PCB Design Resources

High Level Notes

Resource 1

1. The standards for PCB are controlled by IPC (www.ipc.org). IPC-2221 “Generic Standard on Printed Board Design”

Schematics

1. Good practice: Have signals flowing from inputs at the left to outputs on the right

2. Put bypass capacitors next to the component they are meant for.

3. Little notes on schematic that aid in the layout are very important. Eg, “this pin requires a guard track to signal ground”

Units

1. “thou” is 1/1000th of an inch. This is also known as “mils”

2. Use “mils/thous” for tracks, pads, spacings and grids which are most of your basic “design and layout” requirements.

3. Use “mm” for “mechanical and manufacturing” type requirements like hole sizes and board dimensions

4. 1.27mm = 50 mils

5. 100 mils = 0.1 inch = 2.54 mm

Grids

1. Layout your board on a fixed grid called as “Snap Grid”. Use a coarse grid for this, always.

2. 100 mils is standard placement grid for very basic through-hole pads

3. 50 mils being a standard for general tracing work, running tracks between through hole pads.

4. For finer work use 25 mils snap grid.

5. Coarse grid keeps components neat and symmetrical.

6. Good PCB layout practice would involve you staring out with a coarse grid like 50 mils and using a progressively finer snap grid if your design becomes “tight’ on space.

7. Drop to 25 or 10 mils for finer routing and placements when needed.

8. Make sure finer grid is a nice even division of your standard 100 mils. Never use anything else!

9. Some CAD tools have “Electrical Grids”, this grid is not visible, but it makes your cursor “snap” onto the center of electrical objects like tracks and pads, when your cursor gets close enough. Useful for manual routing, editing and moving objects

10. One more type of grid: “Component Grid”, works the same as snap grid, but only for components up to a different grid. Make sure it is a multiple of your snap grid.

Tracks

1. No recommended track sizes.

2. Bigger the track width, the better. They have lower DC resistance, lower inductance, can be easier and cheaper to manufacturer to etch and easier to inspect and rework.

3. Size of tracks depends on:
1. Electrical Requirements of design
2. Routing Space
3. Clearance

4. Lower limit of track width depends upon “track/space” resolution of PCB manufacturer.

5. 10/8 track/space figure means that tracks can be no less than 10 mils wide and the spacing between tracks (pads, or any part of copper) can be no less than 8 mils.

6. IPC standard recommends 4 mils as being the lower limit.

7. Don’t go lower than you need to for your track sizes.

8. Make tracks as big as possible and only change to thinner tracks only when required to meet clearance requirements

9. This “necking” is often required to meet clearance requirements.

1. Track width is dictated by the current flowing through it and the maximum temperature rise of the track you are willing to tolerate.

2. Thickness of copper on PCB is nominally specified in ounces per square foot. With 1 oz copper being most common.

3. Use calculator to calculate the track width required as the calculations to figure out a required track width based on the current and max temperature rise is a little complex.

4. A rule of thumb, a 10 degree C temperature rise in your track is a nice safe limit to design around.

Pads

1. Pad to Hole ratio is an important parameter. Each manufacturer has their own minimum specification for this.

2. Rule of thumb, pad should be at least 1.8 times the diameter of the hole or at least 0.5mm larger. This is for alignment tolerance on drill and the artwork on top and bottom layers.

3. Pad for leaded components should be round like resistors, capacitors and diodes. Around 70 mils diameter being common.

4. DIL (Dual In Line) components like IC’s are better suited with oval shaped pads (60 mils high by 90-100 mils wide)

5. Pin 1 of the chip should always be a different pad shape, usually rectangular and with same dimensions as other pins.

Vias

1. Generally vias are made with electrically plated holes, called Plated Through Holes (PTH). Plated through holes allow electrical connections between different layers on your board.

2. Practically there is no difference between a via and a pad. They are both electrically plated holes.

3. But CAD packages treat vias and pads differently.

4. Holes in vias are usually smaller than component pads typically around 0.5 - 0.7mm

5. Using a via to connect two layers is commonly called “stitching”

Polygons

1. A polygon automatically fills in a desired area with copper, which “flows” around other pads and tracks.

2. Useful for laying down ground planes.

3. Place this after you have placed all your tracks and pads

Clearances

1. Too tight a clearance between tracks and pads may lead to “hairline” shorts and other etching problems during the manufacturing process.

2. Don’t push the limits of your manufacturer unless you have to, stay above their recommended minimum spacing if at all possible.

