Intel 82562 ET(EM), GT(G) LAN Application Note

82562ET(EM) and 82562GT(G) LAN
on Motherboard Design Guide
Application Note (AP-414)
Revision 2.1
April 2005
INFORMATION IN THIS DOCUMENT IS PROVIDED IN CONNECTION WITH INTEL® PRODUCTS. NO LICENSE, EXPRESS OR IMPLIED, BY
ESTOPPEL OR OTHERWISE, TO ANY INTELLECTUAL PROPERTY RIGHTS IS GRANTED BY THIS DOCUMENT. EXCEPT AS PROVIDED IN
INTEL'S TERMS AND CONDITIONS OF SALE FOR SUCH PRODUCTS, INTEL ASSUMES NO LIABILITY WHATSOEVER, AND INTEL DISCLAIMS
ANY EXPRESS OR IMPLIED WARRANTY, RELATING TO SALE AND/OR USE OF INTEL PRODUCTS INCLUDING LIABILITY OR WARRANTIES
RELATING TO FITNESS FOR A PARTICULAR PURPOSE, MERCHANTABILITY, OR INFRINGEMENT OF ANY PATENT, COPYRIGHT OR OTHER
INTELLECTUAL PROPERTY RIGHT. INTEL PRODUCTS ARE NOT INTENDED FOR USE IN MEDICAL, LIFE SAVING, OR LIFE SUSTAINING
APPLICATIONS.
Intel may make changes to specifications and product descriptions at any time, without notice.
Designers must not rely on the absence or characteristics of any features or instructions marked "reserved" or "undefined." Intel reserves these for
future definition and shall have no responsibility whatsoever for conflicts or incompatibilities arising from future changes to them.
The Intel product(s) described herein may contain design defects or errors known as errata which may cause the product to deviate from published
specifications. Current characterized errata are available on request.
Contact your local Intel sales office or your distributor to obtain the latest specifications and before placing your product order.
Copies of documents which have an ordering number and are referenced in this document, or other Intel literature may be obtained by calling 1-800548-4725 or by visiting Intel's Web site at http://www.intel.com.
Copyright © 2005 Intel Corporation
* Other product and corporate names may be trademarks of other companies and are used only for explanation and to the owners’ benefit, without
intent to infringe.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Revision History
Revision
Revision Date
1.1
Mar 2003
• Removed confidential status.
• Added product ordering code in Section 1.0.
2.0
Feb 2005
• Added 82562GT/G board design and layout information.
2.1
Apr 2005
• Removed the note “BIOS must delay driving LAN_RST# 10 ms after 3.3V
and 1.5V SUS wells are valid” from the reference schematics.
Application Note (AP-414)
Description
iii
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Note:
iv
This page is intentionally left blank.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Contents
1.0
2.0
3.0
Introduction .............................................................................................. 1
1.1
Scope .......................................................................................................................1
1.2
Terms .......................................................................................................................1
1.3
Reference Documents ............................................................................................. 2
1.4
Product Codes ......................................................................................................... 3
1.5
Usage Modes for the 82562G/GT ............................................................................ 3
1.5.1 Mode 0: Drop-in Replacement ...................................................................... 3
1.5.2 Modes 1, 2, 3, and 4: New Features ............................................................. 3
Frequency Control Device Design Considerations .............................. 5
2.1
Frequency Control Component Types ..................................................................... 5
2.2
Quartz Crystal .......................................................................................................... 5
2.3
Fixed Crystal Oscillator ............................................................................................ 5
2.4
Programmable Crystal Oscillators............................................................................ 6
2.5
Ceramic Resonator .................................................................................................. 6
Ethernet Component Design Guidelines ............................................... 7
3.1
General Design Considerations for Ethernet Controllers ......................................... 7
3.1.1 Crystal Selection Parameters........................................................................ 7
3.1.2 Reference Crystal........................................................................................11
3.1.3 Reference Crystal Selection........................................................................11
3.1.4 Circuit Board................................................................................................11
3.1.5 Temperature Changes ................................................................................12
3.2
Analog References.................................................................................................12
3.3
Integrated Magnetics Module.................................................................................13
3.4
Designing with the Platform LAN Connect Device .................................................13
3.4.1 Power Supplies ...........................................................................................13
3.4.2 Device Test Capability.................................................................................13
3.4.3 PLC Device LAN Disable Guidelines ..........................................................13
3.4.4 Serial EEPROM...........................................................................................13
3.4.5 Magnetics Modules for PLC Devices ..........................................................15
3.5
Flash Interface .......................................................................................................15
Application Note (AP-414)
v
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.0
General Layout Considerations for PLC Devices ............................... 17
4.1
Guidelines for Component Placement ................................................................... 17
4.1.1 Crystals ....................................................................................................... 18
4.1.2 Board Stackup Recommendations.............................................................. 18
4.2
Critical Dimensions for Discrete Magnetics Module and RJ-45 ............................. 19
4.2.1 Distance A: Magnetics to RJ45 (Priority 1).................................................. 19
4.2.2 Distance B: PHY to Magnetics (Priority 2)................................................... 20
4.2.3 Distance C: LAN Connect Interface Distance ............................................. 20
4.2.4 Distance D: The Overall
Length of Differential Traces from LAN to RJ-45 (Priority 4)....................... 20
4.2.5 Distance E: PLC Device to PCB Edge ........................................................ 20
4.3
Critical Dimensions for an Integrated Magnetics Module....................................... 20
4.3.1 Distance A: The Overall Length of Differential Traces ................................ 21
4.3.2 Distance B: PLC Device to Chipset............................................................. 21
4.3.3 Distance C: LAN Controller to PCB Edge ................................................... 21
4.4
Differential Pair Trace Routing ............................................................................... 21
4.4.1 Signal Trace Geometry ............................................................................... 23
4.4.2 Trace Length and Symmetry ....................................................................... 23
4.4.3 Impedance Discontinuities .......................................................................... 23
4.4.4 Reducing Circuit Inductance ....................................................................... 24
4.4.5 Signal Isolation ............................................................................................ 24
4.4.6 Power and Ground Planes .......................................................................... 24
4.4.7 Traces for Decoupling Capacitors ............................................................... 25
4.4.8 Ground Planes Under a Discrete Magnetics Module .................................. 25
4.4.9 Non-Integrated Magnetics Modules/RJ-45 Connectors) ............................. 26
4.4.10 Layout Guidelines (Routing LAN 3.3 V When Using a Copper Trace)........ 27
4.5
Signal Terminations ............................................................................................... 29
4.5.1 Termination Plane ....................................................................................... 30
4.5.2 Termination Plane Capacitance .................................................................. 30
4.6
Light Emitting Diodes ............................................................................................. 30
4.7
Physical Layer Conformance Testing .................................................................... 31
4.8
Troubleshooting Common Physical Layout Issues ................................................ 31
5.0
Pinout Information ................................................................................. 33
6.0
Self-Review Checklist for a LAN on Motherboard Design.................. 35
7.0
Reference Schematics ........................................................................... 37
A
Measuring LAN Reference
Frequency Using a Frequency Counter ............................................... 41
vi
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figures
1
2
3
4
5
6
7
8
9
10
11
12
13
14
Application Note (AP-414)
Crystal Circuit ................................................................................................ 9
RBIAS10 and RBIAS100 Circuits................................................................12
General Placement Distances.....................................................................18
Critical Dimensions for Component
Placement (Discrete Magnetics Solution) ...................................................19
Critical Dimensions for Component
Placement with Integrated Magnetics Module.............................................21
Corner Trace Routing..................................................................................22
Ground Plane Separation............................................................................25
Ideal Ground Split Implementation (for Integrated RJ-45 without USB)......26
Termination Plane Example for PLC Device and Discrete Magnetics ........27
Decoupled LAN Power Trace (Power Supplied by Trace) ..........................28
Using a Moat to Reduce Noise From Adjacent Traces and Power Fills......29
Termination Resistors Placement (Integrated Magnetics Solution) ............30
Indirect Probing Setup.................................................................................42
Direct Probing Method.................................................................................45
vii
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Tables
1
2
3
4
5
6
7
8
9
10
viii
Product Ordering Codes................................................................................ 3
New Usage Modes ........................................................................................ 4
Recommended Crystals ................................................................................ 5
Crystal Parameters........................................................................................ 7
Memory Layout (128B EEPROM) ............................................................... 14
Memory Layout (512B EEPROM) ............................................................... 14
Recommended EEPROM Manufacturers ................................................... 14
Recommended Magnetics Modules ............................................................ 15
Electrical Specifications at 25°C for 10/100 Magnetics ............................... 16
Pin Assignments.......................................................................................... 33
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
1.0
Introduction
The 82562G/GT and 82562ET/EM are highly-integrated devices designed for 10 or 100 Mbps
Ethernet systems. They are based on IEEE 10BASE-T and 100BASE-TX standards. The IEEE
802.3u standard for 100BASE-TX defines networking over two pairs of Category 5 unshielded
twisted pair cable or Type 1 shielded twisted pair cable. They are also 3.3 V devices available in a
48-pin Shrink Small Outline Package (SSOP).
