Diseño PCB

FP

• Anchura pista
  • MIN 12mils
  • PREF 40mils (VCC i GND 40mils)
• Distancia
  • Entre pistas 100mils
  • Pistas y PCB 200mils
  • Componentes 150mils
  • Pad y pista 100mils
• Agujeros
  • 0.8mm para Resistencias de 1/4W

Fabricación casera que consigo

• Anchura pista
  • MIN 20mils
• Distancia
  • Entre pistas 14mils

Manual Kicad - Miguel Pareja

• Módulo
• Pad, vias o isletas
  • Taladros de fijacion
  • Vias
• Pistas
  • Ancho de pista
    • Depende de los amperios que pasan
    • Para corrientes menores a 300 miliamperios, un valor mínimo de ancho de pista de 0,5 milímetros (20mil)
    • Para mayores corrientes, se puede escoger la norma de 0,5 milímetros (20mil) de ancho de pista por cada amperio, como valor límite o mínimo. Algunos autores recomiendan la norma de 1 milímetro (39mil) de ancho de pista por cada amperio para un valor estándar de recubrimiento de cobre de la placa de circuito impreso de 35 micras.
    • La anchura mínima de las pistas de alimentación será de 2 milímetros (78 mil).
  • Separación entre pistas
    • Depende del voltaje que cae en el componente

PCB Layout Tutorial by David L. Jones

http://server.ibfriedrich.com/wiki/ibfwikien/images/d/da/PCB_Layout_Tutorial_e.pdf

• Grid
  • Submultiplos de 100mils (50,25,20,10, 5)
  • Comenzar con 50mils he ir bajando si los componentes tienen que caber en un espacio reducido
• Ancho pistas
• Pads
  • Parametro importante, pad/hole ratio
    • Cada fabricante tiene su ratio
    • Una regla es que el pad tiene que ser 1.8 veces el diametro del hole o al menos 0.5mm mas largo
  • Los pads de las resistencias, diodos, condensadores deben ser redondos de al menos 70mils de diametro
  • Los pads de los DIL (Dual In Line) se hacen ovales
    • 60mils de alto por 90-100mils de ancho
    • El Pin 1 suele ser rectangular para diferenciarlo
  • Los pads de SMD suelen ser rectangulares aunque los empaquetados SOIC suelen usar pads ovales con el pin 1 rectangular
• Vias
  • Profesionalmente se hacen plateando las vias para interconectar las pistas (PTH - Plated Trough Hole)
  • Suelen ser de 0.5-0.7mm
• Clearances
  • 15 mils es un buen espaciado para diseños through hole
  • 10 mils a 8 mils se usa para montajes smd muy densos

For 240V mains on PCB’s there are various legal requirements, and you’ll need to consult the relevant
standards if you are doing this sort of work. As a rule of thumb, an absolute minimum of 8mm (315 thou)
spacing should be allowed between 240V tracks and isolated signal tracks. Good design practice would
dictate that you would have much larger clearances than this anyway.

• Component Placement & Design
  • Lo mas importante de hacer PCBs es colocar bien los componentes. Tanto la facilidad del ruteo de pistas como la calidad electrica de la PCB dependen de la colocación de los componentes. Colocar los componentes es un arte, y cada diseñador hará la misma placa de diferente manera. Igualmente hay unas normas básicas que se deben seguir
    • Set your snap grid, visible grid, and default track/pad sizes.
    • Throw down all the components onto the board.
    • Divide and place your components into functional “building blocks” where possible.
    • Identify layout critical tracks on your circuit and route them first.
    • Place and route each building block separately, off the board.
    • Move completed building blocks into position on your main board.
    • Route the remaining signal and power connections between blocks.
    • Do a general “tidy up” of the board.
    • Do a Design Rule Check.
    • Get someone to check it
  • Lo primero que hay que hacer es establecer el grid y los tamaños de las pistas y los pads.
  • Un error común es colocar todos los componentes de golpe en el PCB. Esto puede ocasionarte problemas, como por ejemplo quedarte sin espacio para las pistas o dejar espacio "muerto" quedandote una PCB grande y desaprovechada.
  • Una tipica PCB de novato está con los componentes muy espaciados y hay cientos de pistas y vias atravesando la placa.
  • La mejor manera de empezar es haciendo un volcado de todo el esquema.
  • Con todos los componentes en la pantalla y teniendo el tamaño de la PCB puedes ver si tienes que "currarte" una disposición estrecha y eficiente de los componentes o si puedes ser un poco mas liberar en la disposición de los componentes.
  • El siguiente paso es analizar que partes del diseño se pueden dividir en distintos bloques. Imaginemos un gadget que necesita alimanterse de 230V, la fuente de alimentación será un bloque. También tiene un gps (otro bloque) y un módulo GPRS (otro bloque). Una vez tenemos los bloques definidos podemos apartarlos fuera de la placa para ir emplazando sus componentes.
  • También es necesario compartimentar en grandes bloques las partes electricamente sensibles. Un ejemplo son los diseños que tienen circuitos analogicos y digitales. Estos circuitos no se pueden mezclar y tienen que estar fisicamente y electricamente separados. Otro ejemplo es con los circuitos de altas frecuencias y alta corriente, no se deben mezclar con circuitos de bajas frecuencias y baja corriente.
  • Una regla general es tener bien alineados los componentes:
    • Los ICs en la misma dirección
    • Las resistencias todas en horizontal o en vertical
    • Los condensadores electroliticos con la polaridad en el mismo lado
    • Los conectores en los bordes de la placa
  • A pesar de esto los parametros electricos prevalecen al estar bien alineados.
  • La simetria es algo positivo en el diseño de PCBs. Vale la pena poner alineados y de la misma forma bloques iguales.
  • Una vez esten los componentes dsitribuidos se puede pasar a rutear los bloques entre ellos yse pueden poner sobre la PCB
  • El DRC (Design Rule Check) es una parte importante para comprobar que no hay errores de espaciado ni tamaño de pistas/vias.
  • Sino tienes a nadie que puede ayudarte a comprobar el diseño puedes imprimir el esquema e ir marcando cada conexión que veas en la PCB. Cuando acabes no debe quedarte ninguna conexion del esquema por marcar.

