MINIMIZING EMI EFFECTS DURING PCB LAYOUT OF Z8/Z8PLUS CIRCUITS

Transcription

1 APPLICATION NOTE MINIMIZING EMI EFFECTS DURING PCB LAYOUT OF Z8/Z8PLUS CIRCUITS INTRODUCTION The Z8/Z8Plus families have redefined ease-of-use by being the simplest 8-bit microcontrollers to program. Combined with low-cost and extensive device variety, a complete solution is easily implemented. PCB designs using the Z8/Z8Plus must follow several layout guidelines. Although some high-frequency effects are covered, discussion has been limited to the following: The Z8/Z8Plus device operation at low frequency ranges (0-20 MHz) The use of fairly long signal rise times (10-20ns) The mechanical and thermal requirements of PCB boards are not covered but should be known and implemented in a design. The complexity of these circuits are fairly low. Complex and higher-frequency circuits are left to those users more knowledgeable in PCB layout. For a more indepth understanding of PCB layout, see the references at the end of this application note. Many PCB layout books and classes are also available. THE LAYOUT DESIGN PROCESS Creating Good Layouts To create a good layout, evaluate potential problems early in the design process. The goal is to reduce EMI effects from the layout design portion of the application design process. Most unwanted effects can be eliminated early in the layout design by following these guidelines, which are the focus of this application note. Guidelines For Reducing EMI In PCBs 1. Identify the quiet and noisy I/O portions of the circuit. 2. Implement a low impedance power and ground distribution network, and analyze them for possible radiated and susceptibility effects. 3. Plan for good EMI performance by minimizing shared impedance and routing signal paths directly over their return. 4. Minimize conductor inductance to decrease noise voltage swing. 5. Implement ESD and EFT protection during layout. These items are listed in order of importance and are interrelated. For example, implementing a good power and ground distribution network relies on its underlying impedance. Although each is interrelated, use these guidelines in sequence. For example, understanding the quiet and noisy portions of the circuit helps the user layout the power and ground network. NOISY VS. QUIET CIRCUIT AREAS Identifying Noisy Circuits In a typical application, there are noisy and quiet portions of a circuit. A good first step is to understand the noisy and quiet areas on the board. When this is known, the PCB designer can dedicate portions of the board for these circuits and implement noise reduction techniques. When referring to the terms noise or EMI (Electromagnetic Interference), it usually infers a transfer of unwanted signals into a circuit (Voltage or Current). AN Z8X1099 1

2 For EMI or electrical noise to interfere with the operations of a circuit, there has to be a SOURCE of interference, a RECEPTOR for the interference, and a PATH which couples the Source and Receptor. Figure 1 shows a graphical representation of the transfer of EMI. Conducted Source (Emitter) Coupling Path Victim (Receptor) Radiated Figure 1. Model of EMI This application note examines intra-system noise. Intrasystem noise occurs when the sources, victims, and coupling paths are entirely within one system, module, or PCB. Noise emissions can be conducted by power lines into systems or systems can conduct noise emissions onto power lines. Noise emissions can also radiate into the internal circuit space and internal circuits can also be susceptible to radiated noise. For example, a PCB ground loop makes an antenna that effects other portions of the circuit. As illustrated in Figure 1, radiated noise can be coupled into a system and appear as conducted noise. This noise causes logic gates to trip at the wrong voltage level or sensitive analog circuits to have incorrect voltage levels. Two main coupling mechanisms from parallel conductors on the PCB board can increase noise. Parallel conductors can couple a signal onto each other if the signal on one conductor is a time-varying signal. (A time-varying signal has electromagnetic fields that can couple on the other conductor as defined in Maxwell s equations). The conductors are not physically connected but are electromagnetically connected, this is known as the transmission line effect. On the Schematic a capacitor or transformer appears to be connected between the two conductors. In Figure 2, the voltage is coupled to the other parallel conductor by mutual inductance, which appears as a wound transformer. Figure 2. Circuit Model for Inductive Coupling Figure 3. Circuit Model for Capacitive Coupling 2 AN Z8X1099

3 Figure 3 demonstrates stray capacitance. Stray capacitance results from capacitance between conductors that are in close proximity. As the application frequency and rise time increase, the parameter model describes inductive and capacitive coupling (See Figure 4). R L C G C G R L Figure 4. Transmission Line Model The two modes of interference are: differential-mode interference and common-mode interference. Differential-mode is desirable and common-mode is an EMI problem. Figure 5 shows a differential-mode signal. The fields generated by differential currents oppose each other and nearly cancel out; therefore, little interference is caused. IDM VDM Differential Mode Source Load IDM Figure 5. Differential Mode Interference with Canceling Currents In Figure 6, the common mode source adds noise to the differential mode signals. This noise is usually coupled from high-frequency currents affecting the PCB and wiring inductance, causing the wiring to operate as a radiating mono-pole antenna. These common mode signals are not useful, and are the major cause of radiated EMI from cables, PCB traces, and wiring. The wiring inductance is a significant problem and must be tightly controlled. A major source of common mode noise is clocks and repetitive I/O. Figure 7 shows the resulting peak current from a clock source. This peak current may be coupled onto adjacent conductors because it is a time-varying field. CMOS logic has a low average current but high peak currents with a high frequency repetition rate. AN Z8X1099 3