The 82562G/GT and 82562ET/EM comply with the IEEE 802.3u Auto-Negotiation standard and
the IEEE 802.3x Full Duplex Flow Control standard. The 82562G/GT and 82562ET/EM also
include a PHY interface compliant to the current platform LAN connect interface.
1.1
Scope
This application note provides guidelines for system designs based on the Intel® 82562G/GT and
82562ET/EM Platform LAN Connect (PLC) devices.
The table in Section 5.0 lists the pinout assignments for each of the PLC devices. For other
necessary design collateral, please refer to “Reference Documents” (Section 1.3).
1.2
Terms
AFE
Analog Front End.
BER
Bit Error Rate.
DUT
Device Under Test.
ICHx
I/O Controller Hub (ICH) that supports the 82562G/GT (x = 5, 6, or 7).
The ICH that supports the 82562ET/EM (x = 2, 3, or 4).
LCI
LAN Connect Interface.
BGA
Ball Grid Array.
PLC
Platform LAN Connect.
USB
Universal Serial Bus
Application Note (AP-414)
1
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
1.3
Reference Documents
This application note assumes that you have a working knowledge of high-speed design and layout
issues and the Advanced Configuration and Power Interface (ACPI) Specification. An
understanding of power management industry initiatives is valuable prior to beginning the
integration of an 82562G/GT and 82562ET/EM device into any platform. The following reference
list provides sufficient background material.
•
•
•
•
•
•
•
•
82562ET 10/100 Mbps Platform LAN Connect (PLC) Datasheet. Intel Corporation.
82562EM 10/100 Mbps Platform LAN Connect (PLC) Datasheet. Intel Corporation.
82562G 10/100 Mbps Platform LAN Connect (PLC) Datasheet. Intel Corporation.
82562GT 10/100 Mbps Platform LAN Connect (PLC) Datasheet. Intel Corporation.
I/O Control Hub 2, 3 and 4 EEPROM Map and Programming Information. Intel Corporation.
I/O Control Hub 5, 6 and 7 EEPROM Map and Programming Information. Intel Corporation.
I/O Control Hub 2 (ICH2) Datasheet. Intel Corporation.
Intel Packaging Databook, 1999. Intel Corporation (http://developer.intel.com/design/
packtech/)
Please contact your Intel representative for information related to EEPROM programming maps
and ASF 1.0 implementation.
2
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
1.4
Product Codes
Table 1 lists the product ordering codes for the 82562G/GT and 82562ET/EM.
Table 1.
Product Ordering Codes
Device
1.5
Product Code
Product Code (Lead Free)
82562G
GD82562G
LU82562G
82562GT
GD82562GT
LU82562GT
82562ET
DA82562ET
LU82562ET
82562EM
DA82562EM
LU82562EM
Usage Modes for the 82562G/GT
This section describes the usage modes for 82562G/GT devices.
1.5.1
Mode 0: Drop-in Replacement
Mode 0 is a drop-in replacement for a similar 82562ET/EM device without any required software
or hardware modifications. 82562ET/EM product collateral can be used to design for this usage
mode.
Note:
1.5.2
For this mode, some BOM component values can be changed to improve performance using
82562G/GT devices without changing the layout of a board designed for 82562ET/EM devices.
For example, transmit and receive termination resistors as well as RBIAS10 and RBIAS100
resistor values.
Modes 1, 2, 3, and 4: New Features
82562G/GT devices support several new features that offer design flexibility and reduced BOM
cost compared to 82562ET/EM devices. To implement these new features, the board design must
include the proper pull-up and/or pull-down strapping resistor options that are used to change
modes of operation (refer to Table 2).
Application Note (AP-414)
3
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Table 2.
New Usage Modes
Mode
Design Impact
Mode 0: 82562ET/EM
compatible.
No BOM changes necessary
for equivalent performance to
82562ET/EM.
Equivalent functionality to the 82562ET/
EM.
Mode 1: LED configuration B and
single-pin LAN disable.
Usability and reduced BOM
cost.
Strapping resistors, LAN Disable circuit
and LED circuit design.
Mode 2: Same as mode 1,
except LED configuration C.
Usability and reduced BOM
cost.
Strapping resistors, LAN Disable circuit
and LED circuit design.
Mode 3: LED configuration B,
Single Pin LAN Disable, and
enhanced Tx mode1.
Usability, reduced BOM cost,
and stronger Tx drive strength.
Strapping resistors, LAN Disable circuit
and LED circuit design.
Usability, reduced BOM cost,
and stronger Tx drive strength.
Strapping resistors, LAN Disable circuit
and LED circuit design.
Mode 4: Same as mode 3,
except LED configuration C.
See footnote 1.
1.
4
Benefit
Only use this mode if advised to do so by an Intel representative.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
2.0
Frequency Control Device Design Considerations
This section provides information regarding frequency control devices, including crystals and
oscillators, for use with all Intel® Ethernet controllers. Several suitable frequency control devices
are available; none of which present any unusual challenges in selection. The concepts documented
herein are applicable to other data communication circuits, including Physical Layer devices
(PHYs).
The Intel® Ethernet controllers contain amplifiers which, when used with the specific external
components, form the basis for feedback oscillators. These oscillator circuits, which are both
economical and reliable, are described in more detail in “Crystal Selection Parameters”.
The Intel® Ethernet controllers also have bus clock input functionality, however a discussion of
this feature is beyond the scope of this document, and will not be addressed.
The chosen frequency control device vendor should be consulted early in the design cycle. Crystal
and oscillator manufacturers familiar with networking equipment clock requirements may provide
assistance in selecting an optimum, low-cost solution.
2.1
Frequency Control Component Types
Several types of third-party frequency reference components are currently marketed. A discussion
of each follows, listed in preferred order.
2.2
Quartz Crystal
Quartz crystals are generally considered to be the mainstay of frequency control components due to
their low cost and ease of implementation. They are available from numerous vendors in many
package types and with various specification options (see Table 3).
Table 3.
Recommended Crystals
Manufacturer
2.3
Part Number
Raltron
AS-25.000-20-F-SMD-T
Citizen America Corp
HCM4925.000MBBKTR
NDK America Inc
41CD25.0S11005020
TXC Corporation - USA
6C25000131
Fixed Crystal Oscillator
A packaged fixed crystal oscillator is comprised of an inverter, a quartz crystal, and passive
components conveniently packaged together. The device renders a strong, consistent square wave
output. Oscillators used with microprocessors are supplied in many configurations and tolerances.
Crystal oscillators should be restricted to use in special situations, such as shared clocking among
devices or multiple controllers. As clock routing can be difficult to accomplish, it is preferable to
provide a separate crystal for each device.
Application Note (AP-414)
5
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
For Intel® Ethernet controllers, it is acceptable to overdrive the internal inverter by connecting a
25 MHz external oscillator to the X1 lead, leaving the X2 lead unconnected. The oscillator should
be specified to drive CMOS logic levels, and the clock trace to the controller should be as short as
possible. Controller specifications typically call for a 40% (minimum) to 60% (maximum) duty
cycle and a ±50 ppm frequency tolerance across the entire operating temperature range as required
by IEEE specifications. Intel recommends a ±30 ppm frequency tolerance.
Note:
2.4
Please contact your Intel Customer Representative to obtain the most current device documentation
prior to implementing this solution.
Programmable Crystal Oscillators
A programmable oscillator can be configured to operate at many frequencies. The device contains
a crystal frequency reference and a phase lock loop (PLL) clock generator. The frequency
multipliers and divisors are controlled by programmable fuses.
A programmable oscillator’s accuracy depends heavily on the Ethernet controller’s differential
transmit lines. The Physical Layer (PHY) uses the clock input from the device to drive a
differential Manchester (for 10 Mbps operation) or an MLT-3 (for 100 Mbps operation) encoded
analog signal across the twisted pair cable. These signals are referred to as self-clocking, which
means the clock must be recovered at the receiving link partner. Clock recovery is performed with
another PLL that locks onto the signal at the other end.
PLLs are prone to exhibit frequency jitter. The transmitted signal can also have considerable jitter
even with the programmable oscillator working within its specified frequency tolerance. PLLs
must be designed carefully to lock onto signals over a reasonable frequency range. If the
transmitted signal has high jitter and the receiver’s PLL loses its lock, then bit errors or link loss
can occur.
PHY devices are deployed for many different communication applications. Some PHYs contain
PLLs with marginal lock range and cannot tolerate the jitter inherent in data transmission clocked
with a programmable oscillator. The American National Standards Institute (ANSI) X3.263-1995
standard test method for transmit jitter is not stringent enough to predict PLL-to-PLL lock failures,
therefore, the use of programmable oscillators is generally not recommended.
2.5
Ceramic Resonator
Similar to a quartz crystal, a ceramic resonator is a piezoelectric device. A ceramic resonator
typically carries a frequency tolerance of ±0.5%, – inadequate for use with Intel® Ethernet
controllers, and therefore, should not be used.
6
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.0
Ethernet Component Design Guidelines
This section provides recommendations for selecting components and connecting special pins. The
main design elements are the 82562G/GT and 82562ET/EM PLC devices external resistor
connections, a magnetics module with RJ-45 connector, and a crystal clock source.
