The Board Design Guidelines Solution Center provides you with board design-related resources for Intel® devices. Its goal is to help you implement successful high-speed PCBs that integrate device(s) and other elements.

## Target Impedance Decoupling Method

An efficient strategy for determining the PCB decoupling scheme is to use the Frequency Domain Target Impedance Method (FDTIM). This method is used by the PDN Decoupling Calculator Tool and is the recommended method for determining the board-level decoupling requirements using  Intel FPGAs.

### FDTIM Decoupling Concepts

The key concept of the FDTIM method is the determination of the target impedance (ZTARGET) for the power rail under consideration. A reliable decoupling strategy warrants for the effective power rail impedance (ZEFF) to be lower than the ZTARGET from a few KHz up to the highest frequency of interest (fTARGET). Figure 1 illustrates this concept, where the solid horizontal blue line is the ZTARGET and the dotted vertical brown line is the fTARGET. The solid red ZEFF line has been designed by using various decoupling and bulk capacitors such that its impedance remains below the ZTARGET from DC up to fTARGET. With this design, power integrity is achieved from DC up to the target frequency of decoupling. To design a reliable decoupling scheme using the FDTIM, perform the following calculations:

Determine ZTARGET

To calculate ZTARGET for a power rail, you must know the following information:

• Maximum transient current requirements for all devices in the system that are powered by the power rail under consideration. You can get this information the from manufacturers of the respective devices. Note: You can download the PowerPlay Early Power Estimator (EPE) tool to estimate power consumption for all its FPGAs and CPLDs.
• Maximum allowable AC ripple on the power rail as a percentage of the supply voltage. You can get this information from the power supply tolerance specifications of the devices being supplied by the power rail under consideration.
• ZTARGET= [VoltageRail (%Ripple/100)/MaxTransientCurrent]
• ZTARGET= [(1.1)(0.05)/1.5]=36.7mΩ

If this information is available, then ZTARGET can be calculated as:

• ZTARGET= [VoltageRail (%Ripple/100)/MaxTransientCurrent]
For example, to reliably decouple a 1.1-volt power rail that allows 5 percent of AC ripple and is expected to supply a maximum transient current of 1.5 A, the target impedance is:
• ZTARGET= [(1.1)(0.05)/1.5]=36.7mΩ

Determine fTARGET

The highest frequency of interest is the point in frequency after which adding a reasonable number of decoupling capacitors does not bring down the power rail impedance (ZEFF) below the target impedance (ZTARGET) due to the dominance of the parasitic planar spreading inductance and package mounting inductances. Typically, this fTARGET ranges from 50/60 MHz to 150/200 MHz. Beyond these frequencies, it is expected that power integrity is maintained and performed by the on-package and on-die capacitors of the selected target devices.

Select Decoupling CAPS to Meet ZTARGET

To maintain power integrity throughout the entire frequency range of interest, the Power Distribution System relies on the voltage regulator module (VRM), the on-board discrete decoupling capacitors, and inter-plane capacitances (capacitance from the power-ground sandwich in the board stack-up). For the above example, the designer must select these appropriately so that the effective impedance remains below 36.7 Ω within the entire frequency range of interest.

For more details on applying the FDTIM, refer to the  PDN Decoupling Calculator Tool and its corresponding User Guide.

## Plane Capacitance

For high frequencies, decoupling using discrete capacitors is less effective. Use power plane capacitance for decoupling noise at these frequencies. You can understand the concept of plane capacitance by studying the classic parallel plate capacitor, shown in Figure 1.

Figure 1. Parallel Plane Capacitance An electric field is created when there is a power plane next to a ground plane. The upper area in Figure 1 shows the power island or plane, the lower area shows the ground plane, and the arrows represent the electric field lines. This electric field gives rise to a capacitance, the magnitude of which is shown by the following equation:

C=(εοεrA)/h

Where

• εο = permittivity of free space
• εr = relative permittivity of the dielectric used
• A = area of overlap
• h = separation of the planes.

If there are ground planes on both sides of the power island, then the capacitance needs to be calculated for each side and added to determine the total capacitance.

Plane capacitance is the primary way of decoupling at high frequencies, so it must be an integral part of any high-speed design. At high frequencies, the discrete capacitors are not very effective.

As an example, consider the following.

Example: Determine the parallel plate capacitance for 1 square inch of area overlap in an FR-4 dielectric (εr = 4.5) and a separation of 4 mils.

Solution:

• h = 4mils = 1.016 * 10-4 m
• εο = permittivity of free space = 8.85 * 10-12 F/m
• A = 1 sq inch = 6.4516 * 10-4 m2
• εr = 4.5

Applying these numbers to the capacitance equation above yields C = 253 pF.  Therefore, there is about 253 pF per square inch of area overlap on a typical FR-4 board with 4 mils of separation.  The value scales inverse linearly with separation and linearly with area.

## Minimization Parasitic Inductances

The goal of a Power Distribution System (PDS) is to provide and maintain a target constant voltage at the power and ground pads of each device. To effectively accomplish this, the PDS relies on the Voltage Regulator Module (VRM), the bulk and decoupling capacitors (Decaps) and the power and ground plane sandwich (plane capacitance). How effectively each of these components perform their job in helping to maintain a constant voltage under varying transient loads depends highly on their associated parasitic inductances.

VRM

As a first-order approximation, the VRM can simply be modeled as a series connected resistor and inductor, as shown in Figure 1.

Figure 1. Series Impedance Model of a VRM At low frequencies in the range of tens of KHz, the VRM, being primarily resistive, provides very low impedance and thus it is capable of providing the instantaneous current requirements at these lower frequencies. However, beyond a few tens of KHz, the VRM impedance being primarily inductive makes it incapable of providing the transient current requirements. You can get the ESR and ESL values of the VRM from the VRM manufacturer and you can choose a low ESR/ESL regulator for best transient performance.

Decaps

The on-board discrete decoupling capacitors must provide the required low impedance from a few tens of KHz to about a couple of hundred MHz (maximum) depending upon the capacitor ESR and ESL as well as board mounting and spreading inductance parasitics. Even choosing decoupling capacitors with very low ESR and ESL specifications is not enough as the contribution of the parasitic mounting and spreading inductances can limit the effectiveness of these capacitors. Hence, to design an effective PDS, care must be taken to minimize the various parasitic inductances associated with the design of the board.

Mounting Inductance

Mounting Inductance is the additional series inductance contribution associated with the mounting of the capacitor on the PCB. This parasitic inductance adds to the published ESL value that is provided by the cap vendor. Mounting inductance can be minimized by choosing smaller capacitor packages and performing proper layout of the capacitor on the PCB. Figure 2 shows the cross-section of a mounted decoupling capacitor in relation to the PCB planes and BGA device.

Figure 2. Decoupling Cap Mounting To estimate the mounting inductance, use the following equation:

• Lmnt = Ltrace + Lvia

Where,

And,

• Lvia = 10*htop*ln(2s/D) ph

Where,

• Lenpad = Length of the capacitor pads plus trace length from pad to the via (mils)
• Lencap = Length of the capacitor body (mils)
• w = Width of the trace between the capacitor pad and via (mils)
• htop = Distance between the top layer and the nearest power/ground plane (mils)
• s = Distance between the capacitor's power via center and ground via center (mils)
• D = Outer diameter of the via (mils)
• hplanes = Distance between the power and ground plane (mils)
• b = Half the distance between the capacitor and the package power/ground vias (mils)

Generally, to minimize the mounting inductance, keep the capacitors power and ground vias as close as possible to its respective pad and use wide connecting traces and larger via drill diameters, if possible. Placing power and ground plane pairs closer to the surface where the capacitor is mounted reduces the via inductance contribution. Additionally, placing the vias on the same sides of the capacitor (via-on-side configuration) as opposed to the opposite ends of the capacitor (via-on-end configuration) reduces the current loop area, minimizing the amount of flux lines that penetrate the loop and thus reduces the inductance. Figure 3 illustrates the various capacitor layout topologies while Table 1 compares mounting inductances of those various cap layout styles for different size capacitors.

Figure 3. Various Capacitor Layout Topologies •
Via Length 0603 0603 0603 0603 0402 0402 (height above plane,inches) footprint footprint footprint footprint footprint footprint Table 1. Mounting Inductance Comparison (1) 0.020 drill Thin trace from pad to via Short thick trace Via on the end of pads Via on the side of pads Via on the end of pads Via on one side of pads 0.004 1.57 1.04 0.82 0.52 0.8 0.5 0.006 1.96 1.35 1.05 0.65 1 0.63 0.01 2.51 1.87 1.4 0.88 1.34 0.86 0.02 3.45 2.87 2.13 1.39 1.99 1.36 0.010 drill 0.004 1.61 1.08 0.86 0.56 0.84 0.54 0.006 1.99 1.39 1.08 0.69 1.04 0.67 0.01 2.55 1.92 1.45 0.92 1.38 0.9 0.02 3.49 2.91 2.17 1.44 2.03 1.4

Note:

• All Values are in nano-Henries and drill sizes are in inches

As shown in Table 1, the optimum mounting inductance of 0.50 nH is obtained when the smaller 0402 size capacitor is mounted using the via-on-side scheme with wide connecting traces to the larger 20 mil via drill diameter. Figure 4 shows other recommended via placement configurations that further reduce mounting inductance. However, these styles require additional vias and hampers routability.

Figure 4. Via placement Styles that Yield Lower Mounting Inductance Spreading Inductance is the inductance formed by the loop area between the power-ground plane pair and the distance from the decoupling cap to the power-ground balls of the target BGA device. As a result, this inductance is directly related to the inductance of the inter-plane capacitance formed by the power-ground sandwich. This inductance is explained in detail in the inter-plane capacitance section below.