3. 15 mils is good clearance limit for basic THT designs

4. 10 to 8 mils is used for more dense surface mount layouts.

5. 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.

6. Rule of thumb, an absolute minimum of 8mm (315 mils) spacing should be allowed between 240V tracks and isolated signal tracks. Good design practice would dictate much larger clearance anyways.

7. For non-mains voltages, IPC standard has a set of tables that define the clearance required for various voltages.

8. Clearance will vary depending on whether the tracks are on an internal layers or the external surfaces. It also varies with operational height of the board above sea level, due to thinning of the atmosphere at high altitudes.

9. Conformal coating improves these figures for a given clearance, and this is often used on military spec PCBs.

Component Placement & Design

1. PCB design is 90% placement and 10% routing.

2. Good component placement will make your layout job easier and give the best electrical performance.

3. Every designer will have their own method of placing components, and if you gave the same circuit to 100 different designers, you’d get a 100 different PCB layouts every time.

4. There is no absolute right way to place your components, but there are quite a few basic rules which will help ease your routing, give you the best electrical performance, and simplify large and complex designs.

5. Steps for laying out a complete board:
1. Set your snap grid, visible grid and default track/pad sizes
2. Throw down all the components onto the board
3. Divide and place your components into functional building blocks where possible
4. Identify layout critical tracks on your circuit and route them first
5. Place and route each building block separately, off the board
6. Move completed building blocks into position on your main board.
7. Route the remaining signal and power connections between blocks.
8. Do a general “tidy up” of the board
9. Do a Design Rule Check (DRC)
10. Get someone to check it

6. Partition off electrically sensitive parts of your design into bigger blocks. One major example is with mixed digital and analog circuits.

7. Another example is with high frequency and high current circuits, they do not mix with low frequency and low current sensitive circuits.

8. General rule, have your components neatly lined up, having ICs in the same direction, resistors in neat columns, polarised capacitors all around the same way, and connectors on the edge of the board.

9. Electrical parameters should always take precedence over nicely lined up components

10. Once you are done with component placements, you can start to route all the different building blocks separately. When finished, it is then often a simple matter to move and arrange the building blocks into the rest of your design.

11. DRC checks for correct connectivity of your tracks and for widths and clearances

Basic Routing

1. Keep nets as short as possible. Longer your total track length, the greater it’s resistance, capacitance and inductance.

2. Tracks should only have angles of 45 degrees. Don’t use 90 degree turns. Sharp right angle corners on tracks DON’T produce measurable EMI or other problems.

3. Nice rounded track corners, they are harder and slower to place and have no real advantage. Stick to 45 degree increments.

4. “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. First is that it is ugly. Second it is not very space efficient when you want to run more tracks on other layers.

5. Enable your Electrical Grid (or snap to center). 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.

6. Always take your track to the center of the pad. ALWAYS! Your program may not think that the track is making electrical connection to the pad.

7. Only take one track between 100 mils pads unless absolutely necessary. Only on large and very dense designs should you consider two tracks between pads.

8. 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.

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

10. 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.

11. 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.

12. Don’t leave any unconnected copper fills, ground them or take them out

Finishing Touches

1. If you have thin tracks (less than 25 mils) then it’s nice to add a “chamfer” to any “T” junctions, thus eliminating any 90 degree angles.

2. Check that you have any required mounting holes on the board. Keep mounting holes well clear of any components or tracks. Allow room for any washers and screws.

3. Minimise the number of hole sizes. Extra hole sizes cost you money. It also takes time for high speed drill to spin down and change drill bits.

4. Double check for correct hole sizes on all your components. Nothing is more annoying than getting your perfectly laid our board back from the manufacturer, only to find that a component won’t fit in the holes! This is a very common problem, don’t get caught out.

5. Ensure all your vias are identical, with the same pad and hole sizes. Remember your pad to hole ratio. Errors here can cause “breakouts” in your via pad, where the hole if shifted can be outside of your pad. With PTH it is not always fatal, but without a complete annular ring around your hole, your via will be mechanically unreliable.

6. Check that there is adequate physical distance between all your components. Watch out for components with exposed metal that can make electrical contact with other components, or exposed tracks and pads.

7. Change your display to “draft” mode, which will display all your tracks and pads as outlines. This will allow you to see your board “warts and all”, and will show up any tracks that are tacked on or not ending on pad centers.