3.1
General Design Considerations for Ethernet Controllers
These recommendations apply to all 10/100 Mbps designs.
Good engineering practices should be followed with respect to unused inputs by terminating them
with pull-up or pull-down resistors, unless the datasheet, design guide or reference schematic
indicates otherwise. Do not attach pull-up or pull-down resistors to any balls identified as reserved
(unless explicitly included in the reference schematic). These devices may have special test modes
that could be entered inadvertently.
3.1.1
Crystal Selection Parameters
Quartz crystals are generally considered to be the mainstay of frequency control components due to
their low cost and ease of implementation. They are available from numerous vendors in many
package types and with various specification options.
All crystals used with Intel® Ethernet controllers are described as “AT-cut”, which refers to the
angle at which the unit is sliced with respect to the long axis of the quartz stone.
Table 4 lists the crystal electrical parameters and provides suggested values for typical designs. The
parameters listed are described in the following subsections.
Table 4.
Crystal Parameters
Parameter
Vibration Mode
Nominal Frequency
Frequency Tolerance
Suggested Value
Fundamental
25,000 MHz at 25° C (required)
• ±30 ppm recommended; ±50 ppm across the entire operating
temperature range as required by IEEE specifications
• ±30 ppm required for the 82562G/GT
Temperature Stability
• ±50 ppm at 0° C to 70° C
• ±30 ppm at 0° C to 70° C required for the 82562G/GT
Calibration Mode
Non Operating Temperature
Range
Load Capacitance
Parallel
-40 to 90° C for the 82562G/GT
• 16 pF to 20 pF
• 20 pF required for the 82562G/GT
Pullability from Nominal Load
Capacitance
15 ppm/pF maximum for the 82562G/GT
Shunt Capacitance
6 pF maximum
Equivalent Series Resistance
50 Ω maximum
Drive Level
Application Note (AP-414)
0.5 mW maximum
7
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Table 4.
Crystal Parameters
Aging
Insulation Resistance
Package
Note:
±5 ppm per year maximum
500 MΩ minimum at DC 100 V for the 82562G/GT
HC49 for the 82562GZ(GX)
A sampling of crystals that meet the specifications outlined for the 82562G/GT and 82562ET/EM
devices are listed below:
Epson-Seiko MA-406-25.000M-20PF*
Epson-Seiko MA-406H*
Please consult with your Intel representative before implementing a design that uses another type
of clock source. Careful design is required if using a fixed oscillator. Intel discourages the use of
programmable oscillators and ceramic resonators. See Appendix A, “Measuring LAN Reference
Frequency Using a Frequency Counter” for more information.
3.1.1.1
Vibration Mode
Crystals in the frequency range listed in Table 4 are available in both fundamental and third
overtone. Unless there is a special need for third overtone, use fundamental mode crystals.
At any given operating frequency, third overtone crystals are thicker and more rugged than
fundamental mode crystals. Third overtone crystals are more suitable for use in military or harsh
industrial environments. Third overtone crystals require a trap circuit (extra capacitor and inductor)
in the load circuitry to suppress fundamental mode oscillation as the circuit powers up. Selecting
values for these components is beyond the scope of this document.
3.1.1.2
Nominal Frequency
Intel® Ethernet controllers use a crystal frequency of 25.000 MHz. The 25 MHz input is used to
generate a 125 MHz transmit clock for 100BASE-TX operation; 10 MHz and 20 MHz transmit
clocks, for 10BASE-T operation.
3.1.1.3
Frequency Tolerance
The frequency tolerance for an Ethernet physical layer device is dictated by the IEEE 802.3
specification as ±50 parts per million (ppm). This measurement is referenced to a standard
temperature of 25° C.
Note:
8
Intel recommends a frequency tolerance of ±30 ppm.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.1.1.4
Temperature Stability and Environmental Requirements
Temperature stability is a standard measure of how the oscillation frequency varies over the full
operational temperature range (and beyond). Several optional temperature ranges are currently
available, including -40° C to +85° C for industrial environments. Some vendors separate operating
temperatures from temperature stability. Manufacturers may also list temperature stability as 50
ppm in their data sheets.
Note:
Crystals also carry other specifications for storage temperature, shock resistance, and reflow solder
conditions. Crystal vendors should be consulted early in the design cycle to discuss the application
and its environmental requirements.
3.1.1.5
Calibration Mode
The terms “series-resonant” and “parallel-resonant” are often used to describe crystal circuits.
Specifying parallel mode is critical to determining how the crystal frequency is calibrated at the
factory.
A crystal specified and tested as series resonant oscillates without problem in a parallel-resonant
circuit, but the frequency is higher than nominal by several hundred parts per million. The purpose
of adding load capacitors to a crystal circuit is to establish resonance at a frequency higher than the
crystal’s inherent series resonant frequency.
Figure 1 illustrates a simplified schematic of the 82562G/GT and 82562ET/EM device’s crystal
circuit. The crystal and the capacitors form a feedback element for the internal inverting amplifier.
This combination is called parallel-resonant, because it has positive reactance at the selected
frequency. In other words, the crystal behaves like an inductor in a parallel LC circuit.
LAN
Silicon
X1 or Xin
C1
LAN
Silicon
X2 or Xout
C2
Figure 1. Crystal Circuit
Application Note (AP-414)
9
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.1.1.6
Load Capacitance
The formula for crystal load capacitance is as follows:
( C1 ⋅ C2 )
C L = ------------------------- + C stray
( C1 + C2 )
where C1 = C2 = 22 pF (as suggested in most Intel reference designs)
and Cstray = allowance for additional capacitance in pads, traces and the chip carrier
within the Ethernet controller package
An allowance of 3 pF to 7 pF accounts for lumped stray capacitance. The calculated load
capacitance is 16 pF with an estimated stray capacitance of about 5 pF.
Individual stray capacitance components can be estimated and added. For example, surface mount
pads for the load capacitors add approximately 2.5 pF in parallel to each capacitor. This technique
is especially useful if Y1, C1 and C2 must be placed farther than approximately one-half (0.5) inch
from the controller. It is worth noting that thin circuit boards generally have higher stray
capacitance than thick circuit boards.
Standard capacitor loads used by crystal manufacturers include 16 pF, 18 pF and 20 pF. Any of
these values will generally operate with the controller. However, a difference of several picofarads
between the calibrated load and the actual load will pull the oscillator slightly off frequency.
Note:
C1 and C2 can vary by as much as 5% (approximately 1 pF) from their nominal values.
3.1.1.7
Shunt Capacitance
The shunt capacitance parameter is relatively unimportant compared to load capacitance. Shunt
capacitance represents the effect of the crystal’s mechanical holder and contacts. The shunt
capacitance should equal a maximum of 6 pF (7 pF is also acceptable).
3.1.1.8
Equivalent Series Resistance
Equivalent Series Resistance (ESR) is the real component of the crystal’s impedance at the
calibration frequency, which the inverting amplifier’s loop gain must overcome. ESR varies
inversely with frequency for a given crystal family. The lower the ESR, the faster the crystal starts
up. Use crystals with an ESR value of 50 Ω or better.
3.1.1.9
Drive Level
Drive level refers to power dissipation in use. The allowable drive level for a Surface Mounted
Technology (SMT) crystal is less than its through-hole counterpart, because surface mount crystals
are typically made from narrow, rectangular AT strips, rather than circular AT quartz blanks.
Some crystal data sheets list crystals with a maximum drive level of 1 mW. However, Intel®
Ethernet controllers drive crystals to a level less than the suggested 0.5 mW value. This parameter
does not have much value for on-chip oscillator use.
10
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.1.1.10
Aging
Aging is a permanent change in frequency (and resistance) occurring over time. This parameter is
most important in its first year because new crystals age faster than old crystals. Use crystals with a
maximum of ±5 ppm per year aging.
3.1.2
Reference Crystal
The normal tolerances of the discrete crystal components can contribute to small frequency offsets
with respect to the target center frequency. To minimize the risk of tolerance-caused frequency
offsets causing a small percentage of production line units to be outside of the acceptable frequency
range, it is important to account for those shifts while empirically determining the proper values for
the discrete loading capacitors, C1 and C2.
Even with a perfect support circuit, most crystals will oscillate slightly higher or slightly lower than
the exact center of the target frequency. Therefore, frequency measurements (which determine the
correct value for C1 and C2) should be performed with an ideal reference crystal. When the
capacitive load is exactly equal to the crystal’s load rating, an ideal reference crystal will be
perfectly centered at the desired target frequency.
3.1.3
Reference Crystal Selection
There are several methods available for choosing the appropriate reference crystal:
• If a Saunders and Associates (S&A) crystal network analyzer is available, then discrete crystal
components can be tested until one is found with zero or nearly zero ppm deviation (with the
appropriate capacitive load). A crystal with zero or near zero ppm deviation will be a good
reference crystal to use in subsequent frequency tests to determine the best values for C1 and
C2.
