) (If you find you don't have enough, put the mouse pointer over an existing one, click ctrl-D, and drag the new one away. (This can be a little tempermental... be sure you have the pointer tool selected, if it doesn't work. Or use right-click.)
By the way... you will have "lost" the original settings for placing pads! (Try adding a "pad"... it will be one of your weird ones, not a normal one.) Yikes! To go back to an "ordinary" pad, just go to one of the "ordinary" pads from the footprint you started from, invoke "Edit pad". (Don't make any changes to the pad's properties.) Click "OK"... and now if you do "Add Pad", it will be an ordinary pad.
Move the lines around, change their lengths, revise the silkscreen, save component! Done!
PLEASE... if you found that useful... go to http://kicadhowto.org/index.htm http://kicadhowto.wikidot.com/ and "share" or at least "like" at Facebook, Google Plus, etc?? (There are buttons for that at the top of that page. Or "promote" that page any other way? Or promote http://kicadhowto.wikidot.com/ http://kicadhowto.wikidot.com/ with the hard-to-spot buttons at the top of THAT page.