Practical Electronics/PCB Layout

From Wikibooks, the open-content textbooks collection

Jump to: navigation, search

PCB layout: The efficient laying out of traces on a PCB is a complex skill, and requires much patience. This task has been made vastly easier with the advent of readily available PCB layout software, but it is still challenging.

Contents

[edit] Copper Thickness

The vast majority of PCBs are manufactured with "1 ounce copper" on the outer layers. (If there are inner layers, they are almost always manufactured with "1/2 ounce copper"[citation needed]).

The thickness of the copper layer on the PCB affects the behaviour of the circuit. PCB copper thickness is usually measured in ounces per square foot, or frequently, just ounces. It can also be given in micrometres, inches or mils. The measurements for common thicknesses are given below.

oz/ft² μm in mil
0.5 17.5 0.0007 0.7
0.75 25.5 0.0010 1.0
1 35 0.0014 1.4
2 71[1] 0.0028 2.8
3 105 0.0042 4.2

As always, the thickness of a thin slab of metal with a given top surface area is always exactly

thickness = { mass \over { area \times density } }

The area is "1 square foot" (144 square inches), the density of copper is 8.96 mg/mm^3 = 5.18 ounce/(inch^3), and usually the mass is "1 ounce of copper", but occasionally 1/2, 2, 3, or 4 oz.

[edit] Trace Width

Different widths of traces have different properties that could affect the operation of the circuit. For, example, a thin trace has a higher resistance than a thick one, and can therefore carry less current or will heat up more for the same current.

Due to the large number of tables and charts, this information is presented on different pages:

Most manufacturers can manufacture a minimum trace width of 0.010 inch. (Many can manufacture traces 0.008 inch wide). Such minimum-size traces are more than adequate for most digital and analog signals.

[edit] footprints

The manufacturer of each part recommends a "footprint", a copper pattern for the part to be soldered to the PCB.

Sometimes the footprint also includes a drawing of the outline of the part. Some people put that outline on the silk screen. Other people make a "virtual outline" that shows up on the computer screen and on the assembly drawings, but not on the actual PCB.

Footprints for capacitors and batteries should include plus sign (+) polarity marking on the silk screen next to the positive pad. (The positive-end-indicator stripe on the capacitor itself should be placed nearest that plus sign).

Footprints for LEDs and other diodes should have a polarity mark -- the "diode arrow symbol" (triangle + bar), or at least the bar, in silk-screen. The bar matches the cathode-end-indicator stripe on the diode itself. [2]

Footprints for ICs should have a polarity mark "dot" or "1" near pin 1. Most people give pin 1 a "squared-off" pad, and all other pins a "rounded pad". Some people also like additional "10", "20", "30", etc. marks in silkscreen next to pin 10, pin 20, pin 30, etc.

The polarity mark must be visible after mounting the part so it can be seen after inspection. (It's useless to put the polarity mark where no one can see it). It's OK to put the polarity mark underneath a tubular-packaged diode, since people can look "around" the mounted diode and see the polarity mark. [3]

[edit] holes

Most PCBs have many holes drilled in them.

Most PCBs with more than 1 layer have every hole "plated-through-hole", even holes that don't need to be plated through-hole (tooling holes and some through-holes). They do that because it takes extra effort to plug "non-plated" holes before throwing the PCB into the plating bath.

There are 3 general types of holes:

A via -- literally, a "way" to get from one layer of copper to another layer of copper. The vias on a particular PCB should all be the same size. Some people[1] recommend 0.025" (0.6mm) diameter via holes, surrounded by a 0.042" (1.0mm) diameter via copper pad [citation needed], if at all possible. Some very dense SMT boards require smaller vias. Some manufacturers can handle 0.012" diameter via holes, surrounded by 0.024" diameter via pad [citation needed].

Since there is no actual component put into a via, many PCBs are manufactured with "plugged" vias (vias completely filled with metal) and "tented" vias (vias completely covered with solder mask).

