find.c: Fix flag passed to ListStart() in DRCFind().

[geda-pcb/pcjc2.git] / doc / gs / fb-smt.texi

@node SMT Blinker
@section SMT Blinker

The third and final board in the ``first board'' series will teach you
about multi-layer boards, vias, and SMT components.  Again, we assume
you've done the other two boards, and will not re-explain concepts
taught there.  We will be using the same circuit as the last board,
but to make things interesting, we will be adding some constraints.
The board must be as small as possible, EMI-proof, and able to handle
rework.  Ok, I'm making this up, but what it means is that we will be
using the smallest components a hobbyist can expect to use, a
four-layer board, and more vias than would otherwise be needed.  We do
this to give us the opportunity to learn these techniques, without
spending undue time due to an overly large schematic.

We begin with the same schematic as before.  To assist us in assigning
power planes, we need to name the power rails in the schematic.  See
the @code{gschem} documentation for details, but what you want is to
name the ground net @code{GND} and the power net @code{Vdd}.  Set up a
new @code{fb-smt.prj} project file as before.  Use @code{gattrib} to
set the footprint attributes as follows:

@multitable @columnfractions 0.25 0.15 0.15 0.15
@item @tab @b{refdes} @tab @b{footprint} @tab @b{value}
@item @tab C1 @tab 0402 @tab 1uF
@item @tab J1 @tab pj102.fp @tab PJ102
@item @tab LED1 @tab 0402 @tab RED
@item @tab R1 @tab 0201 @tab 100k
@item @tab R2 @tab 0201 @tab 100k
@item @tab R3 @tab 0201 @tab 3.3k
@item @tab U1 @tab MSOP8 @tab LMC555CMM
@end multitable

Run @code{pcb} and set up your blank board.  Put ``component'' and
``component side'' in group 1.  Put ``GND'' in group 2, ``power'' in
group 3, and ``solder'' and ``solder side'' in group 4.  Switch to the
@mnu{Change} tab, select the solder layer in the main window, and
move the solder layer down under the power layer.

@img{fb-smt-1}

Set the board size to 50 mm by 50 mm.  To set a metric size, use the
@mnuuu{View,Grid units,mm} menu option.  Then, the @mnu{Sizes}
preference will use millimeters.  Set the DRC values to 0.35 mm (about
13.5 mil) for drill and 0.15mm (about 6 mil) for everything else.
Save your board, exit @code{pcb}, and run @code{gsch2pcb fb-smt.prj}.
Go back to @code{pcb}, import and disperse the new elements, and load
the netlist.

As before, move the labels out of the way and size them accordingly.
You should end up with something like this:

@img{fb-smt-2}

The final size of our board will be 12.5mm wide by 18 mm high, not
much bigger than the power jack.  Start by rotating the power jack to
face down, and put its mark at 5.5mm by 7mm.  The LED goes just above
it, with R3 to the right of the LED.  The rest of the elements will go
on the other side of the board.  Here's how:

For each element that needs to go on the other side of the board,
place the crosshair over the element and press the @press{B} key

@center @image{fb-smt-3} @image{fb-smt-4}

The element shows as a light gray because it's now on the ``far side''
of the board (Note that one of the layer buttons says @mnu{far side}
on it).  You can flip the board over (making the far side the near
side, and visa-versa) by pressing the @press{Tab} key.  Since the
elements we need to place are on the far side, now, flip the board
over.  Note that this is an up-down flip, so the power jack now
appears in the lower left corner instead of the upper left.  There are
other types of flips you can do by using @press{Shift-Tab} (left-right
flip), @press{Ctrl-Tab} (180 degree rotation), or
@press{Ctrl-Shift-Tab} (nothing moves, sort of an X-Ray view).

Anyway, move the remaining elements around so that they look like
this:

@img{fb-smt-5}

When routing a multi-layer board, I find it best to start with the
power and ground planes.  First, resize the board to be 12.5 mm wide
by 18 mm high, and flip it so you've viewing the component side (the
side with the power jack).  If your version of @code{pcb} does not
permit sizes this small (some versions have a one inch minimum, others
0.6 inch), save the file, exit @code{pcb}, and edit @code{fb-smt.pcb}
in a text editor so that the @code{PCB} line looks like this:

@example
PCB["" 49213 70866]
@end example

When you run @code{pcb} again, the board will have the right size.
Set your grid to 0.5 mm and make sure it's visible.  There are two
ways to create a ``plane layer'', which means a layer that's mostly
copper.  Such layers are often used for power and ground planes.  The
first way is to use the polygon tool; the second is to use the
rectangle tool, which is just a shortcut for the polygon tool.