Inter-Plane Capacitance

As a first-order analysis, the PCB power-ground plane pair can simply be modeled as a series connected resistor, inductor, and, capacitor as shown in Figure 5. Note that this simple model ignores the frequency dependent effects such as skin effect and dielectric absorption.

Figure 5. Simplified Impedance Model of the Power-Ground Plane Sandwich The first-order equations for the ESL in Figure 5 is shown below:

• ESL = (μ0•h•l)/w

Where,

• μ0 = magnetic permeability of free space (32 pH/mil)
• h = distance between the power and ground planes in mils
• l = length of the power plane in inches
• w = width of the power plane in inches

You can interpret the ESL of the power-ground plane sandwich as the spreading inductance that the decoupling capacitor sees as it is supplying current to the BGA device. Therefore, from the ESL equation above, the spreading inductance can be reduced by placing the decoupling capacitors as close as possible to the target BGA device (minimizing the distance l from the cap to the BGA device). Additionally, using a thin dielectric material (minimizing h) and wide plane pairs (maximize w) for the power-ground plane sandwich helps reduce the effective spreading inductance seen by the decoupling capacitor.

Conclusion

To successfully design an effective PDS requires an understanding of the various parasitic inductances that can limit the performance of the PDS. This document explains three parasitic inductances that you must be concerned with in designing the PDS. VRM parasitic inductance, decoupling capacitor mounting inductance, and power plane spreading inductance are examined and techniques to minimize them are presented. For additional information and tools, download the PDN Decoupling Calculator tool and user guide

### Routing Guidelines for Gigabit Channel Designs

Via Optimization Techniques

• General Routing Guidelines

This section provides a summary of routing guidelines for laying out high-speed differential pair traces.

• Use tight coupling for differential traces as much as possible. If it is not possible to maintain tight coupling throughout the trace length, use loose coupling for the entire trace. Figure 1 shows 3.125-Gbps differential transceiver traces, which are loosely coupled on layer 15 and the top layer of the Stratix® GX development board. Tight coupling is not possible on the top layer because of the minimum separation required (because of the mechanical constraints of the SMA connectors). If you used tight coupling on layer 15, the signal would need to transition from tight to loose coupling, which would introduce impedance discontinuities.
• Figure 1. Loose Coupling and Ground Reference Example • Microstrip and stripline transmission lines are both fine for routing. Stripline has the added benefit of shielding the signals from other noise sources. The constraints during layout design often dictate on which layer to do the routing.
• Use rounded corners while routing. Do not use 90° bends, which introduce impedance discontinuities. A 45° bend provides a compromise, but rounded corners offer the best performance.
• Both broadside and edge coupling are fine. Generally, broadside coupling makes it easy to route out of the BGA, but requires more layers. Edge coupling makes it harder to route out of the BGA, but requires fewer layers. Both provide acceptable signal integrity performance.
• Do not allow high-speed signals to cross over plane splits. A crossover causes signals to see a longer return path, which increases trace inductance. The increased inductance changes the impedance of the line, causing signal integrity problems.
• Remove all unused via pads during the manufacturing process. Some fabrication houses refer to unused via pads as "nonfunctional via pads." Unused via pads add additional capacitance on the signal path. Figure 2 shows examples of unused via pads.
• Figure 2. Unused Via Pads • If the signal must be routed through a via, route it so that the via stub length is minimized. The option shown in Figure 3 minimizes the via stub length and is preferred over the option shown in Figure 4. This technique is used in the Stratix GX development board. The high-speed traces were taken to layer 16 from the top layer through the vias to use as much of thevia length as possible and to minimize the stubs.

Figure 3. Optimal Routing Path with Through-Hole Vias Figure 4. Sub-Optimal Routing Path with Through-Hole Vias • For dual stripline traces (Power 1 – Signal 1 – Signal 2 - Power 2 configuration), ensure that the signals on the Signal 1 layer are orthogonal to the signals on the Signal 2 layer if they cross each other.  If they do not cross each other, ensure that they are at least 4W away, where W is the width of the traces.
• Use "tear-dropping" to reduce impedance discontinuity when going from a wide pin and trace to a narrow pin or trace. For example, when you interface an SMA connector to a trace, use tear-dropping. Figure 5 shows the dimensions of an SMA connector and a screen capture of tear-dropping on the Stratix GX development board. The SMA connector has a 50-mil diameter center pin, but the board traces might be 5-mils wide. Tear-dropping helps minimize the impedance discontinuity.

Figure 5. SMA Tear-dropping ### Transmitter Pre-Emphasis and Receiver Equalization

Typical transmission media like copper trace and coaxial cable have low pass characteristics, so they attenuate higher frequencies more than lower frequencies. A typical digital signal that approximates a square wave contains high frequencies near the switching region and low frequencies in the constant region. When this signal travels through low pass media, its higher frequencies are attenuated more than the lower frequencies, resulting in increased signal rise times. Consequently, the eye opening narrows and the probability of error increases.

The high-frequency content of a signal is also degraded by what is called "skin effect." The cause of skin effect is the high-frequency current that flows primarily on the surface (skin) of a conductor. The changing current distribution causes the resistance to increase as a function of frequency.

You can use pre-emphasis to compensate for the skin effect. By Fourier analysis, a square wave signal contains an infinite number of frequencies. The high frequencies are located in the low-to-high and high-to-low transition regions and the low frequencies are located in the flat (constant) regions. Increasing the signal's amplitude near the transition region emphasizes higher frequencies more than the lower frequencies. When this pre-emphasized signal passes through low pass media, it will come out with minimal distortion, if you apply the correct amount of pre-emphasis. See Figure 1 for a graphical illustration of this concept.

Figure 1. Input and Output Signals with and without Pre-Emphasis Stratix II GX and Stratix IV GX devices provide programmable pre-emphasis to compensate for variable lengths of transmission media. You can set the pre-emphasis to be between 5 percent and 25 percent, depending on the value of the output differential voltage (VOD). Please refer to the Stratix II GX and Stratix IV GX user guides.

### Unused I/O Pins Guidelines

To allow flexibility in board design, you can specify the state of unused pins as one of the following five states in the Quartus® Prime or Quartus II software: as inputs that are tri-stated, as outputs that drive ground, as outputs that drive an unspecified signal, as input tri-stated with bus-hold, or as input tri-stated with weak pull-up resistors. To improve signal integrity, set unused pins as outputs that drive ground and tie them directly to the ground plane on the board. Doing so reduces inductance by creating a shorter return path and reduces noise on the neighboring I/O. To reduce power dissipation, set clock pins to drive ground and set other unused I/O pins as inputs that are tri-stated. To make the setting that is appropriate for your design, choose one of the five allowable states for Reserve all unused pins on theUnused Pins tab in the Device & Pin Options dialog box, or apply the Reserve Pin assignment to specific pins in the Pin Planner.

When you compile your design, the software generates the pin report file (.pin) to specify how you should connect the device pins. Unused I/O pins are marked in the report file according to the unused pins option you set in the software. All I/O pins specified as GND* can either be connected to ground to improve the device's immunity to noise, or left unconnected. Leave all RESERVED I/O pins unconnected on your board because these I/O pins drive out unspecified signals. Tying a RESERVED I/O pin to VCC, ground, or another signal source can create contention that can damage the device output driver. You can connect RESERVED_INPUT I/O pins to a high or low signal on the board, while RESERVED_INPUT_WITH_WEAK_PULLUP and RESERVED_INPUT_WITH_BUS_HOLD pins can be left unconnected.

### Device Breakout Guidelines

Board Design Process Overview

A typical high-speed board design begins with a product requirements document, a concept review, and a functional specification. After the specification is finalized, actual system design begins with the selection of key components. At this point, timing analysis for all the interfaces and power analysis — to determine the power requirements — is performed. Based on the power analysis, power supply modules and regulators are chosen, and a decoupling scheme is specified. Based on the timing analysis, a length-matching criterion for the buses is established. Upon completion of these tasks, as well as completion of the system design and selection of remaining components, the schematics are created. These are typically reviewed among engineers who make any necessary changes, after which they are given to the layout designer. A layout guidelines document, which specifies how to place components on the board and how to route the traces, is created and given to the layout designer as well.

A pre-layout simulation is performed to determine the ideal stack-up, trace widths, spacing, and other routing requirements. Any changes to the schematic, based on the simulation results, are incorporated in the schematic and provided to the layout designer. When the layout is complete, a post-layout simulation is performed on the critical sections of the board to ensure that there are no major signal integrity problems.

Based on the results of the post-layout simulation, any changes required are incorporated into the layout, and finally the layout is released to the fabrication house for board manufacturing. Figure 1 shows typical board design process.

Figure 1. Simplified View of a Typical High-Speed Board Design Process • Material Selection and Loss
•

• Cross Talk Minimization

Crosstalk is the unwanted coupling of signals between parallel traces. Proper routing and layer stack-up through microstrip and stripline layouts can minimize crosstalk.

To reduce crosstalk in dual-stripline layouts, which have two signal layers next to each other (see Figure 1), route all traces perpendicular, increase the distance between the two signal layers, and minimize the distance between the signal layer and the adjacent reference plane.

Figure 1.  Dual-Stripline Layout Use the following steps to reduce crosstalk in either microstrip or stripline layouts:

Crosstalk also increases when two or more single-ended traces run parallel and are not spaced far enough apart. The distance between the centers of two adjacent traces should be at least four times the trace width, as shown in Figure 2. To improve design performance, lower the distance between the trace and the ground plane to under 10 mils without changing the separation between two traces.

