(spunky music) - Welcome back. Previously, we talked about
why anyone would want to make a printed circuit board
in the first place. If you're new to designing PCBs, KiCad is a great starting point, because it's free and open source. On this episode, we'll
start our 555 badge project, and create a custom schematic
part, also known as a symbol. If your haven't already,
head to kicad-pcb.org and download the KiCad Software. Follow whatever installation instructions are necessary for your operating system. Once you've installed it, open KiCad, and you'll be presented with
the project manager window. This is where we can
create new KiCad projects, organize files in those projects, and launch the various programs that make up the KiCad suite,
like Eeschema and PCBnew. To start our project, go to
file, new project, new project. I like to create a new folder somewhere, to keep my KiCad projects together. So I'll create a new KiCad directory in the documents folder. Here, I'll create another
folder and name it 555_Badge. Navigate into that folder and give your project a
name, such as 555_Badge. A .pro suffix will be added
to the end of the file name. This file is where KiCad keeps information about your project. Click Save. You should see the files in
your project on the left, which at this point, should just be a blank schematic file,
and a blank PCB file. When you're actually creating a board, you'll probably jump back and
forth between several programs For example, you might jump
right into schematic capture, realize halfway through that,
that you're missing a part. So you open the library
editor, make your symbol, and then go back to
creating your schematic. Showing this slightly chaotic process in a video series, is difficult. So we're going to assume
that you've already realized that you need to make
the 555 timer symbol, and start with the library editor. Back in the KiCad project manager, select tools, run library editor. The library editor program
will open with a blank page. We'll want to create a new component, so click the create a
new component button, which oddly enough, does not
have a menu bar equivalent under file or edit. Let's give it the name 7555 and leave the reference designator as U. Originally, 555 timers
were integrated circuits made with bipolar transistors
intended for things like oscillators and pulse generators. They were created in the 1970s and have a sort of cult following among electrical engineers. Since then, various
derivatives have been made, including the 7555 timer,
which we'll be using. This works the same as a 555 timer, but uses CMOS instead
of bipolar transistors. CMOS can operate at lower voltages, which is how we're able
to power our badge project with a single 3-volt coin cell battery. But do keep in mind that CMOS is a little more sensitive
to electrostatic discharge, so just be careful when
you're handling the component. A reference designator,
or REFDES for short, is a combination of letters and numbers, used to identify electrical
components on a board. If you scroll down the Wikipedia page for reference designator, you'll find a list of
commonly used REFDES letters. You'll see that U is used
for integrated circuits, like our 7555, so we'll use that. Click okay to create our new part. Before we start editing anything, let's create a library to
house our custom parts. Click the save current
component to new library button, which looks like a book with blank pages. Navigate to your project directory, which should be named
something like 555 badge. When creating components
unique to a project like this, I like to give the library
the same name as the project. So we'll call this one 555_Badge.lib. Save it, and you'll get a popup, explaining that the
library isn't available until we load it in Eeschema,
which we'll do later. Note that if you wanted
to store your parts in a larger library that's accessible by all of your projects,
you could do that too. But for the sake of learning KiCad, let's keep our parts in a
project specific library for now. The advantage of having a
project specific library, is that it becomes easier
to share your custom parts if you were to upload your project to say something like GitHub. Even though we saved our
component into a new library, we need to set that library
as our working library. That will allow us to
make edits to our part and save it back into the library. It's a little confusing,
but it's a necessary step. Select preferences, component libraries. Under component library files, click add. Navigate to your project directory, which for me, is in
documents, KiCad, 555_Badge. Select the 555_Badge.lib
file, and click open. If you scroll down, you'll see that the 555
badge library has been added. Click okay. Now that KiCad knows where
to find our custom library, we need to set it as our working library. Click file, current library. Select the 555 badge
library, and click okay. At the top of the window, you should see our library file listed. This means that we have it
selected as the working library, and we can now save any changes we make to our part, to that library. Zoom in on the text in
the center of the page, which you can do with the hot buttons, but I'll use my mouse wheel
to make things easier. Right click on the text. Because there are two fields here, you will be asked to select