A through-hole -- many components (called "through-hole components") require a hole (a "through hole") for each pin. The part manufacturer should specify a "footprint" including the location and size of each hole. If there is no recommendation, common practice is

  • round leads: add 6 mils to the nominal round lead diameter to get the recommended PCB hole diameter. Rectangular leads: find the lead diagonal (sqrt(x^2 + y^2)). Then add 6 mils to get the recommended PCB hole diameter. ( 6 mils ~= 0.15 mm )[2]
  • "The component lead - hole clearance should be 0,4 mm" [3]
  • "The optimum pad diameter for a through-hole component is twice its finished hole diameter."[4]

A tooling hole -- ... preferably 0.125" ...[citation needed] ... mounting holes ... A "tooling hole" -- used to temporarily attach the board to test fixtures, and later bolt the board into the final product case. Needs to big enough for the mounting bolt. If the board is wave-soldered (rather than reflow soldered), there is a risk that these holes may get plugged with solder. So these holes are temporarily plugged with a stopper -- either plugged when the PCB is manufactured (becoming non-plated-through-holes, so solder won't stick), or plugged during the wave-solder process.

[edit] layers

The vast majority of PCBs have an overall thickness of 1/16 inch (1.58 mm). Some very dense SMT boards have an overall thickness of 1/32 inch ( 0.79 mm ), which allows smaller via holes to be drilled, allowing denser packing. Occasionally boards are made with an overall thickness of 3/32 inch (2.3 mm), which makes it more rigid (but requires bigger via holes).

Often some or all layers are covered with a "copper pour" ("ground plane" or "power plane"). Such pours typically have a signal-to-pour clearance of 0.010 inch [citation needed] and clearance from the cut edge (perimeter of the board edge) to pour of 0.020 inch[5].

(more layer stackup tips)

[edit] Reference Handbook

A PDF file is being prepared which will contain many of the diagrams and tables in a downloadable, printable format:








Usually an electronics or electrical engineer designs the circuit, and a layout specialist designs the PCB. PCB design is a specialized skill. There are numerous techniques and standards used to design a PCB that is easy to manufacture and yet small and inexpensive.

[edit] layers

Most PCBs have between one and twenty conductive layers laminated (glued) together in a sandwich with insulating plastic. PCBs with more than two layers help construct complex or dense circuits. They are not always used because they are more expensive, and the inner layers are more difficult to inspect and repair.

In more complex PCBs, two or more of the layers are dedicated to providing ground and power. These ground planes and power planes distribute power well. They also prevent radio waves from antennas unintentionally formed by tracks. These planes are rectangular sheets of foil that occupy entire layers (except for small holes to avoid unwanted connection to vias and through-hole components). They distribute electrical power and heat better than narrow traces. Sometimes solid metal PCBs with thin layers of insulation are used. The power electronic substrate carries away waste heat when air cooling is impossible.

Four-layer PCBs with a ground and power plane are often used in high-quality, but cost-conscious audio, avionics and medical electronics. Most consumer products have one or two layers.

[edit] traces

The width and spacing of conductors (or "traces") on a PCB is very important. If the traces are too close, solder can short adjacent traces, and the PCB will be difficult to construct or repair. If too far apart, the PCB may be too large and expensive. When a PCB carries high frequencies, traces may need to be exact widths and lengths to control the characteristic impedance of the trace.

Some designs cut the ground plane or the entire PCB in strategic locations to control the return paths of currents. The usual desire is to keep high voltages or frequencies away from sensitive portions of a circuit. The actual properties of the design are critical, because in some cases, cutting the ground plane makes the PCB into an antenna that radiates radio noise into nearby equipment.

Removing large areas of copper wastes etchant and increases pollution. Also, a PCB etches more consistently and tends to resist warping if all regions have the same average ratio of copper to bare board. Therefore, designers may widen connectors, leave unconnected copper in place, or cover large areas of what would otherwise be bare board with arrays of small, electrically isolated copper diamonds or squares.

Most PCBs have alignment marks (called fiducials) and tooling holes to align layers. These permit the PCB to be mounted in equipment that automatically places and solders components. Some designs also have quality control patterns to measure soldering and etching processes. In some cases, the test patterns are on break-off tabs that can be removed before the PCB is installed.

Layers may be connected together through drilled holes called vias. Either the holes are electroplated or small rivets are inserted. High-density PCBs may have blind vias, which are visible only on one surface, or buried vias, which are visible on neither, but these are expensive to build and difficult or impossible to inspect after manufacture. Good designers minimize the number of vias to reduce the cost of drilling. On older, two-layer PCBs, it was common to solder a wire through the hole.