Figure 2.  Separating Traces for Crosstalk •
• Widen spacing between signal lines as much as routing restrictions will allow. Try not to bring traces closer than three times the dielectric height.
• Design the transmission line so that the conductor is as close to the ground plane as possible. This technique will couple the transmission line tightly to the ground plane and help decouple it from adjacent signals.
• Use differential routing techniques where possible, especially for critical nets (i.e., match the lengths as well as the gyrations that each trace goes through).
• If there is significant coupling, route single-ended signals on different layers orthogonal to each other.
• Minimize parallel run lengths between single-ended signals. Route with short parallel sections and minimize long, coupled sections between nets.
•

• Power Filtering/Distribution

Clean, evenly distributed power to VCC on all boards and devices can reduce system noise.

Filtering Noise

To diminish the low-frequency (< 1 kHz) noise caused by the power supply, filter the noise on the power lines at the point where the power connects to the PCB and to each device. You may place a 100-μF electrolytic capacitor adjacent to the location where the power supply lines enter the PCB. If using a voltage regulator, place the capacitor immediately after the final stage that provides the VCC signal to the device(s). Capacitors not only filter low-frequency noise from the power supply, but also supply extra current when many outputs switch simultaneously in a circuit.

Another way to filter power supply noise is to place a non-resonant surface-mount ferrite bead, big enough to handle the current, in series with power supply. Place a 10-μF to 100μF bypass capacitor next to the ferrite bead (see Figure 1). Proper terminations, layouts, and filtering in a design eliminate the need for the ferrite bead. In this case, use a 0-Ω resistor instead of the ferrite bead.

Figure 1.  Filtering Noise with Ferrite Bead PCB elements add high-frequency noise to the power plane. To filter high-frequency noise at the device, place decoupling capacitors as close as possible to each VCC and ground pair. Placing the power and ground planes in parallel and separated by dielectric material provides another level of bypass capacitance. These parallel planes reduce the power-related high-frequency noise, since this type of capacitance has no effective series resistance (ESR) and no lead inductance.

Distributing Power

Power distribution also impacts system noise. Either a power bus network or power planes can distribute power throughout the PCB. Usually used on two-layer PCBs, the least expensive way to distribute power is a power bus network, which consists of two or more wide metal traces that carry VCC and ground to the devices. The density of the PCB limits the trace widths, which should be as wide as possible. Power buses have significant DC resistance; the last element on the bus may receive VCC power degraded by as much as 0.5 V.

It is recommended to use power planes to distribute power. Used on multi-layer PCBs, power planes consist of two or more metal layers that carry VCC and ground to the devices. Because the power plane covers the full area of the PCB, its DC resistance is very low. The power plane maintains VCC, distributes it equally to all devices, and provides very high current-sink capability, noise protection, and shielding for the logic signals on the PCB. Sharing the same plane between analog and digital power supplies may be risky due to unwanted interaction of these two circuit types.

For fully digital systems without separate analog power and ground planes on the board, adding two new planes to the board may be prohibitively expensive. Instead, you can create partitioned power islands (split plane). Figure 2 shows an example board layout with phase-locked loop (PLL) power islands.

Figure 2. Board Layout for General-Purpose PLL Power Islands To reduce system noise from power distribution:

•
• Use separate power planes for the analog power supply for equal power distribution.
• Avoid trace and multiple signal layers when routing the PLL power supply.
• Place a ground plane next to the PLL power supply plane. Place analog and digital components only over their respective ground plane.
• Use ferrite beads to isolate the PLL power supply from the digital power supply.
•

• Unused I/O Pins

To allow flexibility in board design, you can specify the state of unused pins as one of the following five states in the Quartus® prime or Quartus II software: as inputs that are tri-stated, as outputs that drive ground, as outputs that drive an unspecified signal, as input tri-stated with bus-hold, or as input tri-stated with weak pull-up resistors. To improve signal integrity, set unused pins as outputs that drive ground and tie them directly to the ground plane on the board. Doing so reduces inductance by creating a shorter return path and reduces noise on the neighboring I/O. To reduce power dissipation, set clock pins to drive ground and set other unused I/O pins as inputs that are tri-stated. To make the setting that is appropriate for your design, choose one of the five allowable states for Reserve all unused pins on theUnused Pins tab in the Device & Pin Options dialog box, or apply the Reserve Pin assignment to specific pins in the Pin Planner.

When you compile your design, the software generates the pin report file (.pin) to specify how you should connect the device pins. Unused I/O pins are marked in the report file according to the unused pins option you set in the  software. All I/O pins specified as GND* can either be connected to ground to improve the device's immunity to noise, or left unconnected. Leave all RESERVED I/O pins unconnected on your board because these I/O pins drive out unspecified signals. Tying a RESERVED I/O pin to VCC, ground, or another signal source can create contention that can damage the device output driver. You can connect RESERVED_INPUT I/O pins to a high or low signal on the board, while RESERVED_INPUT_WITH_WEAK_PULLUP and RESERVED_INPUT_WITH_BUS_HOLD pins can be left unconnected.

•

• Signal Trace Routing

Proper routing helps to maintain signal integrity. To route a clean trace, you should perform simulation with good signal integrity (SI) tools. The following section describes the two different types of signal traces available for routing:

•
• Single-ended trace
• Differential pair trace
• Single Ended Trace Routing

A single-ended trace connects the source and the load/receiver. Single-ended traces are used in general point-to-point routing, clock routing, low-speed, and non-critical I/O routing. This section discusses different routing schemes for clock signals. You can use the following types of routing to drive multiple devices with the same clock.

Use the following guidelines to improve the clock transmission line's signal integrity:

•
• Daisy chain routing
• With stub
• Without stub
• Star routing
• Serpentine routing
• Keep clock traces as straight as possible. Use arc-shaped traces instead of right-angle bends.
• Do not use multiple signal layers for clock signals.
• Do not use vias in clock transmission lines. Vias can cause impedance change and reflection.
• Place a ground plane next to the outer layer to minimize noise. If you use an inner layer to route the clock trace, sandwich the layer between reference planes.
• Terminate clock signals to minimize reflection.
• Use point-to-point clock traces as much as possible.
• Daisy Chain
• With Stub

Daisy chain routing is a common practice in designing PCBs. One disadvantage of daisy chain routing is that stubs, or short traces, are usually necessary to connect devices to the main bus (see Figure 14). If a stub is too long, it induces transmission line reflections and degrade signal quality. Therefore, the stub length should not exceed the following conditions:

TDstub < ( T10% to 90% )/3

Where TDstub = Electrical delay of the stub
T10% to 90% = Rise or fall time of signal edge

For a 1-ns rise-time edge, the stub length should be less than 0.5 inches. If your design uses multiple devices, all stub lengths should be equal to minimize clock skew. Figure 1 shows stub routing. If possible, you should avoid using stubs in your PCB design. For high-speed designs, even very short stubs can create signal integrity problems.

Figure 1. Daisy Chain Routing with Stubs Figures 2 through 4 show the SPICE simulation with different stub length. As the stub length decreases, there is less reflection noise, and the eye opening increases due to less reflection noise.

Figure 2. Stub Length = 0.5 Inch Figure 3. Stub Length = 0.25 Inches Figure 4. Stub Length = Zero Inches •

• Without Stub

Figure 5 shows daisy chain routing with the main bus running through the device pins, eliminating stubs. This layout removes the risk of impedance mismatch between the main bus and the stubs, minimizing signal integrity problems.

Figure 5. Daisy Chain Routing without Stubs •

•

• Star Routing

In star routing, the clock signal travels to all the devices at the same time (see Figure 6). Therefore, all trace lengths between the clock source and devices must be matched to minimize the clock skew. Each load should be identical to minimize signal integrity problems. In star routing, you must match the impedance of the main bus with the impedance of the long trace that connects to multiple devices.

Figure 6. Star Routing •

• Serpentine Routing

When a design requires equal-length traces between the source and multiple loads, you can bend some traces to match trace lengths (see Figure 7). Improper trace bends affects signal integrity and propagation delay. To minimize crosstalk, ensure that S ≥ 3 x H, where S is the spacing between the parallel sections and H is the height of the signal trace above the reference ground plane.

Figure 7. Serpentine Routing It is recommended to avoid serpentine routing if possible. Instead, use arcs to create equal-length traces.

•

•

• Differential Trace Routing

To maximize signal integrity, proper routing techniques for differential signals are important for high-speed designs. Figure 8 shows a differential pair using the microstrip layout.

Figure 8. Differential Trace Routing Note:

Use the following guidelines when using two differential pairs:

•
1. D = Distance between two differential pair signals; W = Width of a trace in a differential pair; S = Distance between the trace in a differential pair; and H = Dielectric height above the group plane.
• Make sure D > 2S to minimize the crosstalk between the two differential pairs.
• To minimize reflection noise, place the differential traces S = 3H as they leave the device.
• Keep the distance between the differential traces (S) constant over the entire trace length.
• Keep the length of the two differential traces the same to minimize the skew and phase difference.
• Avoid using multiple vias, because they can cause impedance mismatch and inductance.
•

•

• Skew Minimization

To minimize skew, make sure the two traces of a differential pair are equal lengths. If there is skew between pair traces and if the traces are loosely coupled, the traces can be designed as shown in Figure 1.To control the trace length, the traces separate and come back together. Because the traces are loosely coupled, the impedance is just slightly affected.

Figure 1. 45° Turns on the Serpentine Traces When using serpentine traces, you should have 45° bends (see Figure 1). Figure 2 shows another example using serpentine traces. However, when using the design shown in Figure 2, make sure there is no coupling between the adjacent lines. When using serpentine traces for high-speed applications, you should avoid having the traces run parallel to each other at any point. See the example shown in Figure 1.

