(upbeat music) - Once you're done drawing your schematic in Eeschema, we'll need to associate schematic symbols with footprints. But first, let's see how to create a custom footprint, should you come across a component that's not in the KiCad
or Digi-Key libraries. For now, we'll assume we
don't have a footprint for the 7555 timer, so we'll need to make one before we can move on
to the actual layout. You may want to create footprints at the same time you're creating schematic symbols. The order doesn't really matter, so as long as you have both of them when you go to associate footprints with symbols. You've already seen the data sheet for the 7555 timer, but I'll show you how to find it for when you're looking
up what parts to use. Head to digikey.com. In the search bar, type 7555. Since the number 7555 can appear in so many different part numbers, you'll want to carefully look through the categories that are shown for the top results. The first one says Clock/Timing, Programming Timers and Oscillators. That seems like what we're looking for, so click on that. The top row shows you a variety of filters that you can select from. You can select multiple filters by holding Control or Shift, and you can clear them by clicking on the Clear
button that appears. There seems to be many options available, and for some of these, we may not know what we want. All we know is that we want a through hole 7555 timer, so click Through Hole to set that filter. There are nine remaining parts, which means we narrowed it down to a much more reasonable list. To narrow it down even more, we can click the In Stock status to see what Digi-Key
can ship us right away. That pares it down to just three. Click Apply Filters and you'll see the three that meet our needs, each from a different manufacturer. What I like to do from here is sort by descending quantity available. Do this by clicking on the down arrow underneath quantity available. This tells you how many units Digi-Key has in stock for that part. In theory, it also gives you an idea of how popular the part is, assuming someone didn't just buy out the whole stock
of something recently. It looks like the Intersil 7555 timer has lots of stock, is cheaper than the others, and will operate just fine on our three volt battery. Click on the part name to bring up the part page. Here, click on the data sheet link. Scroll down. Some data sheets will give you the footprint that you'll need to make, and others, like this one, will just give you the
dimensions of the part. Something like a DIP package is usually so common that it's assumed the footprint is always the same. It'll just vary depending
on the number of pins. You could look up the dimensions for a DIP footprint, but we have enough here to get started. From the Project Manager in Ki-Cad, Click Tools, Run Footprint Editor. In the new window, click File, New Footprint. If you're curious, there is a standard for naming parts and footprints. The IPC is the association responsible for creating standards related to soldering
cable naming, et cetera. If you search for IPC footprint naming, you'll find a PDF showing how to precisely name a footprint. If you're maintaining
an extensive library, and want to make sure
you're meeting standards, then you're welcome to
use these long names. However, for our little project and tiny self-contained library, we'll go with something a little easier. Enter the name ICM7555-PDIP, as that associates our footprint with the exact part from Intersil, and shows that we're using the plastic dual in-line package, or PDIP version. Click okay. Just like when we made a schematic symbol, we need to save this to a new library. Click File, Save Footprint in New Library. Make sure that the base path points to our current project directory, Documents\KiCad\555_Badge for me. Give your library folder a name, such as 555_Badge. Note that .pretty will be appended to the folder's name, as that's how Ki-Cad will know it's storing footprints. Once again, we'll be making a library that's unique to our project, but you're welcome to
store custom footprints elsewhere on your computer. Click okay. Notice that it says, no active library at
the top of the window. We'll need to pick an active library if we plan to save changes to our part. Click Preferences, Footprint Libraries Manager. Here, you can add and manage your footprint libraries. Remember, they're completely different from the schematic symbol libraries. Click Append with Wizard. Make sure files on my
computer is selected, and click Next. Find your project directory and expand it. In it, you should see 555_Badge.pretty. Click on the .pretty
folder and click Next. Ki-Cad should verify that it can read the library, so click Next. Here, you have an
important choice to make. Do you want to import this library and have it usable by all your projects, or just usable by this project? Unless you're working on creating a large, well-curated library for all your projects, I recommend keeping
this custom part local. So, click To the current project only, and click Finish. You'll see your library listed under Project Specific Libraries, and if you click the tab
for Global Libraries, you can see any libraries you might have loaded for all projects, which is none for me. Click okay. Click File, Set Active Library. Click your 555_Badge
library and click okay. You should see the top of the window change to active library 555_Badge. Similar to Eeschema, you can use your mouse
wheel to zoom in and out. Okay, I wanna have a
quick chat about units. PCB layout is weird. Some data sheets will give you units in millimeters, some data sheets will give you units in inches, and some will give them to you in both. Many PCB manufacturing houses use the imperial system, which means you'll be doing a lot of layout in inches. I wish that only one system was used, but until that happens, we just have to be
comfortable working in both. From now on, I'll be using mostly the imperial system, because DIP parts seem to line up more easily with inches, but do know that many surface mount parts line up more easily with millimeters. Also, when I say mil from now on, I mean 1/1000 of an inch. Back in the Footprint Editor, make sure that the inches units button is selected. You can press the millimeter button to change the units to metric if you wish to switch. I also like to set up my grid to make moving things around easier. Something like 10 mils
