(upbeat dance music)
- With our parts placed
and board outline completed
we get to draw traces.
By doing this we're telling the board house
where we want to leave pieces of copper
when they perform the etching process.
This will allow us
to make electrical connections
between components.
We'll still be working in PcbNew in this episode
just like last time.
In KiCad, make sure you have your project open
and select Tools, Run PcbNew.
On the last episode we imported our parts
and carefully moved them around
into these positions.
The idea now, is to draw traces
to make all of these air wires disappear.
While you're working on your layout
it can be a good idea to periodically
run the Design Rules Check or DRC.
Go to Tools, DRC, click Start DRC.
If you have any issues with your layout
such as traces being too close together
they will be listed in the Problems Markers tab.
Click on the Unconnected tab.
Here, you can see all the connections
that we need to make with our copper traces.
When we're done we should be able
to run the DRC tool and see no problems
or unconnected pads listed.
Click OK.
Let's make an easy first connection
so you can see how to draw traces.
The first thing I like to do is change my grid
to something a little smaller
and make it easier to work with.
Click on the Grid dropdown
and change it to 10 mils.
You can go smaller than this if you need to
but 10 mils snapping is a good starting point.
Click Place, Track to select the Trace Drawing tool.
Select the front copper layer on the right
and make sure the little blue arrow is pointing to it.
Remember, we can only draw tracks on the top
or bottom copper layers on this board.
Find and zoom in on C2.
Notice the air wires that go between C2 and pad two of R5.
This is an easy trace to draw.
Click on pad one on C2
and you'll see your trace snapped to the middle of the pad.
Come out from the pad a little ways
and click to place a bend.
You'll see a series of three yellow lines
coming out of the end of the trace
that's on your cursor.
These tell you all the pads
that your current trace needs to be connected to
which includes pad two on R5.
Move up and hover over pad two on R5.
You'll see that the trace will snap to the pad
creating another 45 degree bend as it does so.
Make sure there's a small amount of vertical trace
before it enters pad two.
If you're not happy with the trace,
press escape to try again.
If you are happy, double click over pad two
to draw the trace and that's it.
You've drawn your first trace.
There's no real order you have to follow
when drawing traces.
However, I like to start with my power lines first.
And then look for easy to connect pads
that are close together.
From there I work my way out
from the most complicated parts
which are usually integrated circuits.
Note that I usually don't draw traces
for the ground node,
as I'll use a copper pour to make those connections.
When dealing with power traces
you usually have to make them larger
than your signal traces
as they need to carry much more current.
If you don't they can heat up and potentially melt,
creating an open circuit or worse a fire.
Theoretically, we see that the trace supplying power
from our battery needs to support spikes
up to about 20 milliamps.
Search for trace width calculator
and click on the advanced circuits one.
Set the current to .02 amps or 20 milliamps.
Make sure the trace thickness is one ounce.
As that's the default for most board manufacturers.
Notice the internal layers results.
These are for copper layers in the middle of your board
which we don't have.
The external layers show the trace width
needed for our top and bottom copper layers.
Looks like we'll need something less than a mil thick.
So, our ten mil traces should be fine.
But I'll show you how to make a larger trace
should you need it.
In all honesty, it's only when you start approaching
a few hundred milliamps that you need to really worry.
Back in KiCad, select Design Rules, Design Rules.
In the Net Class Editor tab
you can do some slick things like
assign specific trace widths and clearances
to different nets and nodes.
However, there is a quicker way
to create a different trace width
if you're working on a simple board like this.
Click on the Global Design Rules tab.
Find the Custom Track Widths section.
For the track one field enter .03
to create a trace width of 30 mils.
Click OK.
In the top left, you should see
the Track Selection drop down menu.
Click it and you should see
the 30 mil trace width we just made.
Select it.
Note that the 10 mil width
will still be the default we can draw with.
But this allows us to make larger traces
for things like power nets.
Click on the positive pin on the battery holder.
Double click on the top pin of the switch
to draw the trace.
Click on the middle switch pin.
And then connect the trace to the required pin on R7.
We can then create branches off this main power trunk.
Click on the VCC pin on R1
and draw a trace straight down
to the large trace we just made.
Double click to connect them.
Do the same for R6.
The seven five five five timer
does not require nearly the same amount
of current as the current LEDs.
Select a 10 mil trace width from the dropdown menu.
And draw a trace from the middle switch pin
to pin eight on the seven five five five.
Draw another trace
connecting pin eight to pin four
as shown by the air wire.
Now that we've drawn our power traces
let's connect everything else.
But leave ground alone for now.
Start by looking for easy traces,
pads that are close together.
For example, pin seven of the five five five
to R1 and R2.