8. If you wish, add “teardrops” to all your pads and vias. This gives more reliable track to pad interface. Don’t add teardrops manually though, it’s a waste of time. Use it if your program supports teardrop placement.

Single Sided Design

1. The smaller the number of jumpers used in a single sided design, the better

2. Component placement is even more critical on a single sided board, so making your components neatly aligned shouldn’t be of priority

3. Arrange your components so that they give the shortest and most efficient tracking possible. You have to think multiple steps ahead.

4. Be frugal in your placement, and don’t be afraid to rip everything up and try again if you see a better way to route something

Double Sided Design

1. Stick to using good component placement techniques and efficient building block routing.

2. You can also make use of good ground place techniques, required for high frequency designs.

Silkscreen

1. “Silkscreen” is also known as “Component Overlay” or “Component Layer”

2. It contains component outlines, designators (C1, R1 etc) and free text. It is added to your board using a silkscreening process

3. Keep all your component designators the same text size, and oriented in the same direction

4. Ensure all polarised components are marked. Pin 1 is identified.

5. Your silkscreen layer will be most inaccurately aligned of all your layers, so don’t rely on it for any positional accuracy.

6. Ensure no part of silkscreen overlaps bare pad.

7. There is no minimum width requirement for lines on the component overlay. If the text or lines don’t turn out perfectly on your board then it does not affect your design.

8. General rule, don’t put component values on the silkscreen, just the component designator

Solder Mask

1. It is a thin polymer coating on your board which surrounds your pads to help prevent solder from bridging between pins. This is essential for surface mount and fine pitch devices.

2. Solder mask typically covers everything except pads and vias. Your CAD package will automatically remove solder mask from pads and vias.

3. The gap it leaves between the pad and solder mask is known as the “mask expansion”. This value should be set at least to a few mils. Don’t make this too big, or there might be no solder mask between very fine pitch devices.

4. Normally you don’t need to put anything on your solder mask layer.

5. It is often handy to remove a small square of solder mask from the top of your board, where there are no tracks underneath. This leaves a nice bare and visible part of your board to write something with a pen.

6. There are two types of solder masks:
1. Silkscreen
2. Photo Imageable - Provide better resolution and alignment and are preferred over silkscreened.

7. You can get different color solder masks, but the standard color is green.

8. On most standard quality boards, the solder mask is laid directly over the bare copper tracks. This is known as Solder Mask Over Bare Copper or SMOBC.

9. You can get other coatings over your tracks in addition to the solder mask, but these are usually for fairly exotic applications.

10. You can have vias covered with solder mask if you wish, this is known as tenting. This is useful for close tolerance designs, to prevent solder from flowing into vias.

Mechanical Layer

1. May have other name in different CAD package.

2. Used to provide outline for your board, and other manufacturing instructions.

3. Not part of your actual PCB design, but is very useful to tell the PCB manufacturer how you want your board to be assembled.

Keepout

1. Area on your board that you don’t want auto or manually routed.

2. This can include clearance areas around mounting hole pads or high voltage components for instance.

Layer Alignment

1. While manufacturing there will be an alignment tolerances on the artwork film for each layer. This includes track, plane, silkscreen, solder mask and drilling.

Netlists

1. A netlist is a list of connections (nets) which correspond to your schematic.

2. It also contains the list of components, component designators, component footprints and other information related to your schematic.

Design Rule Checking

1. Circuit connectivity. It checks that every track on your board matches the connectivity of your schematic

2. Electrical clearance. You can check the clearance between tracks, pads and components.

3. Manufacturing tolerances like min/max hole sizes, track widths, annulus sizes, and short circuits.

4. Real time DRC can check all of this while you are laying out your PCB. Which is even better.

5. Usually DRC is done when you are done with your design.

Forward and Back Annotation

1. Forward annotation is when you make changes to your existing PCB layout via the schematic editor.

2. If you update your schematic, the you must forward annotate into your PCB design.

3. Back annotation is when you change one of the component designators (Eg, C1 to C2) on your PCB and then automatically update this information back into your schematic.

4. There shouldn’t be much real need to use back annotation.

Good Grounding

1. Use copper, lots of it. The more copper you have in your ground path, the lower the impedance. This is highly desirable for many electrical reasons. Use polygon fills and planes where possible.

2. Dedicate one of your planes to ground on multi-layer boards. Make it the layer closest to the top layer.

3. Run separate ground paths for critical parts of your circuit, back to the main filter capacitor(s). This is known as “star” grounding , because the ground tracks all run out from a central point, often looking like a star. Try to do this even if you components aren’t critical.