• If a crystal analyzer is not available, then the selection of a reference crystal can be done by
measuring a statistically valid sample population of crystals, which has units from multiple
lots and approved vendors. The crystal, which has an oscillation frequency closest to the center
of the distribution, should be the reference crystal used during testing to determine the best
values for C1 and C2.
• It may also be possible to ask the approved crystal vendors or manufacturers to provide a
reference crystal with zero or nearly zero deviation from the specified frequency when it has
the specified CLoad capacitance.
When choosing a crystal, customers must keep in mind that to comply with IEEE specifications for
10/100Base-T Ethernet LAN, the transmitter reference frequency must be precise within ±50 ppm.
Intel® recommends customers to use a transmitter reference frequency that is accurate to within
±30 ppm to account for variations in crystal accuracy due to crystal manufacturing tolerance. For
information about measuring transmitter reference frequency, refer to Appendix A, “Measuring
LAN Reference Frequency Using a Frequency Counter”.
3.1.4
Circuit Board
Since the dielectric layers of the circuit board are allowed some reasonable variation in thickness,
the stray capacitance from the printed board (to the crystal circuit) will also vary. If the thickness
tolerance for the outer layers of dielectric are controlled within ±17 percent of nominal, then the
circuit board should not cause more than ±2 pF variation to the stray capacitance at the crystal.
When tuning crystal frequency, it is recommended that at least three circuit boards are tested for
frequency. These boards should be from different production lots of bare circuit boards.
Application Note (AP-414)
11
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Alternatively, a larger sample population of circuit boards can be used. A larger population will
increase the probability of obtaining the full range of possible variations in dielectric thickness and
the full range of variation in stray capacitance.
Next, the exact same crystal and discrete load capacitors (C1 and C2) must be soldered onto each
board, and the LAN reference frequency should be measured on each circuit board.
The circuit board, which has a LAN reference frequency closest to the center of the frequency
distribution, should be used while performing the frequency measurements to select the appropriate
value for C1 and C2.
3.1.5
Temperature Changes
Temperature changes can cause the crystal frequency to shift. Therefore, frequency measurements
should be done in the final system chassis across the system’s rated operating temperature range.
3.2
Analog References
There are two inputs, RBIAS10 and RBIAS100, that require external resistor connections to bias
the internal analog section of the device. These inputs are sensitive to the resistor value and
experimentation is needed to select the correct values for any given layout. Resistors of 1%
tolerance must be used. Figure 2 shows an example of one possible design.
Figure 2. RBIAS10 and RBIAS100 Circuits
82562GZ/GX
619
1%
649
1%
12
R B IA S 1 0
R B IA S 1 0 0
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.3
Integrated Magnetics Module
The magnetics module has a critical effect on overall IEEE and emissions conformance. The
device should meet the performance required for a design with reasonable margin to allow for
manufacturing variation. Occasionally, components that meet basic specifications may cause the
system to fail IEEE testing because of interactions with other components or the Printed Circuit
Board (PCB) itself. Carefully qualifying new magnetics modules can go a long way toward
preventing this type of problem.
The steps involved in magnetics module qualification are similar to those for oscillator
qualification:
1. Verify that the vendor's published specifications in the component data sheet meet the required
IEEE specifications.
2. Independently measure the component's electrical parameters on a test bench, checking
samples from multiple lots. Check that the measured behavior is consistent from sample to
sample as well as meeting the published specifications.
3. Perform physical layer conformance testing and EMC (FCC and EN) testing in real systems.
3.4
Designing with the Platform LAN Connect Device
This section provides design guidelines specific to the PLC device.
3.4.1
Power Supplies
PLC devices use a single 3.3 V power supply. The 3.3 V supply must provide approximately 90
mA of current for full speed operation. Standby power must be furnished in order to wake up from
a power down.
3.4.2
Device Test Capability
PLC devices contain an XOR test tree mechanism for simple board tests. Details of the XOR tree
operation are contained in the 82562G/GT and 82562ET/EM datasheets.
3.4.3
PLC Device LAN Disable Guidelines
For the 82562G/GT drop-in mode LAN disable circuit, see the “Drop-in Replacement Schematic”
in Section 7.0 and the appropriate 82562ET/EM product design guide.
3.4.4
Serial EEPROM
Serial EEPROM for LAN implementations based on PLC devices connect to the ICH5, ICH6, or
ICH7 for the 82562G/GT (ICH2, ICH3, or ICH4 for the 82562ET/EM). Depending on the size of
the EEPROM, the device can support legacy manageability or not. Table 5 and Table 6 list the
EEPROM map for the PLC device; Table 7 lists the recommended EEPROM manufacturers. For
details on the EEPROM, see the appropriate I/O Control Hub 2, 3, 4, 5, 6, and 7 EEPROM Map
and Programming Information.
Application Note (AP-414)
13
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Note:
Table 5.
See your Intel representative for later information on later versions of the I/O Control Hub.
Memory Layout (128B EEPROM)
00h
HW/SW Reserved Area
3Fh
Note:
Table 6.
No manageability provided.
Memory Layout (512B EEPROM)
00h
HW/SW Reserved Area
3Fh
40h
FFh
Note:
Table 7.
Legacy manageability only.
Recommended EEPROM Manufacturers
Vendor
Part Number
Package
Interface
Size (Kb)
Catalyst1
CAT93C46S-TE13
SOIC8
uWire
1
Atmel
AT93C46-10SI-2.7
SOIC8
uWire
1
Catalyst
CAT93C66S-TE13
SOIC8
uWire
4
Atmel
AT93C66-10SI-2.7
SOIC8
uWire
4
1.
14
ASF and Legacy
Manageability
Revision H is not supported. Product die revision letter is marked on top of the package as a suffix to the production data
code (e.g., AYWWH.)
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
3.4.5
Magnetics Modules for PLC Devices
A 5-core magnetics module should be carefully selected for specific designs. Table 8 lists
suggested integrated magnetics modules for use with PLC devices. These modules also contain
integrated USB jacks. Table 9 lists the electrical specifications for the 10/100 magnetics.
Table 8.
Recommended Magnetics Modules
Manufacturer
3.5
Part Number
Type
Pulse
H1138
Discrete
Pulse
JWOA1P01R
Integrated
Stewart Connector
Systems
SI-70027
RJ-45/Magnetic
Pulse
H1338 (MDI-X only)
Discrete
Flash Interface
The ICHx does not support a Flash interface.
Note:
The Intel Boot Agent is supported via the System BIOS.
Application Note (AP-414)
15
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Table 9.
Electrical Specifications at 25°C for 10/100 Magnetics
Insertion Loss (TX / RX)
0.1 through 0.999 MHz
1.0 dB maximum
1.0 through 15 MHz
0.35 dB maximum
15.1 through 6 0MHz
0.7 dB maximum
60.1 through 100 MHz
1.2 dB maximum
Return Loss (TX / RX)
1.0 through 30 MHz
18 dB minimum
30.1 through 60 MHZ
19 - [20Log(f/30 MHz)] dB minimum
60.1 through 80 MHz
12 dB minimum
Transmit Common Mode-to-Common Mode Reject
1.0 through 60 MHz
48 dB minimum
60.1 through 100 MHz
43 dB minimum
100.1 through 150 MHz
42 dB minimum
Effective Common Mode-to-Common Mode Reject
1.0 through 60 MHz
38 dB minimum
60.1 through 100 MHz
34 dB minimum
100.1 through 150 MHz
32 dB minimum
Transmit Differential to Common Mode Reject
1.0 through 60 MHz
38 dB minimum
60.1 through 100 MHz
35 dB minimum
100.1 through 150 MHz
32 dB minimum
Receive Differential to Common Reject
1.0 THRU 60 MHz
30 dB minimum
60.1 through 100 MHz
25 dB minimum
100.1 through 150 MHz
20 dB minimum
Crosstalk Isolation (TX / RX)
1.0 through 60 MHz
48 dB minimum
60.1 through 100 MHz
43 dB minimum
100.1 through 150 MHz
38 dB minimum
High Voltage Isolation
16
IEEE 14.3.1.1
2250 V dc for 60 seconds
OCL with 8mA Bias 100 KHz
400 µH
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.0
General Layout Considerations for PLC Devices
Critical signal traces should be kept as short as possible to decrease the likelihood of being affected
by high frequency noise from other signals, including noise carried on power and ground planes.
Keeping the traces as short as possible can also reduce capacitive loading.
Since the transmission line medium extends onto the PCB, special attention must be paid to layout
and routing of the differential signal pairs.
The differential signal pairs should not be routed near each other over long distances. Routing them
too close to each other induces crosstalk and can also cause common mode noise that degrades the
long cable receive bit error rate performance. To prevent these problems, separate the differential
pairs from each other by at least 5 times the height from the GND plane (Figure 3). For example,
separate them by 35 mils on a 7 mil thick prepreg.
4.1
Guidelines for Component Placement
Component placement can affect signal quality, emissions, and component operating temperature
This section provides guidelines for component placement.
Careful component placement can:
• Decrease potential problems directly related to EMI, which could cause failure to meet
applicable government test specifications.
• Simplify the task of routing traces. To some extent, component orientation affects the
complexity of trace routing. One overall objective is to minimize turns and crossovers between
traces.