Go to connect pin six to C1
but notice that KiCad won't let you draw
a trace over another trace or across a pad.
That's because if we tried to fabricate this
those nets would be shorted together, not good.
So, make sure you come out of the pin
a little ways to avoid having your trace
touch other pieces of copper.
Connect the middle pin of Q1 to R5.
Finish making the connections that we first started with.
Connect R5 to R3 and R4.
Notice that the pins who's net
you're currently working with will highlight yellow.
This can help you if you have a large number
of pins to connect together.
For example, if we start drawing a trace
from a ground pin you can see
all the other ground pins turn bright yellow.
Press escape to stop drawing a trace.
That's about all the traces we can draw on this side
with this collection of components.
Most of the other air wires
cross over traces we already drew.
Which means we need to draw
new traces on the bottom side.
On the right side,
click on the bottom copper layer.
Click on pin two of the five five five
and connect it to pin six.
Remember, plated through holes are connected
on the top and bottom layers.
So, you can draw traces
on either layer for PTH parts.
The new trace is green,
showing that it's on the bottom layer.
Even though it crosses one of our other traces,
it's on another layer so they won't actually touch.
If things start to look confusing
you can click on the check box
for the front copper layer to turn it off in our view.
This can make things look clear
as you draw traces on the bottom layer.
Connect pin six to R2.
Connect pin three to R3.
There's slightly more space above Q1,
so I'll route my trace there.
At this point you might be wondering
why is everything on a 90 degree or 45 degree angle.
For parts it's usually easier for machines
like pick and place machines
to line up parts on the 90 degree.
And for traces, many older board houses
could only manufacture straight lines
on that 90 degree or 45 degree angle.
This was reflected in many older layout programs, as well
that only let you draw lines on the 45 and 90.
Also note that when you get up to higher frequencies
such as above one gigahertz
many reflections would be introduced
if you had hard 90 degree bends.
So, you would often see traces with 45 degree bends.
But we don't need to worry about
any of these things in our board.
So, you can draw them at whatever angle you want.
The only other thing you should try to avoid
is acute angles where copper connects.
Some older board manufacturing processes
used harsh chemicals to etch away copper.
So, places with bends of less than 90 degrees
would capture some of those chemicals
in what's known as an acid trap.
Those chemicals would remain after the board was finished
and slowly eat away at the copper over time
potentially causing breaks in the circuit.
Once again, you generally don't
need to worry about that anymore.
But you'll still see me and many others
avoid acute angles in layout.
This board could actually be made without using any vias
but I'm gonna show you how to use one anyway.
Turn on the front copper layer and select it
so we start our trace on this layer.
Start a trace from pin three of the transistor.
Come out a ways and click to start going up
between R6 and R7.
Do you see the faint red circle around my cursor?
That shows you how much space
is needed around the via when we place it.
Position it so that the circle
is in between R6, R7 and the green trace.
Make sure it's not touching any other traces or pads.
Right click and select Place Through Via.
Notice that you're now drawing on the bottom layer.
Your trace is green.
Keep going up.
Click to place a bend.
And connect the trace to pad one on D2.
Draw another trace to connect this and pad one on D1.
We want to keep the traces going
to the LEDs on the bottom side.
If we put them on the top,
you'll be able to see them through the silkscreen.
It won't make for a pretty drawing area.
Connect R6 and R7 to their respective LEDs.
And do this on the bottom layer.
Notice that even though the air wires
show that they need to cross over your other trace
you can simply swing your new traces around the LEDS
without needing to jump to another layer.
We're done with the basic layout.
We have some air wires left
but we're about to fix that by creating a copper pour.
A copper pour is simply an area in the PCB
that's filled with copper.
If you ever have to mill a board to make a prototype
then leaving much of it filled with copper
can make the milling process much easier.
Also, we usually connect the pour
to something like ground or a DC voltage.
This can have the effect of reducing radio emissions
from traces that are surrounded by this pour
especially in circuits with higher frequencies.
Finally, it can make layout easier
as we don't have to worry about
making all those connections manually
in something like our ground net.
Select place, zone.
Click just outside of our board one grid dot down
and to the left of the bottom left corner.
You'll be asked to pick a layer and a net.
Select the front copper layer and select ground.
Notice that it pulls the clearance and minimum width
from our default class design rules.
10 mils and 10 mils should be plenty here.
Click OK.
Create a rectangle just to the outside of our board outline,
clicking to place each of the corners.
Double click to end the zone.
Right click on the zones edge
and select fill or refill all zones.
You should see your entire board be filled with copper.
Turn off the bottom copper layer to see it better.
You can see that there is a 10 mil gap
between the board edge and where the pour starts.
Also, the pour keeps a 10 mil distance
from all the other traces.