4. Separate ground lines keep current and noise from one component from affecting other components

5. If using a ground plane, utilise “split” plane techniques to give effective star grounding.

6. “Stitch” required points straight through to your ground plane, don’t use any more track length than you need.

7. Use multiple vias to decrease your trace impedance to ground

Good Bypassing

1. Active components and points in your circuit which draw significant current should always be “bypassed”. This is to “smooth” out your power rail going to a particular device.

2. “Bypassing” is using a capacitor across your power rails as physically and electrically close to the desired component or point in your circuit as possible.

3. A typical bypass capacitor value is 100 nF, although other values such as 1 uF, 10 nF and 1 nF are often used to bypass different frequencies.

4. You can even have two or three different value capacitors in parallel.

5. When bypassing, you CANNOT replace multiple capacitors with one single capacitor, it defeats the entire purpose of bypassing!

6. As a general rule, you should use at least one bypass capacitor per IC or other switching component if possible.
1. 100 nF - General Purpose
2. 10 nF or 1 nF - High Frequency
3. 1 uF or 10 uF - Low Frequency
4. Special low ESR (Equivalent Series Resistance) - Used on critical designs such as switch mode power supplies

High Frequency Design Techniques

1. High frequency design is where you really need to consider the effects of parasitic inductance, capacitance and impedance of your PCB layout.

2. If you signal is too fast, and your track is too long, then the track can take on the properties of a transmission line

3. If you don’t use proper transmission line techniques in these situations then you can start to get reflections and other signal integrity problems.

4. A “critical length” track is one in which the propagation time of the signal starts to get close to the length of the track.

5. On standard FR4 copper boards, a signal will travel roughly 6 inches every nanosecond. A rule of thumb states that you need to get concerned when you track length approaches half of this figure.

6. Remember that digital square wave signals have a harmonic content, so a 100 MHz square wave can actually have signal components extending into the GHz region.

7. In high speed design, the ground plane is fundamental to preserving the integrity of your signals, and also reducing EMI emissions.

8. Ground planes allow you to create “controlled impedance” traces, which match your electrical source and load. It also allows you to keep signals coupled “tight” to their return path (ground).

9. There are many ways to create controlled impedance transmission lines on a PCB. Two most popular ways are:
1. Microstrip - Simply a trace on the top layer, with a ground plane below. The calculation to find the characteristic impedance of a microstrip is relatively complex. It is based on the width and thickness of the trace, the height above the ground plane, and the relative permittivity of the PCB material.
2. Stripline - Similar to microstrip but has a ground plane on top of the trace. So in this case, the trace would have to be on one of the inner layers. The advantage of stripline over microstrip is that most of the EMI radiation will be contained within the ground planes.

10. There are many free programs and spreadsheets available that will calculate all the variations of microstrip and stripline for you.

11. Keep your high frequency signal tracks as short as possible

12. Avoid running critical high frequency signal tracks over any cutout in your ground plane. This causes discontinuity in the signal return path, and can lead to EMI problems.

13. Avoid cutouts in your ground plane wherever possible. A cutout is different from a split plane, which is fine, provided you keep your high frequency signal tracks over the relevant continuous plane.

14. Have a decoupling capacitor per power pin.

15. If possible, track the IC power pin to the bypass capacitor first, and then to the power plane. This will reduce switching noise on your power plane.

16. For very high frequency designs, taking your power pin directly to the power plane provides lower inductance, which may be more beneficial than lower noise on your plane.

17. Be aware that vias will cause discontinuities in the characteristic impedance of a transmission line.

18. To minimise crosstalk between two traces above a ground plane, minimise the distance between the plane and trace, and maximise the distance between traces. The coefficient of coupling between the traces is given by

1. Smaller diameter vias have lower parasitic inductance, and are this preferred the higher in frequency you go.

2. Do not connect your main power input connector directly to your power planes, take it via your main filter capacitor(s).

Double Sided Loading

1. Often times, with dense high speed surface mount devices packed onto a board, there is either no room for the many bypass capacitors required, or they cannot be placed close enough to the device to be effective.

2. BGA devices are one such component that benefit from having bypass capacitors on the bottom of the board.

DFM: Panelisation

1. If you are looking at getting your board automatically assembled with a pick-and-place machine, then it pays you to get as many boards onto the one “panel” as you can.