The following recommendations can be used as guidelines in the layout phase of the design
implementation:
1. The device should be located at least one inch away from the RJ45 connector (distance D in
Figure 4).
2. The device should be placed at least two inches from the PCB edge (distance E in Figure 4).
Minimizing the amount of space needed for the Ethernet LAN interface is important because other
interfaces will compete for physical space on a LOM near the connector. The Ethernet LAN
circuits need to be as close as possible to the connector.
Figure 3 shows some basic placement distance guidelines. The ideal placement for the device
would be approximately one inch behind the magnetics module. Also note that the Tx and Rx
termination resistors are located close to the device. This is vital for meeting IEEE physical layer
conformance tests.
Application Note (AP-414)
17
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figure 3. General Placement Distances
Keep LAN silicon and traces at least 1 inch from edge of
PB (2 inches is preferred)
Keep LAN silicon 1 to 4 inches from LAN
connector
PLC
Device
Integrated
RJ-45
w/LAN
Magnetics
Keep 5 times the distance to the reference plane
between Tx and Rx differential pairs
While it is generally a good idea to minimize lengths and distances, this figure also illustrates the
need to keep the LAN silicon (PLC device) away from the edge of the PCB and the magnetics
module for best EMI performance.
4.1.1
Crystals
Crystals should not be placed near I/O ports or PCB edges. Radiation from these devices may be
coupled onto the I/O ports or out of the system chassis. Crystals should also be kept away from the
Ethernet magnetics module to prevent interference. Traces should be referenced to a continuous
low impedance ground plane.
Place the crystal and its load capacitors on the PCBs as close to the PLC device as possible (within
0.75-inch). Keep other potentially noisy traces away from the crystal traces.
The restraining straps of the crystal should be grounded to reduce the possibility of radiation from
the crystal’s case. Crystals should lay flat against the PCB to provide better coupling of
electromagnetic fields to the PCB.
4.1.2
Board Stackup Recommendations
PCBs for these designs typically have four, six, eight, or more layers. Following is a description of
a typical four-layer board stackup:
• Layer 1 is a signal layer. It can contain the differential analog pairs from the PLC device to the
magnetics module.
• Layer 2 is a signal ground layer. Chassis ground may also be fabricated in Layer 2 under the
connector side of the magnetics module.
18
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
• Layer 3 is used for power planes.
• Layer 4 is a signal layer.
This board stackup configuration can be adjusted to conform to specific design rules.
4.2
Critical Dimensions for Discrete Magnetics Module and RJ45
There are four critical dimensions that must be considered during the layout phase of an LOM
implementation. These dimensions are identified in Figure 4 as A, B, C, and D.
Figure 4. Critical Dimensions for Component Placement (Discrete Magnetics Solution)
!
"
#
#HIPSET
PLC
':'8
Device
0)%2
PIN"'!
-AGNETICS
-ODULE
$
2*
%
0#"%DGE
4.2.1
Distance A: Magnetics to RJ45 (Priority 1)
The distance labeled “A” in Figure 4 should be given the highest priority in board layout. The
distance between the magnetics module and the RJ45 connector should be kept to less than one
inch of separation. The following trace characteristics are important and should be observed:
• Differential Impedance. The differential impedance should be 100 Ω. The single ended trace
impedance will be approximately 50 Ω; however, the differential impedance can also be
affected by the spacing between the traces.
• Trace Symmetry. Differential pairs should be routed with consistent separation and with
exactly the same lengths and physical dimensions (for example, width).
Caution:
Asymmetrical and unequal length traces in the differential pairs contribute to common mode noise,
which can degrade the receive circuit’s performance and contribute to radiated emissions from the
transmit circuit.
If a PLC device must be placed further than two inches from the RJ45 connector, distance “B” can
be sacrificed. Keeping distance “A” as short as possible should be a priority.
Application Note (AP-414)
19
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.2.2
Distance B: PHY to Magnetics (Priority 2)
Distance B in Figure 4 should also be designed to extend less than two inches between devices.
The high speed nature of the signals propagating through these traces requires that the distance
between these components are closely observed. In general, any section of traces that is intended
for use with high speed signals should observe proper termination practices. Proper termination of
signals can reduce reflections caused by impedance mismatches between devices and traces.
The reflections of a signal may have a high frequency component that may contribute more EMI
than the original signal itself. For this reason, these traces should be designed to a 100 Ω
differential value.
4.2.3
Distance C: LAN Connect Interface Distance
This section contains guidelines for LOM designs that comply with the LCI. These guidelines
should not be treated as a specification; however, it must be ensured that the system meets
specified timings. This can be verified through simulations or other techniques. The LCI can be
routed to support a 10/100 Mbps LOM solution with PLC devices.
Note:
On the LOM design, the length of each data trace is either equal in length to the JCLK trace or up
to 0.5 inches shorter than the JCLK trace.
The length between distance C and the LCI should be less than 12 inches.
4.2.4
Distance D: The Overall Length of Differential Traces from LAN to RJ45 (Priority 4)
The overall length of differential pairs should be less than four inches measured from the PLC
device to RJ-45 through the magnetics module.
The lengths of the differential traces (within each pair) should be equal within 50 mils (1.25 mm)
and as symmetrical as possible.
4.2.5
Distance E: PLC Device to PCB Edge
The PLC device should be placed at least one inch from the PCB edge (two inches is preferred).
4.3
Critical Dimensions for an Integrated Magnetics Module
Figure 5 shows the critical dimensions for component placement with an integrated magnetics
module.
20
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
B
A
8 25 6 2 G Z (G X )/
8
2 5 4Device
1P I(E R )
PLC
1 9 6 p in s B G A
C h ip se t
C
M a g n e tics
M o d u le
P C B E dg e
Figure 5. Critical Dimensions for Component Placement with Integrated Magnetics Module
4.3.1
Distance A: The Overall Length of Differential Traces
The overall length of differential pairs should be between one and four inches measured from the
PLC device to the RJ-45 connector having integrated magnetics (shortest lengths will give best
performance.
4.3.2
Distance B: PLC Device to Chipset
For LCI on 82562G/GT devices, the maximum length should be less than 12 inches on an ICH5,
ICH6, or ICH7 platform. For LCI on 82562ET/EM devices, the maximum length should be less
than 12 inches on an ICH2, ICH3, or ICH4 platform.
4.3.3
Distance C: LAN Controller to PCB Edge
The LAN controller should be placed at least one inch from the PCB edge (two inches is preferred).
4.4
Differential Pair Trace Routing
Trace routing considerations are important to minimize the effects of crosstalk and propagation
delays on sections of the PCB where high-speed signals exist. Signal traces should be kept as short
as possible to decrease interference from other signals, including those propagated through power
and ground planes.
Application Note (AP-414)
21
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Observe the following suggestions to help optimize board performance:
• Maintain constant symmetry and spacing between the traces within a differential pair.
• Keep the signal trace lengths within a differential pair equal to each other.
• Keep the total length of each differential pair under four inches. Designs with differential
traces longer than five inches are much more likely to have:
— Degraded receive Bit Error Rate (BER) performance
— IEEE PHY conformance failures
— Excessive EMI radiation
• Keep at least 5 times the distance to the reference plane between Tx and Rx differential pairs.
• Do not route any other signal traces parallel to the differential pairs closer than 5 times the
distance to the reference plane.
• Keep maximum separation within differential pairs to seven mils.
• For high-speed signals, the number of corners and vias should be kept to a minimum. If a 90°
bend is required, it is recommended to use two 45° bends instead. See Figure 6.
Figure 6. Corner Trace Routing
45°
45°
• Traces should be routed away from PCB edges by 10 mils. This allows the field around the
trace to couple more easily to the ground plane rather than to adjacent wires or boards.
• Do not route traces and vias under crystals or oscillators. This prevents coupling to or from the
clock. And as a general rule, place traces from clocks and drives at a minimum distance from
apertures by a distance that is greater than the largest aperture dimension.
• The reference plane for the differential pairs should be continuous and low impedance. It is
recommended that the reference plane be ground. This provides an adequate return path for
high frequency noise currents.
• Do not route differential pairs over splits in the associated reference plane.
• Differential termination components should be placed as close as possible to the PLC device.
22
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.4.1
Signal Trace Geometry
The key factors in controlling trace EMI radiation are the trace length and the ratio of trace-width
to trace-height above the ground plane. To minimize trace inductance, high-speed signals and
signal layers that are close to a ground or power plane should be as short and wide as practical.
Ideally, this trace width to height above the ground plane ratio is between 1:1 and 3:1. To maintain
trace impedance, the width of the trace should be modified when changing from one board layer to
another if the two layers are not equidistant from the power or ground plane.
Each pair of signals should have a differential impedance of 100 Ω. +/- 20%. If a particular tool
cannot correctly calculate or predict differential traces, it is permissible to specify 55 to 60 Ω
single-ended traces as long as the spacing between the two traces is minimized. As an example,
consider a differential trace pair on Layer 1 that is 8 mils (0.2 mm) wide and 2 mils (0.05 mm)
thick, with a spacing of eight mils (0.2mm). If the fiberglass layer is 8 mils (0.2 mm) thick with a
dielectric constant, ER, of 4.7, the calculated single-ended impedance would be approximately
61 Ω and the calculated differential impedance would be approximately 100 Ω..