4 1/2 VDM L wiring Load VCM Common Mode Source 1/2 VDM L wiring Figure 6. Common Mode Interference with Increased Noise Voltage Repetitive CMOS Signal or Clock Resultant current 8 V + I Time Time Figure 7. Resulting Current from a CMOS Clock or Repetitive I/O Having the basic understanding of how EMI can be coupled, its paths, and its conduction modes, several circuit areas are now suspect and should be examined during layout. Some of the circuitry to be examined are listed below with placement suggestions 1 : Separate Digital Interface circuitry (higher speed, busses) from I/O circuitry (lower speed). Physically isolate and route on separate connectors when possible. Locate oscillators and clock circuits near the center of the printed circuit board. This location minimizes coupling to I/O runs and places the higher-frequency sources in the center of the power and ground distribution system. Locate memory circuits away from I/O circuits and each respective run, preferably near the center of the printed circuit board. These circuits draw high current transients during switching. Separate the analog from the digital portions of the circuit. Coupling may occur from the digital portions to analog lines, increasing noise. Place the microcontroller clock first on the circuit board. At low frequency, the microcontroller clock is one of the nosiest areas of the circuit board. If a clock run is added to drive other portions of a two-sided board, follow these guidelines: Add a ground run shadow to the backside (opposite) of the board. This is the most effective noise-reduction method. Where this is not possible, the ground run should be adjacent to the circuit board on the same side. Where the clock run is adjacent, a second ground is recommended, causing clock runs between two ground runs. When the noisy and quiet areas are identified, partition them on the circuit board to reduce the coupled noise. 4 AN Z8X1099

5 POWER AND GROUND DISTRIBUTION Power and Ground Routing Separating planes for power and ground distribution is the most effective routing method. This requires a multi-layer board. Power and ground planes almost become one at high frequencies. When not using planes, follow this rule: the closer the ground is to the power, the less EMI noise is created. Power traces should be run as close as possible to the ground traces. Power/Ground type effectiveness by layer is listed in Table 1. Table 1. Power/Ground Layers Ranked by Effectiveness (Higher Number = Worse) Increasing Inductance (L) Effectiveness Rank Description Lowest L 1 Multi-layer (V CC Plane and GND Plane). 2 2-sided (V CC trace over GND Plane). 3 2-sided (V CC trace over GND Trace). 4 1-sided (V CC trace parallel to GND Trace) Highest L 5 Random wiring loop The importance of proximity of the power and ground traces is illustrated in Table 1. Route the power and ground traces as close as possible. On a single-layer board, the return path should be routed side-by-side with the power. Decoupling Power The board power supply connection needs to be decoupled and must also have decoupling capacitors for each digital device. The digital device capacitors provide two primary functions: (1) supply sufficient switching transient current, preventing power supply droop, and (2) decouple conducted noise out of the system. These guidelines should be followed in decoupling power: For power and ground distribution, it is recommended that the incoming power and ground signals terminate at the input decoupling network at the printed circuit board connector. This termination should occur prior to connecting to the respective internal planes, which usually happens at the printed circuit board connector. Decouple power by using a 0.1 to 1.0µF Tantalum capacitor. This capacitor essentially bypasses highfrequency noise to ground Minimize the impedance and radiation loop of the coupling capacitor by placing each adjacent to the critical circuit. Because of long capacitor lead lengths, capacitors can become self-resonant at higher frequencies. Shorten capacitor leads and place capacitors as close to the board as possible, preventing self-resonance. Place adequate power-to-ground decoupling capacitors throughout individual digital devices. A standard value for these capacitors is 0.1µF for each device. If more accuracy is needed, the value can be calculated from this simple formula: dv I = C C = I dt dt dv For example, if the maximum V CC droop that is tolerable is 0.1V, the switching time is 4nS, and the current that needs to be supplied is 750mA, then the following formula applies: 4nS C = 750 ma = 30nF 0.1V This equation illustrates that a sufficient value for a standard value decoupling capacitor is 0.047µF or greater. Example Power/Ground Networks The PCB industry document that provides standards for PCB s and PCB assembly is the ANSI/IPC-D This document was created by the Institute for Interconnecting And Packaging Electronic Circuits and contains a section on power and ground distribution. Figures 8 10 are from this publication and are examples of power/ground layouts. Figure 8 is the worst layout, and Figure 10 is the best. Figure 8 shows adjacent signal return paths and high inductance that leads to crosstalk. Figure 9 shows a better layout that 2. Design Standard for Rigid Printed Boards and Rigid Printed Board Assemblies, ANSI/IPC-D-275, September 1991, The Institute for interconnecting and Packaging electronic circuits, Lincolnwood, Ill. AN Z8X1099 5