2. A panel contains many identical copies of your board.

3. A panel will also contain tooling strips on the top and bottom, to allow for automated handling of the panel.

4. Each individual board can be “routed out” and joined with “breakout tabs”, or simply butted together and scoured out with a “V groove”.

5. A V groove is a score mark placed on your board that allows you to easily “snap” the board along the groove.

6. A breakout tab is a small strip of board perhaps 5-10 mm long joining your board to your panel. Small non-plated holes are also drilled along this strip, which allows the board to be snapped or cut out of the panel after assembly.

DFM: Tooling Strips

1. These are strips of blank board down the top and bottom side of your board. They contain tooling holes, fiducial marks, and other manufacturing information if required.

2. Standard tooling holes are required for automated handling of your board. 2.4mm and 3.2,, are two standard hole sizes.

DFM: Fiducial Marks

1. These are visual alignment aids placed on your PCB. They are used by automated pick and place machines to align your board and find reference points.

2. A video camera on pick and place machine identifies the center of fiducial marks and use these points as aa reference.

3. On a panel there should be three fiducial marks, known as global fiducials.

4. The fiducial mark should be a circular pad on the copper layer of diameter 1.5 mm typically.

5. The fiducial should not be covered with solder mask, and the mask should be removed for a clearance of at least 3 mm around.

6. Two local fiducials (one in opposite corners) is also required next to each large fine pitch surface mount device package on your board.

DFM: Thermal Relief

1. If you solidly connect a surface mount pad to a large copper area, the copper area will act as a very effective heat sink. This will conduct heat away from your pad while soldering. This can encourage dry joints and other soldering related problems.

2. For such cases, thermal relief connection, which comprises several (usually 4) smaller tracks connecting the pad to the copper plane. Thermal relief options can be set automatically in many packages

DFM: Soldering

1. There are three basic soldering techniques:
1. Hand - Prototype and small production runs
2. Wave - Used for surface mount and through hole production soldering.
1. It involves passing the entire board over a molten bath of solder. Solder masks are absolutely essential here to prevent bridging.
2. Ensure small components are not in the wave solder shadow of larger components.
3. The board travels through wave solder machine in one direction. So there will be a lack of solder trailing behind larger components
4. Surface mount devices are fixed to the board with an adhesive before wave soldering
3. Reflow - Latest technique, and is suitable for all surface mount components.
1. Blank board is first coated with a mask of solder paste over the pads (solder “stencils” are used)
2. Then each component is placed and is sometimes held in place with an adhesive
3. The entire board is loaded into an infrared or nitrogen oven and “baked”
4. The solder paste melts (reflows) on the pads and component leads to make the joints.
5. A newer reflow method called pin-in-paste or intrusive reflow is available for through hole devices.

2. Wave soldering has the advantage of being cheap, but the disadvantage of imposing placement limits on your components.

3. Reflow soldering is more complex and expensive, but it allows for very dense surface mount packing.

Basic PCB Manufacturing

1. A PCB consists of a blank fibreglass substrate (the board) which is usually 1.6mm thick. Other thicknesses are 0.8 mm or 2.4 mm.

2. There are many PCB substrate material, but by far the most common is a standard woven epoxy glass material known as FR4.

3. The most often used parameter is probably the dielectric constant. This is important for calculating high speed transmission line parameters and other effects.

4. Other exotic base materials like Teflon is also available, but are only used for special designs that require a higher grade base material for a specific reason.

5. There are cheaper materials than FR4 like phenolic base and CEM-1. These are hobbyist board grade base material. But are also often used in some mass consumer products due to their low cost. They are not suitable for plated through holes or fine tolerance designs.

6. A blank base material coated with copper is known as copper clad board.

7. A multi-layer board is made up of various individual boards separated by Preimpregnated Bonding Layers also known as prepreg.

Surface Finishes

1. You can get your PCBs manufactured with several different types of pad and track finishes.

2. Very low cost single and double sided boards without solder mask typically have a basic tin coated finish. Beware of potential shorts between tracks with this method.

3. Standard professionally manufactured board will typically have solder mask over bare copper (SMOBC) tracks and tin finish on the pads and vias which is Hot Air Leveled (HAL).

4. Hot air leveling helps most surface mount components to sit flat on the board.

5. For large and critical surface mount components, a gold “flash” finish is used on the pads. This gives an extremely flat surface finish for dense fine pitch devices.

6. Peelable solder masks are available, and are handy for temporary masking of areas on your board during wave soldering or confrol coating.