But it does automatically connect
to each of the ground pads.
Let's do the same thing for the bottom layer.
Turn on the bottom layer and turn off the top layer.
Select the Zone Tool button on the right.
Click to start a zone and make sure bottom copper
and ground are selected.
Click OK.
Draw another rectangle around your board outline.
Fill in the zones again
which can be accomplished by pressing the B key.
Turn the front copper layer back on
and you'll see that your board is now a yellowish color
as your looking at both layers.
We're done with the layout.
You could fabricate this board and it would work just fine.
Just to be sure, go to Tools, DRC.
Click Start DRC.
You should see nothing listed in the Problems Markers tab
as well as nothing in the Unconnected tab.
This means we have everything connected
with appropriately spaced and sized traces.
Click OK.
To help us assemble the board
we'll want to move all the values
to easier to read locations.
Values are shown by the yellow text
and they won't show up on the final board.
Hover your mouse over BS7 and press M.
If asked, select the Value text.
If you look closely, you'll see a gray or blue line
showing you which part this piece of text belongs to.
Move BS7 to near the other yellow BAT1 text.
It can be helpful to turn off the bottom layer
to make the values easier to read.
Keep moving these pieces of text
to inside the components or next to them.
The light blue RefDes text for each component
is on the silkscreen which means it will show up
on the final board.
Let's move these so we can read them
and know which part they're referring to.
Press M over the light blue BAT1 and press R to rotate it.
And move it just to the left of the positive pin.
Move S1 and the RefDes text for the top row of resistors
to just above their respective parts.
Once again, you can look for a faint blue line
to see which part the RefDes text refers to.
You'll want to avoid having any of this
silkscreen text overlapping pins or vias.
Remember, there likely won't be any solder mask
over through holes.
Which means you can't draw silkscreen there.
Move R5 down a notch.
And move Q1 to above the transistor.
Keep U1 above the seven five five five.
And move C1 And C2 to just below the parts.
We can leave D1 and D2 alone
since we're about to cover them up
with a big chunk of silkscreen.
The idea is that we want a large silkscreen square
to take up most of the front of the badge.
This will provide a canvas
for you to draw on with a Sharpie.
Click on the Zone Tool button
and select the front silkscreen layer.
Click near your LEDs
and make sure F silk S is selected.
Click OK.
Draw something like a square around your LEDs.
Zoom in on the bottom left corner.
Right click it and select zones, move corner.
Move it to 5.06, 3.9.
Move the top left corner to 5.06, 1.9.
Move the top right corner to 7.06, 1.9.
And move the bottom right corner to 7.06, 3.9.
You should now have a large swath of silkscreen
surrounding your LEDs.
If you'd like you can add a piece of silkscreen text
to help you remember part orientation or other notes.
Click the Text button and select the front silkscreen layer.
Click to the right of the battery's positive terminal
and enter a plus symbol for the text.
Click OK.
And drop the symbol near the positive terminal.
Click again and write ON in capital letters.
Press OK.
Place the ON text to the left of pin three on S1.
This will tell us which position
the switch needs to be in to give power to the circuit.
Turn off the top copper and top silkscreen layers.
Turn on the bottom copper and bottom silkscreen layers.
Click again and enter five five five badge as the text.
This is a good way to show
the name of your board on silkscreen.
Change the width and height to .1
and change the thickness to .02.
For the Layer, select the bottom silkscreen layer.
When we are looking at our board layout
in a Cad program like this
we're pretending we can see straight through the layers
starting with the top layers.
This means that if you were to flip over the board
all the bottom layers would appear to be reversed.
This means we actually need to mirror our text
if it's going on the bottom layer
so that it will appear the right way when we look at it.
Under Display, select Mirrored.
And click OK.
Place it centered somewhere between the LEDs
and the badge clip slot.
I'll put mine at about 6.06, 2.35
the last thing I like to do
is put a version number on the board.
And this version number
should match the one on the schematic.
You can do this in silk
but I like to do it on the copper layer
to make it a little less obvious.
Select the Text tool in the bottom copper layer.
Click to bring up the text window
and write V zero one.
Click OK and place it in the bottom right corner
making sure the text doesn't extend
past the ground pour edges.
Also, ensure that the text is mirrored
just like our board name.
Press B to redraw the pour
and you should see your text appear.
Don't forget to change this
if you update your schematic or board.
Zoom out and turn your layers back on.
Take a look at your final board.
I think we're ready to make it.
Don't forget to save your work.
And we're done with layup.
Feel free to high five yourself.
Or throw a tiny party.
We still need to generate Gerber files
to send to OSH Park.
As well as create a bill of materials.
But we are almost done.
See you next time.
And don't forget to subscribe
to keep up with these videos.
(upbeat dance music)