Figure 2. Example of Serpentine Traces Figure 3 shows skew control for tightly coupled pairs. Because the traces are tightly coupled, the impedance changes when the traces are separated and then brought closer together. In a tightly coupled pair, skew-matching is performed at the pin level.

Figure 3. Skew Control Tightly-Coupled Differential Pairs When designing traces on adjacent signal layers, the traces should not cross each other unless they are almost perpendicular. Parallel traces on adjacent signal layers will have coupling between the traces.

•

• Termination Schemes

Mismatched impedance causes signals to reflect back and forth along the lines, which causes ringing at the load receiver. The ringing reduces the dynamic range of the receiver and can cause false triggering. To eliminate reflections, the impedance of the source (ZS) must equal the impedance of the trace (Z0), as well as the impedance of the load (ZL). Stratix devices feature support for on-chip implementation of a termination resistor. This section discusses the following signal termination schemes:

•
• Simple parallel termination
• Thevenin parallel termination
• Active parallel termination
• Series-RC parallel termination
• Series termination
• Differential pair termination
• On-chip termination
• Simple Parallel Termination

In a simple parallel termination scheme, the terminating resistor (RT) is equal to the line impedance. Place the termination resistor as close to the load as possible to be efficient. See Figure 1.

Figure 1. Simple Parallel Termination The stub length from RT to the receiver pin and pads should be as small as possible. A long stub length causes reflections from the receiver pads, resulting in signal degradation. If your design requires a long termination line between the terminator and receiver, the placement of the resistor becomes important. For long termination line lengths, use fly-by termination (see Figure 2).

Figure 2. Simple Parallel Fly-By Termination •

• Thevenin Parallel Termination

An alternative parallel termination scheme uses a Thevenin voltage divider (see Figure 3). The terminating resistor is split between R1 and R2, which equals the line impedance when combined. Although this scheme reduces the current drawn from the source device, it adds current drawn from the power supply because the resistors are tied between VCC and GND.

Figure 3. Thevenin Termination Stub length is dependent on signal rise and fall time and should be kept to a minimum. If your design requires a long termination line between the terminator and receiver, use fly-by termination or Thevenin fly-by termination. See Figures 3 and 4.

Figure 4. Thevenin Fly-By Termination •

• Active Parallel Termination

Figure 5 shows an active parallel termination scheme, where the terminating resistor (RT = Z0) is tied to a bias voltage (VBIAS). In this scheme, the voltage is selected so that the output drivers can draw current from the high- and low-level signals. However, this scheme requires a separate voltage source that can sink and source currents to match the output transfer rates.

Figure 5. Active Parallel Termination Figure 6 shows the active parallel fly-by termination scheme.

Figure 6. Active Parallel Fly-By Termination •

• Series-RC Parallel Termination

A series-RC parallel termination scheme uses a resistor and capacitor (i.e., series-RC) network as the terminating impedance. The terminating resistor (RT) is equal to Z0. The capacitor must be large enough to filter the constant flow of DC current. However, if the capacitor is too large, it will delay the signal beyond the design threshold.

Capacitors smaller than 100 pF diminish the effectiveness of termination. The capacitor blocks low-frequency signals while passing high-frequency signals. Therefore, the DC loading effect of RT does not have an impact on the driver, as there is no DC path to ground. The series-RC termination scheme requires balanced DC signaling (i.e., the signals spend half the time on and half the time off). AC termination is typically used if there is more than one load. See Figure 7.

Figure 7. Series-RC Parallel Termination Figure 8 shows series-RC parallel fly-by termination.

Figure 8 Series-RC Parallel Fly-By Termination •

• Series Termination

In a series termination scheme, the resistor matches the impedance at the signal source instead of matching the impedance at each load (see Figure 9). The sum of RT and the impedance of the output driver should be equal to the Z0. Because Altera device output impedance is low, you should add a series resistor to match the signal source to the line impedance. The advantage of series termination is that it consumes little power. However, the disadvantage is that the rise time degrades due to the increased RC time constant. Therefore, for high-speed designs, you should perform the pre-layout signal integrity simulation with Altera input/output buffer information specification (IBIS) models before using the series termination scheme.

Figure 9. Series Termination •

• Differential Pair Termination

Differential signal I/O standards require a termination resistor between the signals at the receiving device (see Figure 10). For the LVDS and LVPECL standard, the termination resistor should match the differential load impedance of the bus (i.e., typically 100 Ω). Intel® Stratix® family of devices, and Mercury™ devices have an on-chip termination option. Using on-chip termination decreases required board space.

Figure 10. Differential Pair (LVDS and LVPECL) Termination Figure 11 shows the differential pair fly-by termination scheme for the LVDS and LVPECL standard.

Figure 11. Differential Pair (LVDS and LVPECL) Fly-By Termination 3.3-V PCML uses two parallel 100-Ω termination resistors at the transmitter and two parallel 50-Ω termination resistors at the receiver (see Figure 12). The termination voltage (VT) is the same as the VCCIO voltage (3.3 V).

Figure 12. Differential Pair (3.3 V PCML) Termination Figure 13 shows the differential pair, fly-by termination scheme for 3.3-V PCML.

Figure 13. Differential Pair (3.3 V PCML) Fly-By Termination •

• On-Chip Termination

Stratix family of devices has on-chip resistors designed to support termination for several I/O standards. On-chip resistors simplify the task of board design by freeing board space and offering more freedom in signal routing. Also, using the on-chip resistors reduces stub reflection. Consequently, Stratix series devices provides better load and/or source termination, which leads to better signal integrity.

All transceivers in Stratix series devices have programmable, per channel internal termination resistors, which can be programmed to be either 50-, 60-, or 75-Ω single-ended resistors. In differential mode, the resistors generate 100-, 120-, or 150-Ω termination. Figures 14 and 15 show receiver and transmitter on-chip termination schemes. Because different I/O standards require different termination resistors, programmable internal termination resistors can be helpful. For example, XAUI and Infiniband applications require 100-Ω differential termination, while Gigabit Ethernet and Fibre Channel require 150-Ω differential termination. You can bypass the on-chip resistors used in the receiver and use external resistors.

Figure 15. Transmit On-Chip Termination •

• Termination Design Example

When designing a circuit board, one challenge is determining the type of termination to use and where to place it. This section helps you determine the type of termination needed and the best possible location for your custom board design.

If transmission lines associated with data or clock circuitry are not terminated properly, the signal experiences reflections. In this example, the design has the following features:

In this design example, you need to determine if the transmission line should be terminated, and if so, how it should be accomplished.

Determine the Delay

Use the following equations to determine the delay for a 300-ps rise-time signal traveling through a transmission line embedded in a dielectric with an electrical permittivity of εr.

For stripline configuration:

For microstrip configuration:

In FR-4, a transmission line with a stripline configuration induces approximately 180 ps per inch of delay on the signal. Therefore, the velocity of the signal through the transmission line becomes the inverse of the delay, which is 5.5*10-9 inches per second.

Determine the Bandwidth

Figure 16 shows that the voltage at any instant t is:

Figure 16. Characteristic Voltage Plot for Charging of an AC Circuit At 10 percent of the curve we will have:

At 90 percent of the curve we will have:

The 10 percent equation divided by the 90 percent equation gives:

Where:

The time constant variable is related to the 3-dB frequency by the equation:

From the previous equation, we can determine the equation for the time constant, r.

Plug the time constant into the voltage equation to get:

Use the following equation to determine the bandwidth for sinusoidal signal

The highest frequency component for a signal with a rise time of Tr will have a frequency given by this equation.

The signal previously discussed had a rise time of 300 ps, which means that the highest frequency component present in the signal will be:

Using the equation

with the bandwidth and speed numbers, we can determine that:

If the transmission line is longer than wavelength/10, then termination is required. In this design example, the transmission line is two inches long, so termination is required.

Using Series Termination

When using series termination, only near-end termination can be applied. Series termination should only be used with clock signals. With the near-end series termination (Z0) and the transmission line following, the circuit looks like a voltage divider circuit to the driver, reducing the amplitude V at the driver to V/2 after the series termination. Because there is no termination at the end of the transmission line, when the signal reaches the end, the entire signal reflects being restored to V.

The reflection coefficient is calculated using the following equation:

Using Parallel Termination

You can place parallel terminations on either ends or only the far end of the transmission line. You should place terminations as close to the source or destination as possible. Any transmission line between the termination and the end of the transmission line appears as a capacitive load to the signal. If you cannot place terminations close to the integrated circuit (IC), place them after the pin (i.e., fly-by configuration).

•
• A 300-ps rise-time signal
• Two-inch long transmission path between the source and the destination
• delay = 85√εr ps per inch
• delay = 85√(0.457εr+0.67) ps per inch
• V = VFINAL(1–e–t/RC)
• 0.1 VFINAL = VFINAL (1–e–t1/RC)
• 0.9 = e–t1/RC
• 0.9 VFINAL = VFINAL (1–e–t2/RC)
• 0.1 = e–t2/RC
• 9 = e(t2–t1)/RC
• ln 9 = (t2–t1)/RC
• 2.197 = (t2–t1)/RC
• t2–t1 = Rise time of the signal (Tr) and RC = time constant = r
• Frequency = 1/2 πr
• r = RC = 1/2 πf
• 2.197 = 2 πf Tr
• f = 0.35/Tr
• Bandwidth = 0.35/Tr
• Bandwidth = 0.35/300 ps = 1.16 GHz
• Speed = Frequency x Wavelength
• 5.5 giga inches per second = 1.16 GHz x wavelength
• wavelength = 4.74 in.
• wavelength/10 = 0.474 in.
•

•

• Time Domain Reflectometry and Discontinuities
• Time Domain Reflectometry

Time domain reflectometry (TDR) is a way to observe discontinuities on a transmission path. The time domain reflectometer sends a pulse through the transmission medium. Reflections occur when the pulse of energy reaches either the end of the transmission path or a discontinuity within the transmission path. From these reflections, the designer can determine the size and location of the discontinuity. This section provides an understanding of TDR.