When performing a board layout, do not allow the CAD tool auto-router to route the differential
pairs without intervention. In most cases, the differential pairs will have to be routed manually.
Note:
4.4.2
Measured differential trace impedance for layout designs targeting 100 Ω often indicates lower
actual impedance. Designers should verify actual trace impedance and adjust the layout
accordingly. If the actual impedance is consistently low, a target of 105 – 110 Ω should compensate
for second order effects.
Trace Length and Symmetry
As indicated earlier, the overall length of differential pairs should be less than four inches measured
from the LAN controller to the RJ-45.
The differential traces (within each pair) should be equal length within 50 mils (1.25 mm) and as
symmetric as possible. Asymmetric and unequal length traces in the differential pairs contribute to
common mode noise. Common mode noise can degrade the receive circuit’s performance and
contribute to radiated emissions.
4.4.3
Impedance Discontinuities
Impedance discontinuities cause unwanted signal reflections. Avoid vias (signal through holes) and
other transmission line irregularities. If vias must be used, a reasonable budget is two per
differential trace. Unused pads and stub traces should also be avoided.
Application Note (AP-414)
23
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.4.4
Reducing Circuit Inductance
Traces should be routed over a continuous ground plane with no interruptions. If there are vacant
areas on a ground or power plane, the signal conductors should not cross the vacant area. This
increases inductance and associated radiated noise levels. Noisy logic grounds should be separated
from analog signal grounds to reduce coupling. Noisy logic grounds can sometimes affect sensitive
DC subsystems such as analog to digital conversion, operational amplifiers, etc. All ground vias
should be connected to every ground plane layer; similarly, every power via should be connected to
all equal potential power plane layers. This helps reduce circuit inductance. Another
recommendation is to physically locate grounds to minimize the loop area between a signal path
and its return path. Rise and fall times should be as slow as permissible because signals with fast
rise and fall times contain many high frequency harmonics, which can radiate significantly. The
most sensitive signal returns closest to the chassis ground should be connected together. This
results in a smaller loop area and reduce the likelihood of crosstalk. The effect of different
configurations on the amount of crosstalk can be studied using electronics modeling software.
4.4.5
Signal Isolation
To maintain best signal integrity, keep digital signals far away from the analog traces. If digital
signals on other PCB layers cannot be separated by a ground plane, they should be routed at right
angles with respect to the differential pairs. If there is another PLC device on the PCB, take care to
keep the differential pairs from that circuit away.
Some rules to follow for signal isolation:
• Separate and group signals by function on separate layers if possible. Maintain a gap of five
times the distance to the reference plane between all differential pairs (Ethernet) and other
nets, but group associated differential pairs together.
• Physically group together all components associated with one clock trace to reduce trace
length and radiation.
• Isolate I/O signals from high-speed signals to minimize crosstalk, which can increase EMI
emission and susceptibility to EMI from other signals.
• Avoid routing high-speed LAN traces near other high-frequency signals associated with a
video controller, cache controller, processor, or other similar devices.
4.4.6
Power and Ground Planes
Good grounding requires minimizing inductance levels in the interconnections and keeping ground
returns short, signal loop areas small, and power inputs bypassed to signal return, will significantly
reduce EMI radiation.
The following guidelines help reduce circuit inductance in motherboards:
• Route traces over a continuous plane with no interruptions. Do not route over a split power or
split ground plane. If there are vacant areas on a ground or power plane, avoid routing signals
over the vacant area. This increases inductance and EMI radiation levels.
• All ground vias should be connected to every ground plane layer; similarly, every power via
should be connected to all equal potential power plane layers. This helps reduce circuit
inductance.
• Physically locate grounds between a signal path and its return. This minimizes the loop area.
24
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
• Avoid fast rise/fall times as much as possible. Signals with fast rise and fall times contain
many high frequency harmonics, which can radiate EMI.
• If the magnetics module is a discrete module, the ground plane beneath the magnetics module
should be split. The RJ45 connector side of the transformer module should have chassis
ground beneath it (see Section 4.4.8).
4.4.7
Traces for Decoupling Capacitors
Traces between decoupling and I/O filter capacitors should be as short and wide as practical. Long
and narrow traces are more inductive and would reduce the intended effect of decoupling
capacitors. Also for similar reasons, traces to I/O signals and signal terminations should be as short
as possible. Vias to the decoupling capacitors should be sufficiently large in diameter to decrease
series inductance.
4.4.8
Ground Planes Under a Discrete Magnetics Module
The magnetics module’s chassis or output ground (secondary side of transformer) should be
separated from the digital or input ground (primary side) by a physical separation of 100 mils
minimum. Splitting the ground planes beneath the transformer minimizes noise coupling between
the primary and secondary sides of the transformer and between the adjacent coils in the magnetics.
This arrangement also improves the common mode choke functionality of magnetics module.
Figure 7 illustrates the split plane layout for a discrete magnetics module. Capacitors are used to
interconnect chassis ground and signal ground.
Figure 7. Ground Plane Separation
0.10 Inches Minimum Spacing
Magnetics Module
Void or Separate
Ground Plane
Separate Chassis Ground Plane
Figure 8 shows the preferred method for implementing a ground split under an integrated
magnetics module/RJ-45 connector without USB. The capacitor stuffing options (C1-C6) are used
to reduce/filter high frequency emissions. The value(s) of the capacitor stuffing options may be
different for each PCB. Experiments need to be performed to determine which value(s) provide
best EMI performance. Integrated RJ-45 discrete magnetics with USB usually do not have split
planes under them.
Application Note (AP-414)
25
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figure 8. Ideal Ground Split Implementation (for Integrated RJ-45 without USB)
Board Edge
RJ/Mag.
Chassis
GND
Capacitor
Stuffing
Options
C1
C2
RJ Shield
connected
to Chassis
GND
Capacitor
Stuffing
Options
C3
C4
C5
C6
Digital
GND
Resistive
Terminations
LAN IC
The table below gives some starting values for these capacitors.
Capacitors
Value
C1, C6
4.7µF or 10 µF
C2, C3, C4, C5,
470 pF to 0.1 µF
The placement of C1 – C6 may also be different for each PCB design. For example, all capacitors
might not need to be populated). Also, the capacitors may not be needed on both sides of the
magnetic module.
4.4.9
Non-Integrated Magnetics Modules/RJ-45 Connectors)
It is possible to employ discrete (non-integrated) magnetics modules and RJ-45 connectors. Similar
rules apply to design and layout. The differential pairs should be routed to be as short and
symmetrical as possible and the overall lengths of the differential pairs (including the width of the
magnetics module) should not exceed approximately four inches.
26
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Additional design and layout steps are required to add a dedicated board termination plane parallel
to chassis ground, 75 Ω termination resistors, and a 1500 pF capacitor. This “Bob Smith”
termination scheme is normally contained inside an integrated magnetics module.
In Ethernet designs, it is common practice to terminate unused connections on the RJ-45 connector
and the magnetics module to ground. Depending on overall shielding and grounding design, this
may be done to the chassis ground, signal ground, or a termination plane. Care must be taken when
using various grounding methods to insure that emission requirements are met. In the “Bob Smith”
termination method, a floating termination plane is cut out of a power plane layer. This floating
plane acts as a plate of a capacitor with an adjacent ground plane. The signals can be routed
through 75 Ω resistors to the plane. Stray energy on unused pins is then carried to the plane.
It is recommended that the termination plane capacitance equal a minimum value of 1500 pF. This
helps reduce the amount of crosstalk on the differential pairs from the unused pairs of the RJ-45
connector. Pads may be placed for an additional capacitance to chassis ground, which may be
required if the termination plane capacitance is not large enough to pass Electrical Fast Transient
(EFT) testing. If a discrete capacitor is used, to meet the EFT requirements it should be rated for at
least 1000 Vac.
Figure 9. Termination Plane Example for PLC Device and Discrete Magnetics
TDP
N/C
TDN
RDP
RJ-45
RDN
Magnetics module
Termination Plane
Additional capacitance that may be
required for EFT testing
4.4.10
Layout Guidelines (Routing LAN 3.3 V When Using a Copper Trace)
When 3.3 V for the PLC device is NOT supplied by a solid copper power plane, then it becomes
more important to make sure the power source will not carry system noise to the PLC device, and
to ensure that the power trace does not restrict current flow to the PLC device.
4.4.10.1
Avoid Restricting Current Flow
When a 3.3 V power trace is used to supply power to the PLC device, the power trace should be at
least 50 mils wide, to avoid restricting current flowing to the PLC device. On designs where there
is enough PCB space, a power trace that is 200 mils wide or wider, is better.
Application Note (AP-414)
27
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.4.10.2
Power Trace Decoupling
If a power trace is more than an inch long, it should be decoupled at both the source and near the
destination.
Extremely long power traces should be decoupled every three to five inches. Placing a decoupling
cap on the power trace, once every few inches, greatly reduces the amount of noise that will reach
the PLC device. In-turn, this reduces radiated emissions, and improves IEEE PHY conformance.