Make the GND layer the current layer and select the POLY tool:

@img{fb-smt-6}

The polygon tool works by clicking on each corner of the polygon, in
sequence.  You complete the polygon by either clicking on your start
point again, or by pressing @press{Shift-P}.  We will create a polygon
that's 0.5mm away from the board edge.  In these images, we start at
the lower left corner and work our way around clockwise.  When we
click on the lower left corner again, the polygon is created:

@center @image{fb-smt-7} @image{fb-smt-8} @image{fb-smt-9} @image{fb-smt-10} @image{fb-smt-11}

In this case, we're just drawing a rectangle, but if you need any
other shape, just click on the corners as needed.  As a shortcut, you
can create a rectangle with the rectangle tool, which creates
rectangle-shaped polygons.  Make the power layer the current layer and
select the RECT tool:

@img{fb-smt-12}

Like the polygon tool, the rectangle tool works by clicking on
corners.  However, you only have to click on two diagonally opposite
corners, like this:

@center @image{fb-smt-13} @image{fb-smt-14}

If the color difference is too subtle for you, you can choose other
colors through the @mnuu{File,Preferences} menu option.  We will set
the GND layer to green and the power layer to red for the remainder of
this tutorial.

To connect the ground and power planes to their respective nets, we'll
use a thermal to connect the power jack's pins to them.  We could also
just draw a line from the pin to the polygon, but thermals are better
suited to this task.  Select the THRM tool:

@img{fb-smt-16}

What the thermal tool does is connect (or disconnect) thermal fingers
between pins or vias, and the polygons around them.  Each time you
click on a pin or via, the thermal fingers are connected to the
current layer.  We want to find the pin on the power jack that's
connected to ground in the schematic, and connect it to ground on the
board.  We use the netlist dialog to do so.  First, optimize the rats
net with @press{O} and make the GND layer current.  If the netlist
dialog isn't shown, use @mnuu{Window,Netlist} to show it.  Select the
GND net and click on @mnu{Find}:

@img{fb-smt-17}

Notice that one of the pins on the power jack has been highlighted.
That's the one that is supposed to be connected to the ground plane.
Click on it to create a thermal:

@img{fb-smt-18}

If you optimize the rats nest again, the rats won't connect to that
pin any more, and the other pins and pads that need to connect to the
ground plane are now marked with circles, meaning ``these need to be
connected to a plane''.  Anyway, make the power plane the current
plane, find the VDD net in the netlist and create its thermal on the
found power jack pin.  Note that the green GND thermal fingers on the
other pin show through the gap in the red power plane - thermals are
created on a specific layer, not on all layers.

@img{fb-smt-19}

If you tried to autoroute the board at this point, it would just
connect all those power and ground pins to the power and ground pins
on the power jack.  So, we will first tie all the power and ground
pins to their planes manually, using vias.  We're doing this mostly to
demonstrate how to do it, of course.  The first step is to place the
vias.  Select the VIA tool from the left panel:

@img{fb-smt-20}

Click on the @b{Route Style} button to bring up the route styles
dialog, and set @b{Via hole} to 0.4mm and @b{Via size} to 0.8mm.  Also
set @b{Line width} to 0.25mm.  Create vias near the pins that are
connected to the planes, as such:

@img{fb-smt-21}

Note that I've shut off the ground and power planes, as well as rat
lines, to help you see where the vias should go.  Shut off the GND
plane and ``find'' the VDD net again, to highlight which rat circles
(and thus their vias) need to connect to the power plane.  Like you
did with the power jack's pins, use the thermal tool to connect the
relevent vias to the power plane.  Repeat for the GND plane.

@center @image{fb-smt-22} @image{fb-smt-23}

Now you have to connect the vias to the pins that need them.  For the
LED it's easy, that trace goes on the top.  Make the component layer
the current layer and use the LINE tool like you've done before to
draw a line from the via next to the LED, to the pad on the LED that's
connected to VDD.  For the other connections, you'll want to flip the
board over, so use the @press{Tab} key to flip the board over, make the
solder layer the current layer, and connect the rest of the power/gnd
pins to their vias.  If you press @press{O} now, you'll see that all the
rat-circles have gone away:

@center @image{fb-smt-24} @image{fb-smt-25}

The last step is autorouting.  Hide all the power, ground, and silk
layers, optimize the rats nest (@press{O}), and run the autorouter,
optimizer, and miterer.  Done!  Here's what the board looks like with
the ``thin draw polygons'' setting checked, to only draw outlines for
the power and ground planes, along with some photo-quality prints:

@center @image{fb-smt-26} @image{fb-smt-top} @image{fb-smt-bottom}