Figure 1 shows a TDR voltage plot for a cable that is not connected to a PCB. The middle line is a 50-Ω cable one meter long. At point A, a pulse starts (Z0 = 50-Ω) and transmits through the cable, stopping at the end of the transmission line (i.e., Point B). Because the end of the transmission line is open, there is infinite impedance, ZLOAD = α. Therefore, the reflection coefficient at the load is determined with the equation:

The entire signal is reflected. At point B, the amplitude of the signal doubles. See Figure 1.

Figure 1. TDR Voltage Plot with Cable Not Connected to PCB If the same meter-long cable is then connected to a PCB through an SMA connector, the plot changes. See Figure 2. Because the SMA connector is more capacitive than inductive in nature, it appears as a capacitive load, shown as a dip in the TDR plot.

Figure 2. TDR Voltage Plot with Cable Connected to PCB Figure 3 shows an expanded curve for the SMA connector. Because the rise time of the pulse sent for TDR analysis is very small (around 20 ps), the TDR voltage plot shows every discontinuity on the transmission path.

The SMA is a capacitive discontinuity on the transmission path, so the signal dips on the voltage plot. The impedance of an ideal transmission line is defined by the following equation:

Therefore, when the capacitance increases, the impedance decreases. If the discontinuity is inductive, then the impedance increases, which appears as a bump in the TDR plot. You can calculate the capacitance and inductance from the curves on a TDR plot. If the plot shows a dip, as in Figure 3, then calculate the capacitance.

Figure 3. TDR Voltage Plot for the Section Around the SMA Connector on PCB The equivalent circuit approximation for a dip in the TDR plot is a capacitor to ground, as shown in Figure 4.

Figure 4. Equivalent Circuit for a Transmission Line with Capacitive Discontinuity The RC equation for this type of circuit is:

The two transmission lines behave as if they are parallel to each other.

You can determine the change in voltage (ΔV) and rise time (Tr) from the curve. Then, you can enter the values into the equation (i.e., Z0 = 50 Ω):

Use this equation to determine the RC time constant. You can also use the curve to approximate the RC time constant. Between 0 to 63 percent of the rise is RC. Once the RC is found, you can use it to determine the capacitance (discontinuity, as seen by the signal).

If the discontinuity looks more inductive in nature (i.e., the curve goes up), then the signal experiences a circuit similar to Figure 5. The transmission line is split, with an inductive discontinuity in between.

Figure 5. Equivalent Circuit for a Transmission Line with Inductive Discontinuity Use the following two equations to find inductive discontinuity (L):

To determine the inductance value, use the equation for (Z0 = 50 Ω) :

Figure 6 shows a cross section of a PCB transmission path, which illustrates many discontinuities.

Figure 6. Example TDR Voltage Plot for a Cross Section of a PCB If you experience a TDR plot similar to Figure 7, calculate the capacitive discontinuity introduced by the SMA connector by factoring in the voltage dip.

Figure 7. TDR Plot for a Section of a PCB You can determine Tr and V for the equation

from the curve as shown in Figure 8.

Figure 8. TDR Plot for the SMA In this example,

From the equation:

The examples in this section can be used when modeling discontinuity with a simulator. However, instead of using TDR to extract the parasitic for the discontinuity, you can model the discontinuity in the 2D and 3D field solvers.

•
• Reflection coefficient in this case = (α– 50)/(α + 50) = 1
• Z0 = √(L/C)
• R = Z0/2
• RC = Z0C/2
• (ΔV/250 mV) = 1 - (Tr /2RC)
• R = 2Z0
• L/R = L/2Z0
• (ΔV/250 mV) = 1 - (Tr x Z0 /L)
• (ΔV/250 mV) = 1 - (Tr /2RC)
• RC = (Tr x 250 mV)/2 (250 mV - ΔV) = 29.9 ps
• RC = Z0C/2
• If Z0 = 50 Ω, then C = 1.196 pF
•

• Discontinuities Related to a Transmission Path

Discontinuity on a transmission path degrades signals. Signals with fast rise times have higher degradation than signals with slow rise times. Thus, high-speed board designs require careful planning to avoid the problems associated with discontinuity. This section discusses inductive and capacitive discontinuities related to a transmission path.

• Inductive Discontinuity

Figure 9 illustrates a TDR voltage plot for two different SMA connectors, one side of the SMA connector is 50 Ω and the other is 58 Ω. The curve rises upwards due to the increasing inductance in the region.

The two plots in Figure 9 represent two different discontinuities due to SMA connectors. The curve with the higher peak represents a connector with higher inductive discontinuity of about 3.8 nH. The curve with a lower peak represents a connector with lower inductive discontinuity of about 2.6 nH. You can calculate the inductance for the discontinuity for both these curves from the graph.

Figure 9. Impedance Curves for SMA Connectors Figure 9 shows a 3.125-Gbps signal transmitted through the two SMA connectors. The rise time of the signal is approximately 70 ps.

Figure 10 shows the eye opening plot when a signal passes through the lower-inductance (2.6 nH of discontinuity) SMA connector. The eye opening is 336 mV, and the jitter is 20 ps.

Figure 10. Lower-Inductance SMA Connector Eye Opening and Expanded View of the Eye Opening An expanded view of the eye (Figure 10) provides a better jitter reading; the peak-to-peak jitter value is approximately 20 ps.

Figure 11 shows an eye opening plot of the same signal; however, this time the signal goes through 3.8 nH of inductive discontinuity due to the higher-inductance SMA connector. The eye opening is approximately 332 mV. When comparing the plots, the plot in Figure 11 has more jitter than Figure 10.

An expanded view of the eye (Figure 11) provides a better jitter reading; the peak-to-peak jitter value is approximately 24 ps.

Figure 11. Higher-Inductance SMA Connector Eye Opening and Expanded View of the Eye Opening Jitter increases and the eye opening gets smaller when the wrong type of connectors are used or other forms of inductive discontinuities are added to the transmission path. Increasing jitter behavior becomes a significant problem with signals with faster rise times. Also, when the signals become more stressed (i.e., random), jitter is more pronounced.

•

• Capacitive Discontinuity

This section discusses the effects of capacitive discontinuity, which usually occurs when components are introduced on the transmission path.

The two connector plots in Figure 12 show capacitive loads, one acting as a lower capacitive discontinuity and the other as higher capacitive discontinuity. The capacitance (C) for the load can be calculated with the equation:

A 3.125-Gbps signal (a pseudo random binary sequence (PRBS) pattern) is sent through the first connector that looks like a lower-capacitive connector (1.2 pF); the eye opening and jitter are observed on the other end.

Figure 12. Lower- and Higher-Capacitive Load Connectors Illustrating the Effects of Capacitive Discontinuity Figure 13 shows the eye opening with the connector that induces a discontinuity of 1.2 pF. The eye opening is a 330-mV differential. The expanded view of the eye shows the peak-to-peak jitter as approximately 27 ps.

Figure 13. Lower-Capacitance Connector Eye Opening and Expanded View of the Eye Opening Figure 13 shows a 3.125-Gbps PRBS pattern sent through the second connector that looks like a higher-capacitive connector; the eye opening and jitter are observed on the other end.

Figure 14 shows the eye opening for the same signal passing through an SMA connector with a capacitance of 2.9 pF. The eye opening is approximately 280 mV, differential. The expanded view of the eye opening shows that the peak-to-peak jitter is 43 ps.

Figure 14. Higher-Capacitance Connector Eye Opening and Expanded View of the Eye Opening You should avoid adding connectors and components on the transmission path whenever possible. However, if connectors are required, select ones that creates the least amount of inductive and/or capacitive discontinuity on the transmission path. The jitter and amplitude impact on a 3.125-Gbps signal when transmitting through a 2.9 and 1.2 pF capacitor is very significant. The eye opening shows an amplitude difference of 50 mV, and the expanded view shows a peak-to-peak jitter difference of 16 ps.

•
• ρ = RC = (Z0C/2)
•

• Via Discontinuity

Avoid vias and layer changes as much as possible when routing a trace because vias slow down edges and cause reflections. Vias are both inductive and capacitive in nature; however, they are dominantly capacitive. A design that uses differential signals requires vias. However, to ensure that the true and complement signals experience the same discontinuity, vias must be in the same configuration for each signal of the differential pair. Thus, any variation in signal due to the via-induced discontinuity will be in a common mode. A differential mode discontinuity will cause a reduction in the dynamic range.

Blind vias are more expensive, smaller, and act less as a discontinuity than full-sized vias. Blind vias do not go through the PCB and are designed to reduce discontinuity from vias. For better performance when using full-sized vias, use vias in series with the transmission line. The via section that is left hanging behaves like a capacitive stub.

Figure 15 shows an 18-layer board. Layers 1, 3, and 16 are signal layers. Route a trace from layer 1 down to layer 16, rather than routing through layer 3. If you route a trace that stops at layer 3, then the part of the via left hanging behaves like a capacitive stub.