should be good enough, but you can also change it with this dropdown menu anytime you want to switch. Hover your mouse over the part name and press the M key to move it down and out of the way. Do the same with the
ref text and move it up. It's usually a good idea to create your part with the origin in the center, so that it's easier to place and rotate during the layout process. However, and this is where some fun math comes in, most data sheets don't give you dimensions from the center. We'll be looking at the
eight lead PDIP package to make this footprint. So, what I'll do is draw something that represents a top-down view of the component body, and where I think the
pads or holes need to go, since that's all we care about in a basic footprint. I'll draw a little plus
symbol in the middle to denote the origin. I've also numbered the pins and added a little orientation marker on the left, to help show where pin one is. It's also important to note that Ki-Cad is a little backwards. To the right is positive for X, but down is positive for the Y-axis. By reading the data sheet, little E on the chart tells us that the distance between pins on one side is 0.1 inches. So, that means it's 0.05 inches from zero to the second pin, and another 0.1 inch to the first pin, giving us -0.15 inches in the X direction. EA tells us the distance the pins should be apart from each other in the Y direction, which is 0.3 inches. Note that you'll need to bend the pins to get this. So, half of that is 0.15 inches, which gives us positive 0.15 for the Y coordinate. Remember, down is positive. To get the location of the second pin, we know that its Y coordinate
will stay the same, but we need to add the
distance between the pins in the X direction, which gives us (-0.05, 0.15). We can mirror these points about the X and Y axes to get the other six coordinates. To know how big we should make the hole, we see that the maximum width of a pin is 22 mils, according to B. So, we'll add a few mils
on either side of that, and say that 30 mils
should be good enough. It's also a good idea to draw the component body for reference. You'll want to make sure other components won't hit it when you're laying out the board. We see that D tells us the longest part will be 0.4 inches, and E1 says that the
widest will be 0.28 inches. It's usually a good idea to go with the worst case scenario when dealing with possible
component body sizes, so that's why we look at max. By taking the half of these distances, we see that one quarter
of the component body will be at (0.2, 0.14) in coordinate form. Once again, we can flip the signs of these numbers to get all four corners on our rectangle. In the Footprint Editor, select Place, Pad. Click somewhere in the
editor to place a pad. Right click on the pad and click Edit. Leave the pad number as one. Notice that you can change the pad type and shape
to SMD and rectangular to make pads for a
surface mount footprint. But, we'll leave ours as through hole and circular. I'll overlay the hand drawn recalculated part dimensions, so you can see where I'm getting these numbers from. Change Position X to negative 0.15, and Position Y to positive 0.15. Make sure the drill size is 0.03 inches. The distance between the
edge of the drill hole and the edge of the copper is known as the annular ring. We want this copper to be wide enough so that we can get a soldering tip down, and 0.015 inches should be plenty. Double that to get 0.03, and add in the diameter of the drill hole, and we get that the diameter of the pad should be 0.06. Click okay, and you should see our pad move down into the left of the origin, which is shown by the
intersecting blue lines. Place a new pad, either by selecting Place, Pad, or by using the Add Pads
button on the right, and click in the editor. You can also edit the properties of a pad by hovering your mouse over it and pressing E. This time, make sure it's pad two. Change the X and Y coordinates to negative 0.05 and 0.15. Make sure that the drill is 0.03, and size is 0.06, just like in the first pad. If you want to copy a pad, right click on a pad, and select Duplicate Pad. Click the place to
duplicate pad somewhere, and place E to manually
edit the properties. Change the pad number to three, and change the X to positive 0.05. Remember that it's 0.1 inches away in the X direction from pad two. Keep Y at 0.15, and press okay. Repeat this process for pin four, whose X will be 0.15. The pin numbering on DIP parts make a U-shape starting with pin one, just to the left of the cutout notch. Once you get to the end of that row, jump across and keep numbering while going up back toward the notch. So, this would be one, two, three, four, across to five, six, seven, eight. Duplicating a pin also works by hovering over it and pressing Control + D. Create pin five and change
its X, Y coordinates to (0.15, -0.15). Continue this process
for the last three pins. Now, we want to draw an outline of the component body. We'll do this initially on the top fabrication layer, which is something we only see in layout. It usually isn't printed on the board or taken into account during the fabrication process. This will help us see our part in relation to other parts, and it'll also help us
draw a silkscreen later, should we wish to outline the component on the physical board. Additionally, if you're
having someone else or another service populate your board with parts, they can look at the fabrication layer to see which components go where, and in what orientation. Click Place, Line. Click somewhere to the right of our pins to start a line. Make a somewhat vertical line and click again to end the segment. You could keep drawing
another connected line, but let's press Escape to end it here. Right click on the line, and select Edit. We want to start where we showed in the hand drawn diagram, 0.2 for X, and 0.14 for Y. Keep the end X the same as the starting X, since we want to draw a vertical line. Flip the sign on the end Y, so we'll want negative 0.14. The default thickness is too big for us, so we'll change it to 0.004. You can make it whatever you like, but something between two and 10 mils usually works well here. Change the layer to F.Fab, which stands for front fabrication. Note that I'll sometimes say top layer, which Ki-Cad calls the front layer. Same thing for the back and bottom layer. They're the same thing. Right click on the line