which one you want to edit. Click field value 7555, which is the name of our
component, and click move. Move the text down a ways,
and click again to place it. Note that you can hover
your mouse over an object like our REFDES, and
press the M key move it, which I'll be doing often
in order to speed things up. Let's move the U designator
up and out of the way for now. Click the add pins button, and click somewhere on
the page to create a pin. This is where it can be handy to look at the datasheet for our part. At the bottom of the first page, we see the 8-pin DIP package,
with pin names and numbers. Pin names give a description
of what that pin does. And pin numbers are used to designate where the pin is on the physical part. Notice that on our DIP package, the numbering starts with
one to the left of the notch, and counts up going down. Pin five is across from pin four. And the numbering continues
going up on the opposite side. We see that pin one is
ground, pin two is trigger. And notice the horizontal
bar over the pin name. This means that the pin is active low, and it can be useful to keep
that bar on the pin name when looking at schematics, so we'll replicate it on our part. You can choose to make
the schematic symbol look like the part here, but
it doesn't ultimately matter. The important thing is that the pin names and numbers match up. Putting the datasheet and
library editor side by side can be very helpful here. Back in our library editor, name the pin GND and
assign it the number one. Don't worry about orientation,
we'll fix that in a minute. The electrical type is really only useful if we're doing an electrical rules check, once we've made the schematic. Most of the time, I find
setting up this check to be more trouble than it's worth, so we can just ignore the type for now. Click okay. Click again anywhere in
the sheet to place the pin. Because we're still in the add pin mode, we can just click on an
empty area in the sheet to create another pin. Name this ~TRIG, in all capital letters. Note that the tilde gives it the horizontal bar over the name. Give it the number two. Click okay, and click
again to drop the pin. Repeat this process
for the other six pins, where OUT is pin three, ~RST is pin four, CV is pin five, THRESH is pin six, DIS is pin seven, and VDD is pin eight. Our pulsing LED circuit is based on a simple 555 timer flashing circuit, like this one from 555-timer-circuits.com. Notice that the pins on the 555 symbol aren't ordered by number. Instead, they're configured in a way that makes reading the schematic easier, with power and ground pins
on the top and bottom, the output on the right, and
everything else on the left. We want to organize the pins to line up with the pins on
the example circuit symbol. Right click on pin one, and
select rotate pin to spin it. Do this once to have the pin face down, just like in the example circuit. Right click on it again,
and select move pin. Place this pin down and
over from the middle line by one grid dot. Hover over pin five with your mouse and press the M key to move it. While the pin is on your cursor, you can press the R key to rotate it. Move and rotate the pin so that it is next to the ground pin, but to the right of the
middle line by one grid dot. I like to keep pins at least two grid spaces
away from each other to allow the text to be easily read. Continue moving the pins
around until they are organized the same way as in our example circuit. If you need help remembering
the hotkeys, press the ? key, and that'll bring up a list for you. While this is a perfectly
usable schematic symbol, we should probably draw a box around it to make it look nice. Click the draw rectangle tool, and draw a box around the pin names, but just touching the inside of the pins. Notice that the origin of our grid is shown by the two
intersecting blue lines. When we go to place the part in the schematic capture program, the part will be attached to our cursor at this origin point. And it will also rotate
around this origin point. Right now the origin is
in the center of our part, which is a good spot. If yours is not, you can
click the anchor tool, and click in the middle of
the part to move the origin. We can tighten up our symbol by moving the REFDES to the
top left of the symbols box, and the part name to the bottom right. There's no real standard as to where these pieces
of text should be, but I like to try to keep custom parts with the REFDES on top
and name on the bottom. And that's it! We just made our first schematic symbol. Click file, save current library. You'll be asked if you want to include the latest component changes. Click yes, and click yes again
to modify the library file. Go ahead and close out
of the library editor. Now that you've seen how to create your own schematic symbol, we're ready to make the full schematic. The good news is that we don't have to create a
custom part for everything. There are libraries maintained by KiCad, Digi-Key, and others, that make our lives a lot easier. But knowing how to make
your own part is very useful for when you need something that's not in one of those libraries. On the next episode, we'll see how to connect our 7555 timer to other parts that are
found in those libraries. See you then. (spunky music)