Figure 10. Decoupled LAN Power Trace (Power Supplied by Trace)
C
C
C
C
C
C
C
C
LAN/LOM IC
Power Rail
C
Power rail between 30 - 50 mills wide
C
Pairs of caps are
4 inches apart
FB
C
C
Optional
Ferrite
Board
1. Big C >= 4.7 uF. Little c = 0.1 uF (or 0.01 uF).
2. Noise above 500 MHz might require a COG cap between 470 pF and 1000 pF.
3. To reduce noise in the LAN device and on the wire; If a power trace is more than an inch long, it should be
decoupled both at source and near destination. Also, a series Ferrite Bead near the destination can help.
4.4.10.3
Moat (a Space) Around LAN Power Trace, to Reduce Noise
From Adjacent Signals
To further reduce power supply noise, it is desirable to keep the LAN power trace or LAN power
fill separated from other signals and other voltage rails, by 30 mils, if possible. Separating power
traces and power-fills with 20 to 30 mil wide moats reduce signal and power noise from coupling
onto the LAN power trace or onto the LAN power-fill.
28
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figure 11. Using a Moat to Reduce Noise From Adjacent Traces and Power Fills
30 mil moat or gap between main power plane and other power fill areas
C
Optional
Ferrite
Board
Power trace between 50 - 200 mills wide
C
C
FB
C
C
Power trace between 50 - 200 mills wide
C
C
C
C
C
C
C
C
C
OMa
L
/ re
N
LAIC A
C
C
C
C
C
C
Main Power Plane
4.5
Signal Terminations
110 Ω (1%) resistors are used to terminate the transmit differential (TDP and TDN) and the receive
differential (RDP and RDN) pairs. They should be placed as close to the PLC device as possible
since they terminate the entire impedance seen at the termination source including the wire
impedance reflected through the transformer.
Termination resistor values were recently increased from 100 Ω to 110 Ω to improve return loss.
However, on some designs, this change caused the PCB’s output amplitude to be slightly above the
peak-to-peak center of the IEEE specification. As a result, RBIAS resistor values were increased
(RBIAS10 549 to 619 Ω and RBIAS100 619 to 649 Ω) to reduce the PCB’s output amplitude to
better meet the IEEE peak-to-peak center specification.
For 100Base-TX designs, the IEEE specification allows a -950 mVpk to -1050 mVpk for the
negative peak and +950 mVpk to +1050 mVpk for the positive peak. Ideally, a typical PCB output
amplitude should be within -975 mVpk to -1025 mVpk for the negative peak and +975 mVpk to
+1025 mVpk for the positive peak.
For 10Base-T designs, the IEEE specification allows a -2.2 mVpk to -2.8 mVpk for the negative
peak and +2.2 mVpk to +2.8 mVpk for the positive peak. Ideally, a typical PCB output amplitude
should be within -2.35 mVpk to -2.55 mVpk for the negative peak and +2.35 mVpk to +2.55 mVpk
for the positive peak.
The RBIAS values previously listed should be considered starting values. Intel recommends that
board designers measure each of their PCB’s output amplitude and then adjust the RBIAS values as
required.
Application Note (AP-414)
29
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figure 12. Termination Resistors Placement (Integrated Magnetics Solution)
/$1&RQQHFW,QWHUIDFH
3/&
'HYLFH
0DJQHWLFV
0RGXOH
5-
3ODFH7HUPLQDWLRQ
5HVLVWRUVDV&ORVH
WR3/&GHYLFHDV3RVVLEOH
4.5.1
Termination Plane
Resistors are used to terminate noise from the unused inputs of both the RJ45 connector and the
magnetics module to the termination plane. The netname “termplane” is provided as a guide to the
termination plane. A termplane is a plane fabricated into the PCB substrate. This plane, which has
no DC termination, acts like one-half of a capacitor that provides a path for the coupled noise.
4.5.2
Termination Plane Capacitance
It is recommended that the termination plane capacitance equal a minimum value of 1500 pF. This
helps reduce the amount of crosstalk on the differential pairs (TDP and TDN and RDP and RDN)
from the unused pairs of the RJ45. Pads may be placed for additional capacitance, which may be
required if failure occurs during electrical fast transient testing.
Note:
4.6
This capacitor must be designed to tolerate 2 KV voltage injections to meet International Special
Committee on Radio Interference (CISPR) Electrostatic Discharge (ESD) specifications.
Light Emitting Diodes
The PLC device has three high-current outputs to directly drive LEDs for link, activity and speed
indication. Since LEDs are likely to be integral to a magnetics module, take care to route the LED
traces away from potential sources of EMI noise. In some cases, it may be desirable to attach filter
capacitors.
30
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
4.7
Physical Layer Conformance Testing
Physical layer conformance testing (also known as IEEE testing) is a fundamental capability for all
companies with Ethernet LAN products. PHY testing is the final determination that a layout has
been performed successfully. If your company does not have the resources and equipment to
perform these tests, consider contracting the tests to an outside facility.
Crucial tests are as follows, listed in priority order:
1. Bit Error Rate (BER). This test is a good indicator of real world network performance. It
should be done with long and short cables and many link partners. The test limit is 10 to 11
errors (10/100 Mbps).
2. Output Amplitude, Rise and Fall Time (10/100 Mbps)
3. Return Loss. This test indicates proper impedance matching, measured through the RJ-45
connector back toward the magnetics module.
4. Jitter Test (10/100 Mbps).
5. Harmonic Content for 10 Mbps.
6. Output Symmetry for 100 Mbps.
7. Rise and Fall Time for 100 Mbps.
8. Duty Cycle Distortion for 100 Mbps.
4.8
Troubleshooting Common Physical Layout Issues
The following is a list of common physical layer design and layout mistakes in LOM designs.
1. Unequal length of the two traces within a differential pair. Inequalities create common-mode
noise and will distort the transmit or receive waveforms.
2. Lack of symmetry between the two traces within a differential pair. Asymmetry can create
common-mode noise and distort the waveforms. For each component or via that one trace
encounters, the other trace should encounter the same component or a via at the same distance
from the Ethernet silicon.
3. Excessive distance between the PLC device and the magnetics. Long traces on FR4 fiberglass
epoxy substrate will attenuate and distort the analog signals. In addition, any impedance
mismatch in the traces will be aggravated if they are longer than the four inch rule.
4. Routing any other trace parallel to and close to one of the differential traces. Crosstalk getting
onto the receive channel will cause degraded long cable BER. Crosstalk getting onto the
transmit channel can cause excessive EMI emissions and can cause poor transmit BER on long
cables. At a minimum, other signals should be kept 0.1 inch from the differential traces.
5. Routing one pair of differential traces too close to another pair of differential traces. After
exiting the PLC device, the trace pairs should be kept 0.1 inch or more away from the other
trace pairs. The only possible exceptions are in the vicinities where the traces enter or exit the
magnetics, the RJ-45 connector, and the LAN controller.
6. Using a low quality magnetics module.
7. Re-use of an out-of-date physical layer schematic in a PLC device design. The terminations
and decoupling can be different from one PHY to another.
Application Note (AP-414)
31
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
8. Incorrect differential trace impedances. It is important to have approximately 100 Ω
impedance between the two traces within a differential pair. This becomes even more
important as the differential traces become longer. To calculate differential impedance, many
impedance calculators only multiply the single-ended impedance by two. This does not take
into account edge to edge capacitive coupling between the two traces or other edge effects.
When the two traces within a differential pair are kept close to each other, the edge coupling
can lower the effective differential impedance by 5 Ω to 20 Ω. Short traces will have fewer
problems if the differential impedance is slightly off target.
9. Use of capacitor that is too large between the transmit traces or too much capacitance on the
magnetics module’s transmit center tap to ground. Using capacitors more than a few
picoFarads in either of these locations can slow the 100 Mbps rise and fall time. This will also
cause return loss to fail at higher frequencies and will degrade the transmit BER performance.
If capacitors are used, the total of all capacitors placed on the transmit traces and the center tap
should equal less than 22 pF.
32
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
5.0
Pinout Information
Table 9 lists the pin assignments for the PLC device.
Table 10. Pin Assignments
Pin
Number
Pin Name
Pin
Number
Pin Name
Pin
Number
Pin Name
Pin
Number
Pin Name
1
VCC
13
VSS
25
VCC
37
JRXD2
2
VCCA
14
VCCT
26
TOUT
38
VSSP
3
VSSA
15
RDP
27
LILED#
39
JCLK
40
VCCP
4
5
1.
2.
3.
RBIAS10
RBIAS100
16
17
RDN
VCCT
2
28
ISOL_TI
29
ISOL_EXEC2
41
ADV10/
LAN_DISABLE#3
6
VSSA2
18
VSS
30
ISOL_TCK2
42
JRSTSYNC
7
VCCA2
19
VCCR
31
SPDLED#
43
JTXD0
8
VSS
20
VSSR
32
ACTLED#
44
JTXD1
1
9
VCCT
21
TESTEN
33
VSSP
45
JTXD2
10
TDP
22
VSSR
34
JRXD0
46
X1
11
TDN
23
VCCR
35
JRXD1
47
X2
12
VCCT
24
VSS
36
VCCP
48
VSS
Requires an external 200 K Ω pull-up resistor.