Figure 15. Eighteen-Layer Board with Trace Stub The capacitive stub effects on a via become more pronounced when the board design involves:

A board thickness of 93 mils — with capacitive stubs — has less impact on a 3.125-Gbps signal as would a 200 mils-thick board running at the same frequency. Thus, vias affect signal integrity (at 3.125 Gbps) for boards that are too thick.

When possible, avoid vias and via stubs, and remove any unnecessary pads on vias because the pads create parallel plate capacitance between each other. When designing a 100-mils-thick board, you do not need to back drill the vias for a 3.125-Gbps signal. However, back drilling may be advisable for boards measurably thicker than 100 mils.

A current flow on a transmission line creates a magnetic field. The flux lines induce a return current on the reference structure. When a transmission line has its broadside facing reference planes, most of the return current travels underneath the transmission line at a skin depth on the reference plane. The value of skin depth can be calculated with the following equation:

Where:

You can calculate the current density at any point x in the reference plane with the following equation:

Where:

You should provide a good path for return currents. Figure 16 shows a layer change (from layer 1 to 13) for a pair of differential signals (i.e., red and green structures). The signal starts at point A (in Figure 16) and transmits to point B (Figure 18).

Figures 16 through 18 show that solid reference planes (i.e., light blue structures) are provided for the signal lines.

Create GND islands when necessary. When creating islands of GND, ensure that other signals referencing the plane do not pass over the split. If a signal does pass over the split, its loop will increase, also increasing the inductance in the region.

Figure 16. Layer Changes At the point of the layer change, GND vias should be provided for the return current paths. If the return path does not have GND vias, the return currents look for the closest path, but these paths may not be close enough. In this scenario, the current takes a longer path, increasing its loop. Because of the number of flux lines going through the loop, increasing the loop also increases the inductance. Although Figure 16 only shows two vias, it is better to have more vias circling the signal vias.

Figure 17 is a side view of the layer change view in Figure 16. The signals transmit from layer 1 to the layer 13. Each layer has via pads. Because there is parallel plate capacitance between the pads, the unnecessary pads add capacitive loading. Therefore, remove all of the pads except the ones that directly connect the via to the transmission lines.

Figure 17. Side View of Layer Changes In Figure 18, a GND island is provided to give a good reference path for the signal. GND vias (i.e., the light blue structures) are brought up to avoid too much discontinuity.

The PCB in Figure 18 does not have enough GND vias, so you should add more around the signal vias, evenly distributed for the two signal lines. In Figure 18, only one side of the differential pair has a GND via close to it.

Figure 18. Transmission Path to Point B Figure 19 shows a TDR plot that contains an example via from the Stratix® GX development board, a 93-mils thick board. The via looks like a capacitive discontinuity of 0.7 pF. The via connects two transmission lines that are on layer 1 and layer 13 of an 18-layer board.

Figure 19. Capacitive Discontinuity Due to a Via on a 93-mil Thick Board •
• Higher signal speeds
• Thicker boards
• skin depth = 1/√(πƒµoµrσ)
• ƒ = frequency
• µo = magnetic permeability of air
• µr = relative magnetic permeability
• σ = conductivity of the material
• Ix = Ioe -x/do
• Ix = current density at x
• Io = current density on skin depth
• x = distance from surface
• do = skin depth
•

• Right-Angle Bends Related to a Transmission Path

To minimize impedance discontinuities on the transmission line, avoid using right-angle bends. At the bend, the effective transmission line width increases, this result in an impedance discontinuity, increasing the capacitance.

Instead of 90° bends, use mitered 45° bends. Mitered 45° bends reduce reflection on the signal by minimizing impedance discontinuities. Right-angled bends also look like antennas. Figure 20 shows a 60-mils transmission line immersed in FR-4 dielectric (εr = 4.1, loss tangent = 0.022) with dimensions for 50-Ω impedance. The 90° and 45° bend (see Figure 21) traces are simulated using SPICE models. The parasitics are extracted with a 3D field solver.

Figure 20. 90° Bend on a Transmission Line Figure 21. 45° Bend on a Transmission Line Figure 22 shows the board’s cross section.

Figure 22. Board’s Cross Section A 1-ns (rise time) signal is fed to one side of the trace and the output is observed at the other end. Because of the extra capacitive loading, the output of the 90° bend has a slight delay and more ringing on it. When driving through long traces or other stressful conditions, even a little bit of ringing is destructive. For instance, adding more closure to an almost closed eye can result in the receiver failing to recognize some bits of data. The 90° bend will affect signals running at 3.125 Gbps even more severely. Figure 23 shows the effects of bends on signals.

Figure 23. Effects of Bends on Signals •

•

•

• Ground Bounce

As digital devices become faster, their output switching times decrease. Faster switching times cause higher transient currents in outputs as they discharge load capacitances. These higher currents, which are generated when multiple outputs of a device switch simultaneously from a logic high to a logic low, can cause a board-level phenomenon known as ground bounce.

Many factors contribute to ground bounce. Therefore, no standard test method predicts ground bounce magnitude for all possible PCB environments. Determine each condition's and each device's relative contributions to ground bounce by testing the device under these conditions: Load capacitance, socket inductance, and the number of switching outputs, which are the predominant conditions that influence the magnitude of ground bounce in programmable logic devices (PLDs).

Design Guidelines

It is recommended to follow the below design methods to reduce ground bounce:

Figure 1. Suggested Via Location that Connects to Capacitor Pad These design guidelines provide information and help for high-speed logic designs operating over a range of PCB conditions.

•
• Add decoupling capacitors for as many VCC/GND pairs as possible.
• Place the decoupling capacitors as close as possible to the power and ground pins of the device.
• Add external buffers at the output of a counter to minimize the loading on Intel® device pins.
• Configure the unused I/O pin as an output pin and then drive the output low. This configuration acts as a virtual ground. Connect this low driving output pin to GNDINT and/or the board's ground plane.
• Any unused I/O pin may be driven to ground by programming the “programmable ground” bit (one per I/O cell). In doing so, the macrocell does not need to be sacrificed, but can be used as a buried macrocell.
• When speed is not critical, turn on the slow slew rate logic option.
• Limit load capacitance by buffering loads with an external device, or by reducing the number of devices that drive the bus.
• Eliminate sockets whenever possible.
• Reduce the number of outputs that can switch simultaneously and/or distribute them evenly throughout the device.
• Move switching outputs close to a package ground pin.
• Create a programmable ground next to switching pins.
• Eliminate pull-up resistors or use pull-down resistors.
• Use multi-layer PCBs that provide separate VCC and ground planes.
• Add appropriate resistors in series to each of the switching outputs to limit the current flow into each of the outputs.
• Create synchronous designs that are not affected by momentarily switching pins.
• Assign I/O pins to minimize local bunching of output pins.
• Place the power and ground pins next to each other. The total inductance is reduced by mutual inductance, because current flows in opposite directions in power and ground pins.
• Use a bigger via size to connect the capacitor pad to the power and ground plane to minimize the inductance in decoupling capacitors.
• Use the wide and short trace between the via and the capacitor pad or place the via adjacent to the capacitor pad. See Figure 1.
• Use surface mount capacitors to minimize the lead inductance.
• Use low effective series resistance (ESR) capacitors. The ESR should be < 400 mÎ©.
• Each GND pin/via should be connected to the ground plane individually.
• To add extra capacitance on the board, Intel recommends placing a ground plane next to each power (VCC) plane. This placement gives zero lead inductance and no ESR. The dielectric thickness between the two planes should be ~5 mils.
• Analyzing Ground Bounce

Figure 2 shows a simple model for analyzing ground bounce. The external components driven by the device appear as capacitance loads to that device (C1 to Cn). These capacitive loads store a charge determined by the following equation:

Thus, the charge increases as the voltage and/or load capacitance increases.

Figure 2. Ground Bounce Model A device's environment and ground path have intrinsic inductances (shown in Figure 2 as L1, L2, and L3). L1 is the inductance of the bond wire from the device's die to its package pin, and of the pin itself. L2 is the inductance of the connection mechanism between the device's ground pin and the PCB. This inductance is greatest when the device is connected to the PCB through a socket. L3 is the inductance of the PCB trace between the device and the PCB location where the power supply's reference ground is connected.

Ground bounce occurs when multiple outputs switch from high to low. The transition causes the charge stored in the load capacitances to flow into the device. The sudden rush of current (di/dt) exits the device through the inductances (L) to board ground, generating a voltage (V) determined by the equation V = L × (di/dt). This voltage difference between board ground and device ground causes the relative ground level for low or quiet outputs to temporarily rise or bounce. Although the rush of current is brief, the magnitude of the bounce can be large enough to trigger other devices on the PCB.

In synchronous designs, ground bounce is less often a problem because synchronous outputs have enough time to settle before the next clock edge. Also, synchronous circuits are not as likely to be falsely triggered by a voltage spike on a quiet output.

Capacitive loading on the switching outputs and quiet outputs affect ground bounce differently.

•
• Charge (Q) = [voltage (V) × capacitance (C)]
•

• Switching Outputs

When the capacitive loading on the switching outputs increases, the amount of charge available for instantaneous switching increases, which in turn increases the magnitude of ground bounce. Depending on the device, ground bounce increases with capacitive loading until the loading is approximately 100 pF per device output. At this point, the device output buffers reach their maximum current-carrying capacity and inductive factors become dominant.

One method of reducing the capacitive load and, consequently, ground bounce is to connect the device's switching outputs to a bus driver integrated circuit (IC). The outputs of this IC drive the heavy capacitive loads, reducing the loading on the device and minimizing ground bounce for the device's quiet outputs.