Electrical Testing

1. You can have your PCBs checked for electrical continuity and shorts at the time of manufacture.

2. This is done with an automated “flying probe” or “bed of nails” test machine.

3. It checks that the continuity of the tracks matches your PCB file. It may cost a fair bit extra, but this is pretty mandatory for multi-layer boards.

4. If you have a manufacturing error on one of your inner layers, it can be very difficult to fix.

Resource 2

1. First use of Earth was as a return path for lightning energy.

2. Later people used the Earth as a return path for telegraph signals. Although its not a great return path, it is an adequate return path under certain circumstances.

3. For modern electronics, Earth is only used for safety and that is its only role, it has nothing todo with passing EMI tests.

4. Sometimes if you don’t connect the Earth properly, it might become the source of EMI problem by acting like an antenna. When you connect this third wire, you have put some inductance in the wire so that it would prevent the device from sending high frequency energy back down the wire. Since its a high frequency signal, it would receive high impedance while going to the earth and hence start to radiate EM waves and cause EMI problems.

5. The chasis of the system is neither “Earth Ground” or “Chasis Ground”. The function of the metal box is to behave like a faraday cage. Keep intended fields inside and unintended fields outside.

6. “Ground” on PC Boards is often considered a region of ZERO Volt Potential with ZERO resistance, ZERO impedance etc. NOT TRUE!!!

7. When you send energy down a transmission line and you get current in ground that current causes a voltage drop. That means from one point to another the ground potential difference is never exactly zero volts. Close but never zero. This statement is only close to true for DC!

8. As you go up in frequency ground is anything but zero volts and zero impedance.

9. “Ground” is often thought of as a place to attach components to bleed off or filter noise as if it is a sink hole that eliminates noise from circuits. NOT TRUE!!!

10. Where is the energy in the circuit? Is it in the voltage or in the current? Actually it’s neither.

11. Energy is entirely in the fields. Better known as the Electric (E) Field and Magnetic (H or B) Fields.

12. Where are the fields located in a circuit board? In the traces? In the planes? Actually it’s neither

13. Energy does not travel in the copper at all, the energy travels in the space between traces and the planes. It travels in the dielectric.

14. The energy in a circuit travels in the plastic and fibreglass material of the PCB. No energy travels in the copper.

15. The energy (E & H/B Fields) in a transmission event is called a Wave, an Electro-Magnetic Wave.

16. The traces or the trace and plane that make up the transmission line steer the energy from point A to point B. These copper elements act as wave guides!

17. Why does energy follow the trace? Because it’s the path of lowest impedance!

18. We can launch energy into dielectric without traces? Yes we can, when we launch signals into air for radio and television broadcast.

19. Energy in air travels approximately close to the speed of light. And it travels approx. at half the speed of light in FR4.

20. A transmission line (or a wave guide, both are the same) is a pair of conductors or wires used to move energy from point A to point B!
1. There is voltage across the copper and current in the copper!
2. The E & H Fields are travelling in the dielectric

21. A common misconception is when you launch energy into the circuit, the current travels down the trace to the load and then comes back up the ground trace back to the driver. This is NOT how it works.

22. The energy is launched into the circuit in the form of waves consisting of fields. These fields create a voltage across both copper features at the same time and they create a forward and a return current in both copper feature simultaneously.

23. So the return current is formed at the same time as the forward current in the transmission line. It is a simultaneous event.

24. How we take care of the return side or ground makes a big difference as to how things will perform.

25. When no energy is launched into the trace.

1. When you launch energy into the transmission lines, the first thing that appears is the electric field.

2. The energy in the field excites the electrons in the copper (electrons in the atoms). They start to move causing current flow in the copper of the planes and in the copper of the trace.

3. Reaction to that is to form a magnetic field which surrounds the trace and is sandwiched between the trace and the planes. Notice all the energy is between the trace and the plane.

4. Also notice that it also spreads out a little bit, it isn’t contained exactly under the trace and plane. There is a spreading of energy, this is what causes crosstalk and other forms of interference if we get things to close to one another.

5. These are the fields of an outer layer transmission line, a trace routed above a ground plane and layer two of a board. The fields expand more and it does cause some radiation from the outer surface of the board. And this is a problem in some cases. This by itself will never cause you to fail EMI, but it will exacerbate an existing problem when you have one.

6. Fields expand in outer layers, crosstalk is worse on outer layers

Resources

1. PCB Design Tutorial - David L Jones - Link

2. How to Achieve Proper Grounding - Rick Hartley - Link