Has an internal 10 K Ω pull-down resistor.
LAN_DISABLE# applicable to the 82562GT(G) only.
Application Note (AP-414)
33
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Note:
34
This page intentionally left blank.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
6.0
Self-Review Checklist for a LAN on Motherboard
Design
A Portable Data Format (PDF) Self-Review Checklist for a LAN on Motherboard design is
available to aid designers via:
http://developer.intel.com
Application Note (AP-414)
35
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Note:
36
This page intentionally left blank.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
7.0
Reference Schematics
Following are reference schematics for the 82562G/GT (Drop-In Mode 0).
Application Note (AP-414)
37
38
3 $ * ( , 1 ' ( ;
7 LWOH3 DJH
* 7 /$ 1 & RQWUROOHU0 DJDQG5-
PIN 3 3 /0
*7
02'('523,102'(
5()(5(1&('(6,*1
) NTEL
''4 2 EF $ES IGN
5
2 EV 82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Application Note (AP-414)
Application Note (AP-414)
7UDQVLVWRUPXVWEHSRZHUHG
E\9&&686VXSSO\
&RQQHFWWR,&+[
/&,LQWHUIDFH
5
''4 2 EF $ESIGN
) NTEL
7HUPSODQHLVDSODQHI LOOZKLFK
I RUPVDFDSDFLWDQFHZLWKUHVSHFW
WRWKHFKDVVLVJURXQG
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
39
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Note:
40
This page intentionally left blank.
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Appendix A Measuring LAN Reference Frequency Using a
Frequency Counter
A.1
Background
To comply with IEEE specifications for 10/100 Mbps and 10/100/1000Base-T Ethernet LAN, the
transmitter reference frequency must be correct and accurate within ±30 parts per million (ppm).
Most Intel LAN devices will operate properly with a 25.000 MHz reference crystal, provided it
meets the recommended requirements for frequency stability, equivalent series resistance at
resonance (ESR), and load capacitance.
Most circuits for series resonant crystals include two discrete capacitors (typically C1 and C2),
with values between 5 pF and 36 pF.
The most accurate way to determine the appropriate value for the discrete capacitors is to install the
approximately correct values for C1 and C2. Next, a frequency counter should be used to measure
the transmitter reference frequency (or transmitter reference clock).
• If the transmitter reference frequency is more than 20 ppm below the target frequency, then the
values for C1 and C2 are too big and should be decreased.
• If the transmitter reference frequency is more than 20 ppm above the target frequency, then the
values for C1 and C2 are too small and should be increased.
This Appendix provides instructions and illustrations that explain how to use a frequency counter
and probe to determine the Ethernet LAN device transmit center frequency. An example describing
how to calculate the frequency accuracy of the measured and averaged center frequency with
respect to the target center frequency is also included.
A.2
Required Test Equipment
•
•
•
•
•
Tektronix CMC-251, or similar high resolution, digital counter
Tektronix P6246, or similar high bandwidth, low capacitance (less than 1 pF) probe
Tektronix 1103, or similar probe power supply or probe amplifier
BNC, 50 Ω coaxial cable (less than 6 feet long)
System with power supply and test software for the LAN circuit to be tested
Application Note (AP-414)
41
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
A.3
Indirect Probing Method
The indirect probing test method is applicable foremost devices that support 100BASE-T. Since
probe capacitance can load the reference crystal and affect the measured frequency, the preferred
method is to use the indirect probing test method when possible.
Almost all Intel LAN silicon that support 1000BASE-T Ethernet can provide a buffered 125 MHz
clock, which can be used for indirect probing of the transmitter reference clock. The buffered 125
MHz clock will be a 5X multiple of the crystal circuit’s reference frequency (Figure 13).
Different LAN devices may require different register settings, to enable the buffered 125 MHz
reference frequency. Please obtain the settings or instructions that are appropriate for the LAN
controller you are using.
LAN Silicon IEEE Test Out +
2-pin
header
P6246 or similar
high impedance
probe
with less than 1 pF
input
Ch.1
input
Ch.2
LAN Silicon IEEE Test Out -
Tektronix
1103
Probe
Power Supply
50 ohm Coaxial
Cable
50 ohm
input
125.00047
Tektronix CMC251
or a similar capability
Frequency Counter
Figure 13. Indirect Probing Setup
42
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
A.4
Indirect Frequency Measurement and Frequency Accuracy
Calculation Steps
1. Make sure the system BIOS has the LAN controller enabled.
2. Connect the test equipment as shown in Figure 13.
3. Using the appropriate controls for your model of high resolution digital counter, make sure it
can display ~125.0000 MHz with at least four decimal places frequency resolution.
4. Enable the 125 MHz buffered reference clock.
5. Determine the center reference frequency as accurately as possible. This can be done by taking
30 to 50 different readings using the frequency counter and then calculating the average results
of the readings.
6. Calculate the accuracy of the measured and averaged center frequency with respect to an ideal
125.0000 MHz reference frequency.
(x – y)
FrequencyAccuracy ( ppm ) = -------------------------------( y ⁄ 1000000 )
where
x = Average measured frequency in Hertz and
y = Ideal reference frequency in Hertz
Example 1.
Given: The measured averaged center frequency is 124.99942 MHz (or 124,999,420 Hertz).
( 124999420 – 125000000 )
FrequencyAccuracy ( ppm ) = ---------------------------------------------------------------- = – 4.64ppm
( 125000000 ⁄ 1000000 )
Application Note (AP-414)
43
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Example 2.
Given: The measured averaged center frequency is 125.00087 MHz (or 125,000,870 Hertz).
( 125000870 – 125000000 )
FrequencyAccuracy ( ppm ) = ---------------------------------------------------------------- = 6.96ppm
( 125000000 ⁄ 1000000 )
Note:
The following items should be noted for an ideal reference crystal on a typical printed circuit
board.
• If the transmitter reference frequency is more than 8 ppm below the target frequency, then the
values for C1 and C2 are too big and they should be decreased. When tests are performed
across temperature, it may be acceptable for the center frequency deviation to be a little greater
than 8 ppm.
• If the transmitter reference frequency is more than 8 ppm above the target frequency, then the
values for C1 and C2 are too small and they should be increased. When tests are performed
across temperature, it may be acceptable for the center frequency deviation to be a little greater
than 8 ppm.
A.5
Direct Probing Test Method, Applicable for Most 10/100
Devices (Devices that do NOT support 1000Base-T)
Because probe capacitance can load the reference crystal affecting the measured frequency, it is
preferable to use a probe with less than 1 pF capacitance.
The probe should be connected between the X2 (or Xout) pin of the LAN device and a nearby
ground. Typically, it is possible to connect the probe pins across one of the discrete load capacitors
(C2 in Figure 14).
44
Application Note (AP-414)
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
Figure 14. Direct Probing Method
A.6
Direct Frequency Measurement and Frequency Accuracy
Calculation Steps
1. Make sure the system BIOS has the LAN controller enabled.
2. Connect the test equipment as shown in Figure 14.
3. Using the appropriate controls for your model of high resolution digital counter, make sure it
can display ~25.0000 MHz with at least four decimal places frequency resolution.
4. Ensure the LAN circuits are powered.
5. Determine the center reference frequency as accurately as possible. This can be done by taking
30 to 50 different readings using the frequency counter and then calculating the average results
of the readings.
6. Calculate the accuracy of the measured and averaged center frequency with respect to an ideal
25.0000 MHz reference frequency.
Application Note (AP-414)
45
82562G/GT and 82562ET/EM LAN on Motherboard Design Guide
(x – y)
FrequencyAccuracy ( ppm ) = -------------------------------( y ⁄ 1000000 )
where
x = Average measured frequency in Hertz and
y = Ideal reference frequency in Hertz
Example 3.
Given: The measured averaged center frequency is 24.99963 MHz (or 24,999,630 Hertz).
( 24999630 – 25000000 )
FrequencyAccuracy ( ppm ) = ---------------------------------------------------------- = – 14.8ppm
( 25000000 ⁄ 1000000 )
Example 4.
Given: The measured averaged center frequency is 25.00027 MHz (or 25,000,270 Hertz).
( 25000270 – 25000000 )
FrequencyAccuracy ( ppm ) = ---------------------------------------------------------- = 10.8ppm
( 25000000 ⁄ 1000000 )
Note:
The following items should be noted for an ideal reference crystal on a typical printed circuit
board.
• If the transmitter reference frequency is more than 8 ppm below the target frequency, then the
values for C1 and C2 are too big and they should be decreased. When tests are performed
across temperature, it may be acceptable for the center frequency deviation to be a little greater
than 8 ppm.
• If the transmitter reference frequency is more than 8 ppm above the target frequency, then the
values for C1 and C2 are too small and they should be increased. When tests are performed
across temperature, it may be acceptable for the center frequency deviation to be a little greater
than 8 ppm.
46
Application Note (AP-414)
">