Some bus applications use pull-up resistors to create a default high value for the bus. These resistors cause the load capacitances to charge up to the maximum voltage. Consequently, the driving device produces a higher level of ground bounce. Eliminate pull-up resistors in applications in which ground bounce is a concern, or design bus logic that uses pull-down resistors instead.

The number of switching outputs also affects ground bounce. As the number of switching outputs increases, the total charge stored also increases. The total charge is equal to the sum of the stored charges for each switching output. Therefore, the amount of current that must sink to ground increases as the number of switching outputs increases. Ground bounce can increase by as much as 40 to 50 mV for each additional output that is switching.

To counteract these effects, Intel devices provide multiple VCC and GND pin pairs. Reduce ground bounce by moving switching outputs close to a ground pin and distributing simultaneously switching outputs throughout the device.

Besides placing switching pins next to a ground pin, create a programmable ground pin by creating an output pin in the design that drives only ground. By connecting this output pin to ground on the board, the device ground has another connection to the board ground, which helps reduce ground bounce.

Many Intel FPGA devices have slew rate options for the output drivers. Turning on the slow slew rate option for all or most of the drivers slows down the drivers, decreasing di/dt and reducing ground bounce.

To further reduce ground bounce, limit the number of outputs that can switch simultaneously in the design. For functions such as counters, use Gray coding as an alternative to standard sequential binary coding, because only one bit switches at a time.

In extreme cases, adding resistors in series to each of the switching outputs in a high-speed logic device can limit the current flow into each of the outputs and, thus, reduce ground bounce to an acceptable level.

•

• Quiet Outputs

An increase in capacitive loading on quiet outputs acts as a low-pass filter and tends to dampen ground bounce. Capacitive loading on a quiet output can reduce ground bounce by as much as 200 to 300 mV. However, an increase in capacitive loading on a quiet output can increase the noise seen on other quiet outputs when the capacitive-loaded pin does switch.

•

Using multi-layer PCBs that provide separate VCC and ground planes can also reduce the ground bounce caused by PCB trace inductance. Wirewrapping the VCC and ground supplies usually increases the amount of ground bounce. To reduce unwanted inductance, use low-inductance bypass capacitors between the VCC supply pins and the board ground plane, as close to the package supply pins as possible. It is required to use low ESR decoupling surface mount capacitors of 0.01 μF to 0.1 μF in parallel to reduce ground bounce. Adding a 0.001 μF capacitor in parallel to these capacitors filters high frequency noise (>100 MHz).

For more information see the Minimizing Ground Bounce & VCC Sag white paper (PDF).

•

•

• Understanding Transmission Lines

The transmission line is a trace and has a distributed mixture of resistance (R), inductance (L), and capacitance (C). There are two types of transmission line layouts:

Figure 1 shows a microstrip layout, which refers to a trace routed as the top or bottom layer of a PCB and has only one voltage-reference plane (i.e., power or GND). Figure 2 shows a stripline layout, which uses a trace routed on the inside layer of a PCB and has two voltage-reference planes (i.e., power and/or GND).

Figure 1. Microstrip Transmission Line Layout Figure 2. Stripline Transmission Line Layout Notes to Figures 1 and 2:

•
• Microstrip
• Stripline
• W = width of trace, T = thickness of trace, and H = height between trace and reference plane.
• W = width of trace, T = thickness of trace, and H = height between trace and two reference planes.
• Impedance Calculation

Any circuit trace on the PCB has characteristic impedance associated with it. This impedance is dependent on the width (W) of the trace, thickness (T) of the trace, dielectric constant (εr) of the material used, and height (H) between the trace and reference plane.

• Microstrip Impedance

A circuit trace routed on an outside layer of the PCB with a reference plane (i.e., GND or VCC) below it constitutes a microstrip layout. Use the following equation to calculate the impedance of a microstrip trace layout.

Using typical values of W = 8 mil, H = 5 mil, T = 1.4 mil, εr and (FR-4) = 4.1 and solving for microstrip impedance (Z0) yields:

The measurement unit in the equation is mils (i.e., 1 mil = .001 inches). Also, copper (Cu) trace thickness (T) is usually measured in ounces (i.e., 1 oz = 1.4 mil).

Figure 3 shows microstrip trace impedance versus trace width (W) using the values in the equation, keeping dielectric height and trace thickness constant.

Figure 3. Microstrip Trace Impedance with Changing Trace Width Figure 4 shows microstrip trace impedance versus height (H), using the values in the microstrip trace impedance equation, keeping trace width and trace thickness constant.

Figure 4. Microstrip Trace Impedance with Changing Height The impedance graphs show that the change in impedance is inversely proportional to trace width and directly proportional to trace height above the ground plane.

Figure 5 plots microstrip trace impedance versus trace thickness (T) using the values in the microstrip trace impedance equation, keeping trace width and dielectric height constant. Figure 5 shows that as trace thickness increases, trace impedance decreases.

Figure 5. Microstrip Trace Impedance with Changing Trace Thickness •
• Z0 = [(87/√(εr + 1.41)) ln [(5.98 ×H)/(0.8W + T)] Ω
• Z0 = [(87/√(4.1+1.41)) ln (5.98×(5)/0.8(.8)=1.4)] Ω
• Z0 ~ 50 Ω
•

• Stripline Impedance

A circuit trace routed on the inside layer of the PCB with two low-voltage reference planes (i.e., power and/or GND) constitutes a stripline layout. Use the following equation to calculate the impedance of a stripline trace layout.

Equation 2:

Using typical values of W= 9 mil, H= 24 mil, T = 1.4 mil, εr and (FR-4) = 4.1 and solving for stripline impedance (Zo) yields:

Figure 6 shows impedance versus trace width using the stripline trace impedance equation, keeping height and thickness constant for stripline trace.

Figure 6. Stripline Trace Impedance with Changing Trace Width Figure 7 shows stripline trace impedance versus dielectric height (H) using the stripline trace impedance equation, keeping trace width and trace thickness constant.

Figure 7. Stripline Trace Impedance with Changing Dielectric Height As with microstrip layout, the stripline layout impedance also changes inversely proportional to line width and directly proportional to height. However, the rate of change with trace height above GND is much slower in a stripline layout compared to a microstrip layout. A stripline layout has a signal sandwiched by FR-4 material, whereas a microstrip layout has one conductor open to air. This exposure causes a higher, effective dielectric constant stripline layout compared to microstrip layouts. Thus, to achieve the same impedance, the dielectric span must be greater in stripline layouts than in microstrip layouts. Therefore, stripline layout PCBs with controlled impedance lines are thicker than microstrip layout PCBs.

Figure 8 shows stripline trace impedance versus trace thickness using Equation 2, keeping trace width and dielectric height constant. Figure 8 shows that the characteristic impedance decreases as the trace thickness increases.

Figure 8. Stripline Trace Impedance with Changing Trace Thickness •
• Z0 = [(60/√εr) ln (4H/0.67π(T+0.8w))] Ω
• Z0 = [(60/√(4.1)) ln (4(24)/0.67π(1.4)=0.8(9))] Ω
• Z0 ~50 Ω
•

•

• Propagation Delay

Propagation delay (tPD) is the time required for a signal to travel from one point to another. Transmission line propagation delay is a function of the dielectric constant of the material.

• Microstrip Layout Propagation Delay

Use the following equation to calculate the microstrip trace layout propagation delay.

•
• tPD(microstrip) = 85 √(0.475εr +0.67) ps per inch
•

• Stripline Layout Propagation Delay

Use the following equation to calculate the stripline trace layout propagation delay.

Figure 9 shows the propagation delay versus the dielectric constant for microstrip and stripline traces. As the εr increases, the propagation delay (tPD) also increases.

Figure 9. Propagation Delay vs. Dielectric Constant for Microstrip and Stripline Traces •
• tPD(stripline) = 85 √εr ps per inch
•

•

•

• Coplanar Wave Guides

There are three types of coplanar wave guides: simple, grounded, and grounded differential.

• Simple Coplanar Wave Guide

The simple coplanar wave guide, shown in Figure 1, is used primarily in microwave systems. This structure does not require vias, and you can easily mount passive or active devices in the signal path, resulting in a low-loss, high-speed transmission line. The simple coplanar wave guide requires that the substrate thickness (H) be “infinite,” so that the fields remain outside the dielectric. You cannot use this structure on multilayer boards because it cannot have a second layer.

Figure 1. Simple Coplanar Wave Guide •

• Grounded Coplanar Wave Guide

The grounded differential coplanar wave guide is the differential version of the grounded coplanar wave guide and is used in high-speed digital systems that require maximum noise immunity. Figure 3 shows the topology. The same limitations for S and G apply in this topology as for the grounded coplanar wave guide.

Figure 2 Grounded Coplanar Wave Guide •

• Grounded Differential Coplanar Wave Guide

The grounded differential coplanar wave guide is the differential version of the grounded coplanar wave guide and is used in high-speed digital systems that require maximum noise immunity. Figure 3 shows the topology. The same limitations for S and G apply in this topology as for the grounded coplanar wave guide.

Figure 3. Grounded Differential Coplanar Wave Guide •

•

• Simultaneous Switching Noise Guidelines

Simultaneous switching noise (SSN) is another important factor to consider when designing a PCB. Although SSN is dominant on the device package, the board layout can help reduce some of the noise.

Every current loop has an inductance value. The current loop in Figure 1 has the following inductance:

Figure 1. Inductance Due to a Current Loop When a driver switches from high to low, a voltage develops in the GND plane, thus:

The noise that develops in the GND plane can become a problem for signal-integrity, especially when there are a lot of drivers switching simultaneously. The noise generated by SSNs can couple to adjacent structures. Proper layout and decoupling reduces noise coupling. The high number of simultaneously switching drivers can cause the power supply to collapse. Thus, the power supply voltage at a certain region loses some of its strength, depending on where the switching is concentrated.