A solder mask is a plastic layer that resists wetting by solder (the solder is said to "bead up"), and keeps islands of solder from running together. It also protects the outside conductors layers from abrasion and corrosion. Without the solder mask, the fiberglass-reinforced epoxy appears a translucent off-white. Solder masks are usually green, but they may be found in other colors.

A silkscreen legend on the top or bottom surface of the board provides readable information about component part numbers and placement. This aids in manufacturing and repair. To aid manual construction and repair, diodes, capacitors and integrated circuits are sometimes oriented in the same direction.

New technology allows for the component designators to be printed directly onto the board surface, saving time and money by doing away with silkscreens. This is sometimes done by a special inkjet printer. A similar process has experimentally produced solder masks.

Radio transmitters and radio receivers are difficult to design. PCB designers working on them must minimize parasitic effects due to layout of components, or take them into account with a general model and use simulation software such as SPICE.

Fortunately, many practical circuits can be laid out using a much simpler lumped element model.

PCB layout Basic guidelines:

  • it is often a good idea to have made a prototype circuit using point-to-point construction or wire wrap, as you will have solved certain basic issues to do with component selection: (eg: should I use a 1/4 watt resistor here, or do I need 1/2 watt? etc.)
  • consider physical constraints on the assembled board's size and heat dissipation requirements; choose your heat sinks if needed.
  • consider carefully the physical size of the components you are laying out; the circuit schematic doesn't tell you this. Equivalent components often have different packages.
  • How do the components attach to the board? Are they surface mount components? or do they require holes, screws, washers, etc?
  • are there mechanical parts directly mounted to the board? eg: switches or variable resistors?
  • How will the board mount in its container? What stresses (shock, strain, shear) will there be upon it and upon components?
  • How will the board connect to its power source? What other connectors will be required (e.g: signal inputs, outputs)?
  • use construction paper and a pencil and sketch the board in its actual size; or use component layout software that includes information about the component outlines.
  • decide appropriate widths for each of the signal traces; this depends on the current each trace is expected to carry.
  • decide whether you will have a single-layer board, 2-layer, or multi-layer based on the circuit complexity and fabrication costs.
  • begin by placing component outlines, then by placing signal traces; leave a little room around each for tolerances.
  • for a single layer board, spend more effort to avoid having traces cross each other; play with component placement or run traces underneath components; sometimes a jumper wire is needed.
  • in 2-layer and multilayer boards simply run the traces on different layers, and use plated-through holes to jump from one layer to another.
  • try to predict and avoid assembly errors: where there are multiple components of the same kind, or where pins have a polarity (eg: electrolytic capacitors), try to place them in parallel and orient the positive pin in the same direction.
  • If your PWB design software has a DRC (design rule check), use it.

PCB layout guidelines for RF circuits on a 2-layer or multilayer board:

  • identify the critical parts of the circuit and lay them out first
  • have one of the layers act as a continuous ground plane (usually the 'bottom' side).
  • if signal traces are constant width and height above the ground plane, and are properly terminated, then their characteristic impedance is more well-behaved and may be calculated.
  • avoid sharp corners.
  • keep signal traces and component leads as short as possible.
  • inputs and outputs should be far apart, so that RF energy will not leak back from output to input. stages should line up, rather than snake around.
  • decouple the RF parts of the circuit from the DC parts of the circuit.
  • shield AF and IF components from RF components.

[edit] further reading

Wikipedia-logo.png

Wikipedia has more about this subject:
Wikipedia-logo.png

Wikipedia has more about this subject:

[edit] references

  1. ↑ National Semiconductor knowledge base: "What is the translation between PCB copper thickness in ounces, inches, and mm?"
  2. ↑ Screaming Circuits: "LED and diode markation guidelines"
  3. ↑ Diversified Systems: "Production electronic assembly layout guidelines: Designating polarity"

[edit] Further reading

[edit] External links

[edit] Manufacturer design tips

Generally every PCB manufacturer gives some design for manufacturing tips on how to design things to fit their particular manufacturing process, for example

[edit] Other external links

Wikipedia-logo.png

Wikipedia has more about this subject:
Retrieved from "http://en.wikibooks.org/wiki/Practical_Electronics/PCB_Layout"
In other languages