and select Duplicate. Move it to the left of the pins. Edit the properties, and make sure it starts at (-0.2, 0.14), and ends at (-0.2, -0.14), which just flips the sign on the X coordinate from the first line. Duplicate the line again and press E while hovering over it to edit it. This time, we want to connect the bottoms of the previous two lines. So, the first coordinate is the one we have listed on the
diagram, (0.2, 0.14). We want to keep the Y coordinate the same, since this is a horizontal line. Flip the sign on the X coordinate to make it negative 0.2. Click okay. Duplicate the new line above the pins. Use the same X coordinates as before, but change the Y coordinates
to negative 0.14. Click okay. While this is a good
representation of the part, it's always helpful to show the orientation of the part, or show where pin one goes. Because our DIP package has a little notch on one side, we can draw a semi-circle to show how to line up that notch. Click Place, Arc. We want this arc on the
front fabrication layer, so on the right side, under the layers tab, click F.Fab to change our layer. You should see a little blue arrow appear next to it, showing that we're now
drawing on that layer. Because pin one should be to the left of the notch, if you're looking at the top of the part, we'll place the arc on the left side. Hover your mouse over
where the part outline meets the X axis, which is the horizontal blue line. Take a look at the grid coordinates at the bottom right of the window. You should see that we're at negative 0.2 and zero. X and Y show the absolute coordinates from the origin. You can press the space bar to place a temporary marker. While the absolute X and Y don't change, you'll see the relative coordinates, dx and dy change. This can be useful when you're trying to
draw intricate patterns, but remember that when you're entering coordinates by hand, they're based on the absolute system, the X and Y. Click at negative 0.2 and zero to start an arc. While looking at your coordinates, click again at negative
0.2 and negative 0.05. Hover over the arc and press E to edit its properties. Change the arc angle to 1,800. This means we want it to be 1,800, with units of 0.1 degrees, or 180 degrees, a semi-circle. Change the line thickness to match the other lines we drew, 0.004. Click okay, and you
should see a nice notch in your part outline. It's usually a good idea to show some of this on the physical board in the form of silkscreen, but keep in mind that silkscreen will not be drawn on our pads. That's because a solder mask keep out is automatically generated
on pads by Ki-Cad, so that the copper's left exposed, and we can generally only draw silkscreen on places with solder masks. Back in the Footprint Editor, let's draw another line. Use the menu bar, or click Add graphic
line button on the right. Select the F.SilkS layer on the right to draw silkscreen on the top layer. We can't draw where the pins are, but we can draw some silkscreen to show the other two sides of the part. Click the part outline corner by pin one. Notice that your drawing should snap to the grid
where that corner is. Click again on the corner by pin eight and press Escape to stop drawing. Right click over the line. If you're asked which line to edit, choose the F.SilkS layer and select Edit. Change the width to 0.008. We want this line to be slightly bigger than the fabrication line. Press okay. Hover over the line and press Control + D to duplicate it. If asked, you want the F.SilkS line. Move it to just cover the line at the other end of the part. It can also be very helpful to add something to the silkscreen to show how to orient the part, or where pin one is. It means that you won't need to look at the assembly drawings with the fabrication
layers to build your board. The easiest thing to do would be to just copy the semi-circle to the silkscreen layer. However, this would mean that once the part has been placed, you would not see this marker anymore, and it can be handy to see where pin one is supposed to be if you have to debug the board. So, what we'll do instead is place a small circle near pin one on the silkscreen. Click the Add graphic
circle button on the right. Make sure the front
silkscreen layer is selected, and click to start a
circle two grid dots down and one dot to the left of the corner near pin one. Move up a grid dot and click again to place the circle. Edit its properties and change the thickness to 0.008. Where this circle goes doesn't need to be precise, so long as it clearly marks pin one, and can be seen once the
part has been placed. Move the ref designator
just above the footprint, and centered on the Y axis, and move the part name
just below the footprint, and also centered on the Y axis. Notice that the name
is on the F.Fab layer, so it won't be printed on the board, but the ref des is on
the silkscreen layer, so it will show up. Also, the REF** is a
special name in Ki-Cad. This text will automatically change to the correct reference designator when we associate footprints
to schematic symbols in a later step. We're done. Click File, Save Footprint in Active Library, and click okay. If you don't want to start from scratch, or want to see how
other people made parts, you can click File, Load Footprint, Load Footprint From File. Navigate to the Digi-Key libraries and go into the
digikey-footprints.pretty folder. Open one of the SOIC footprints to see what a nicely done SMD footprint looks like. If you're creating something similar, it might be easier to start from here, make whatever changes you need, and then save it into a new library, or to your current active library. We won't do this now, so just close out of the Footprint Editor. I hope this has helped you see how to create your own
footprints from scratch, as well as where to go if you need example footprints. Next time, we'll be associating these footprints with schematic symbols, before loading them into
the PCB layout program. (upbeat music)