•
• Lloop = L1 (signal) + L2 (GND) – 2 LM (mutual inductance)
• V = Lloop (di/dt)
•

• Design Security Features in FPGAs
•

• EMI

Electromagnetic interference (EMI) is directly proportional to the change in current or voltage with respect to time. EMI is also directly proportional to the series inductance of the circuit. Every PCB generates EMI.

Precautions such as minimizing crosstalk, proper grounding, and proper layer stack-up can significantly reduce EMI problems.

Place each signal layer in between the ground plane and power plane. Inductance is directly proportional to the distance an electric charge has to cover from the source of an electric charge to ground. As the distance gets shorter, the inductance becomes smaller as well. Therefore, placing ground planes close to a signal source reduces inductance and helps contain EMI. Figure 1 shows an example of an eight-layer stack-up. In the stack-up, the stripline signal layers are the quietest because they are centered by power and GND planes. A solid ground plane next to the power plane creates distribution capacitances with low equivalent series inductance (ESL). With IC edge rates becoming faster, these techniques help to contain EMI.

Figure 1. Example Eight-Layer Stack-Up Component selection and proper placement on the board is very important to controlling EMI. The following guidelines can help reduce EMI:

•
• Select low-inductance components, such as surface mount capacitors with low ESR and ESL
• Provide good return path to minimize lop inductance
• Use solid ground planes next to power planes
• Use adjacent ground planes next to each segmented power plane for analog and digital circuits
•

• Discrete Component Selection for High-Speed Design

Deciding which components to use is an important part of board design. Information and guidelines for selecting discrete components for the PCB is provided below.

• Resistors and Capacitors

Choose the smallest footprint available when selecting discrete components such as resistors and capacitors. The small footprint means that the pad on the board can be small and that the parasitic capacitance and inductance will also be small. Altera typically uses 40 mil × 20 mil (0402) package components for high-speed signals.

Inductors typically require bigger footprints because they are often used for power supply filtering and must be bigger to support high currents without saturating.

The three parameters of interest when choosing ferrite beads are:

•
• DC resistance
• AC impedance
• Current handling capability
•

A good ferrite bead has low DC resistance, high AC impedance, and high current handling capability. However, as the current handling capability increases, the AC impedance tends to drop, so there is a tradeoff involved. Figure 1 shows the impedance versus frequency plot of a typical ferrite bead.

Figure 1. Typical Impedence Profile of a Ferrite Bead In Figure 1, the impedance at 2 GHz is more than 100 Ω. The ratio between that impedance and the power supply impedance, which is often lower than 1 Ω, is more than 100. As a result, most of the noise is blocked by the ferrite bead and is shunted to ground instead.

Some ferrite beads that meet performance are:

•
• The Steward MI0805M221R-00 ferrite beads for transceiver power and ground planes. The DC resistance for this part is lower than 50 mΩ, and it can handle 2.5 A of current. The impedance is over 200 Ω at 1 GHz.
• Two Steward ferrite beads connected in parallel can provide 5 A of current capability with 25 mΩ of DC resistance and over 100 Ω of AC impedance. This performance level is adequate for most applications.
• The Murata BLM31PG500SN1 ferrite bead has 25 mΩ of DC resistance, 3 A of current, and 75 Ω of AC impedance at 1 GHz.
•

• SMA Connectors

SMA connectors are typically used for high-speed signals because of their controlled impedance, mechanical robustness, and good signal integrity. These connectors come in the form of edge launch or vertical launch. For edge launch, the connector is connected to the board edge, the central conductor stays flush with the board, and the board is sandwiched between the ground conductors.

The vertical launch type is through-hole or surface mount. For the through-hole type, all the legs and the center conductor go through the board. For a surface mount type, the center conductor barely touches the top layer of the board.

The type of launch technique does not affect the signal quality very much. However, a long center conductor adds inductance to the transmission path and degrades the signal.

With vertical launch surface mount, you can often strip the center conductor down to below 20 mils. This stripping might be slightly harder to achieve in edge launch configuration, but the choice is dependent on the capability of the SMA manufacturers. Altera has stripped the center conductor down to less than 20 mils short in its designs. Altera uses Lighthorse Technologies and Northrop Grumman for SMA connector requirements.

•

•

• S-Parameters

It is difficult to define voltages or currents in transmission lines and to measure them at microwave frequencies, because direct measurements usually involve the magnitude (inferred from power) and phase of a wave traveling in a given direction or the standing wave. Thus, equivalent voltages and currents, and the related impedance and admittance matrices, become somewhat of an abstraction when dealing with high-frequency networks.

A representation more consistent with direct measurements, and with the ideas of incident, reflected, and transmitted waves, is provided by the scattering matrix (S-parameters). S-parameters are often used to quantify the impedance, total losses, input return loss, insertion loss, and isolation and crosstalk for the different transmission lines structures. These concepts are most useful at those frequencies where you must consider distributed rather than lumped parameters.

To understand S-parameters, consider the two-port network shown in Figure 1. The network can contain a transmission line or any linear time invariant component. The incident voltages at ports 1 and 2 are E11 and E12; and the reflected voltages are ER1 and ER2. Z0 is the characteristic impedance of the transmission line. ZS and ZL are the source and the load impedances.

Figure 1. S-Parameters Taking the incident and reflected voltage waves on each side of the two port network and dividing them by the square root of the characteristic impedance, Z0, results in new variables (a1, a2, b1, and b2), which are the normalized voltage wave amplitudes at each port.

The square of the magnitude of a1 (| a1|2) represents the incident power in port 1, and (| b1|2) represents the reflected power from this port. The same relations apply to port 2.

The resulting parameters relate the scattered wave (reflected wave) from the network to the incidents waves. These parameters are called S-parameters and are defined by:

Where, S11 is the input reflection coefficient, S21 is the forward transmission through the network, S12 is the reverse transmission through the network, and S22 is the output reflection coefficient.

The measurement setup for S-parameters is shown in Figure 2 and Figure 3. Apply the following conditions for these measurements:

Figure 2. Measurement Setup for S11 and S21 Figure 3. Measurement Setup for S22 and S12 For example, to measure S11, ensure that a2 = 0. Do this by making sure that there is no reflection from the load (in other words, set ZL = Z0).

S-parameters are typically measured using network analyzers.

•
• a1=EI1/√Z0 a2=EI2/√Z0
• b1=ER1/√Z0 b2=EI2/√Z0
• b1=S11a1+S12a2
• b2=S21a1+S22a2
• S11=(a1/b1) | a2=0
• S21=(b2/a1) | a2=0
• S12=(b1/a2) | a1=0
• S22=(b2/a2) | a1=0
•

• Smith Chart

The Smith Chart is a graphical representation of the impedances in a complex plane. You can use this to analyze transmission line impedance matching networks and capacitive or inductive behavior of loads. Figure 1 shows a typical Smith Chart. If the impedance is inductive, it shows up in the top half of the circle; if it is capacitive, it shows up in the bottom half. The far-right point in the middle represents an open circuit; the far left represents a short circuit. The middle point (label 1.0) represents a perfect load match to the characteristic impedance of the line.

Figure 1. Smith Chart •

• AC Versus DC Coupling

AC coupling refers to the use of a series capacitor on a signal to block the DC signals from going through. DC coupling refers to the case where this capacitor is not present and the signal passes through without any interruption. In AC coupling, a DC restore circuit is generally required after the capacitor to ensure that the common mode voltage requirements of the receiver are met. In Altera® devices with transceivers, the DC restore circuitry is built into the device. In that case, external DC restore circuitry is not necessary. DC coupling works only in cases where the output common mode voltage of the transmitter is in the required range of the input common mode voltage of the receiver.

The advantage of AC coupling is that it allows chips with different common mode voltages to interface with each other. The disadvantage is that it requires an extra capacitor, which can add some jitter or other degradation if not properly selected.

If you are certain that the common mode voltage requirements of the receiver are a subset of the common mode voltage output of the transmitter, use DC coupling. If you are in a borderline case, or if the requirements are not satisfied, then use AC coupling.

In choosing the value of the coupling capacitor, consider what happens if the capacitor is too big or too small. If the capacitor is too big, it can significantly slow the signal down and can also respond poorly to fast changing input signals because of the long charge and discharge times. If the capacitor is too small, it presents a fair amount of impedance and can increase attenuation and change the characteristic impedance of the path. A good balance between these two conflicting requirements is a 0.01 μF capacitor, which Altera uses for its 3.125 Gbps transceiver designs.

When selecting components, use the smallest size possible, because smaller size components have smaller size pads, which reduce the discontinuity. Altera has used 0402 components (40 mils x 20 mils) in its designs.

You can design the DC restore circuitry in a variety of ways. Altera typically uses a simple resistive voltage divider (see Figure 1). Be sure to use precision resistors (0.1% or 1%) for differential signals, so that the restored DC levels on the positive and negative signals are very closely matched. In Figure 1, the DC restore circuitry restores the DC level to 3.3 * 78.7/(140 + 78.7) = 1.1875 volts.

Figure 1. AC Coupling Transceiver devices have DC biasing on the high-speed transceivers inputs and reference clock inputs designed for the 1.5-V PCML standard, so AC coupling is not required. This saves components and board space. If you are using other I/O standards such as LVPECL or LVDS, then you need to AC-couple them, because their common mode voltage is different from the 1.5-V PCML common mode voltage. External biasing networks are not needed, because the common mode is generated internally in the device.

•