• Basic Routing

Now it’s time for some basic routing rules. Routing is also known as “tracking”.
Routing is the process of laying down tracks to connect components on your board. An electrical connection
between two or more pads is known as a “net”.

 Keep nets as short as possible. The longer your total track length, the greater it’s resistance,
capacitance and inductance. All of which can be undesirable factors.

 Tracks should only have angles of 45 degrees. Avoid the use of right angles, and under no
circumstances use an angle greater than 90 degrees. This is important to give a professional and
neat appearance to your board. PCB packages will have a mode to enforce 45 degree movements,
make use of it. There should never be a need to turn it off. Contrary to popular belief, sharp right
angle corners on tracks don’t produce measurable EMI or other problems. The reasons to avoid right
angles are much simpler - it just doesn’t look good, and it may have some manufacturing
implications.

 Forget nice rounded track corners, they are harder and slower to place and have no real advantage.
Stick to 45 degree increments. Rounded track bends belong to the pre-CAD taped artwork era.

 “Snake” your tracks around the board, don’t just go “point to point”. Point to point tracking may look
more efficient to a beginner at first, but there are a few reasons you shouldn’t use it. The first is that
it’s ugly, always an important factor in PCB design! The second is that it is not very space efficient
when you want to run more tracks on other layers.

 Enable your Electrical grid, which is sometimes referred to as a “snap to center” or “snap to nearest”
option. Let the software find the centers of pads and ends of tracks automatically for you. This is
great for when you have pads and tracks which aren’t lined up to your current snap grid. If you don’t
have these options enabled then you may have to keep reducing your snap grid until you find one
that fits. Far more trouble than it’s worth. There is almost never a reason to have these options
disabled.

 Always take your track to the center of the pad, don’t make your track and pad “just touch”. There are
few reasons for this. The first is that it’s sloppy and unprofessional. The second is that your program
may not think that the track is making electrical connection to the pad. Proper use of a snap grid and
electrical grid will avoid problems here.

 Use a single track, not multiple tracks tacked together end to end. It may make no difference to the
look of your final board, but it can be a pain for future editing. Often you’ll have to extend a track a
bit. In this case it’s best to delete the old one and place a new one. It may take a few extra seconds,
but it’s worth it. People looking at your finished board may not know, but YOU’LL know! It’s the little
touches like this that set good PCB designers apart.

 Make sure your tracks go right through the exact center of pads and components, and not off to one
side. Use of the correct snap grid will ensure that you get this right every time. If your track doesn’t
go through the exact center then you are using the wrong snap grid. Why do you need to do this? It
makes your board neater and more symmetrical, and it gives you the most clearance.

 Only take one track between 100 thou pads unless absolutely necessary. Only on large and very
dense designs should you consider two tracks between pads. Three tracks between pads is not
unheard of, but we are talking seriously fine tolerances here.

 For high currents, use multiple vias when going between layers. This will reduce your track
impedance and improve the reliability. This is a general rule whenever you need to decrease the
impedance of your track or power plane.

 Don’t “drag” tracks to angles other than 45 degrees

 “Neck down” between pads where possible. Eg, a 10 thou track through two 60 thou pads gives a
generous 15 thou clearance between track and pad.

 If your power and ground tracks are deemed to be critical, then lay them down first. Also, make your
power tracks as BIG as possible.

 Keep power and ground tracks running in close proximity to each other if possible, don’t send them in
opposite directions around the board. This lowers the loop inductance of your power system, and
allows for effective bypassing.

 Keep things symmetrical. Symmetry in tracking and component placement is really nice from a
professional aesthetics point of view.

 Don’t leave any unconnected copper fills (also called “dead copper”), ground them or take them out.