6 further reduces power distribution, logic-return impedances, conductor crosstalk, and board radiation. Figure 10 illustrates the most effective layout for EMI reduction. However, it shows the trade-off between the number of adjacent returns and the area of layout. Figure 8. Poor Voltage/Ground Distribution Layout Concept (From ANSI/IPC-D-275) Figure 9. Acceptable Voltage/Ground Distribution Layout Concept (From ANSI/IPC-D-275) 6 AN Z8X1099

7 Figure 10. Preferred Voltage/Ground Distribution Layout Concept (From ANSI/IPC-D-275) Minimizing Power and Ground Network Impedance A critical parameter to observe while laying out the power and ground network (along with signal runs) is the characteristic impedance of the conductor pairs. In most layouts, three configurations of the conductors are used: parallel strips, strips over ground plane, and strips side-by-side. Table 2 shows the impedance of each configuration and a a cross-section of the board, looking into the conductors. The impedance varies between the parallel strips and strip over ground plane compared to side-by-side configurations. causes unwanted noise when a side-by-side configuration is used for a long run on a board and the impedance is not carefully watched. The type of material used in board manufacturing can minimize conductor pair impedance. This directly effects the characteristic impedance because of the different ε R of the material where ε R is the dielectric constant of the material. Two of the three conductor configurations in Table 2 can be effected by the material used in the manufacture of the PCB board. This is seen more clearly in Table 2, where the characteristic impedance calculation equations are shown for the three impedances. Z Z Z 377 h = where W > 3h, h 3t ε W R 377 h = where W 3h ε W R 377 D 2 = ln + D 1 where W >> t ε W R 01 > 02 > 03 AN Z8X1099 7

8 It is important to know the ε R properties of the material used in board manufacturing to understand the impedance variations. The characteristic impedance must be tightly controlled to keep noise margins at a satisfactory level.moreover, the characteristic impedance can vary widely during manufacturing. A significant voltage level transient can be generated from a relatively high impedance. For example, examine a power bus using a side-by-side conductor routing method and TTL logic. Using the 25Ω (or higher) impedance, and knowing that TTL logic requires a current of approximately 16mA, means that dv=0.016 X 25Ω = 400 mv. This 400mV is equal to the noise immunity level of the TTL logic. Always determine if manufacturing can meet your design goals. Table 2. Characteristic Impedance of Different Conductor Pairs W D t W h h t W Z 01 Z 02 Z 03 W/h or D/W Parallel Strips Strips Over Ground Plane Strips Side by Side N/A N/A N/A N/A N/A AN Z8X1099

9 PLAN FOR GOOD EMI PERFORMANCE Application Note Minimizing Shared Impedance A common circuit problem is shared impedance. This contributes to incorrect voltage levels. Shared impedance increases the noise sensitivity from transient switching current or radiated EMI. For example, the effective inductance from the power connector to the chip power has a specific inductance, but the inductance through the same connection to the I/O can be different. It is this inductance that causes voltage variations along this connection and also causes a voltage reference at one point to be different from another point. See Figure 11. L1 L2 Power Connector (VCC) Vcc R "Shared Impedance" Z8/Z8+ I/O NPN Gnd Ground Connection (GND) L3 L4 Figure 11. Characteristic Impedance of Different Conductor Pairs a a. Gerald L. Ginsberg, Printed Circuits Design, pp. 82 As shown in Figure 11, the ground at the chip can be different from the ground at the emitter of the NPN BJT. The same is true for the chip power. A more effective configuration is shown in Figure 12. A common connection point has reduced shared impedance. This connection scheme can reduce shared impedance and still allow large line inductance values. Controlling line inductance is described later in this document. Power Connector (VCC) Vcc R Z8/Z8+ I/O NPN Gnd Ground Connection (GND) Figure 12. Better Connection to Reduce Shared Impedance AN Z8X1099 9

10 JP1 JP2 2 1 HEADER 1 POWER 2 1 HEADER 2 Input Output C4 J1 1 2 HF_FILTER J3 2 1 C3 HF_FILTER ESD ISLAND C5 C1 C2 1 OUTPUT ISLAND 2 1 U1A RC_OR_FERRITE C6 Y1 J4 RESONATOR RC_OR_FERRITE J2 DIGITAL ISLAND U P24 P P25 P P26 P P27 Z86E08 P VCC GND 13 7 XTAL2 P XTAL1 P P31 P00 10 P32 P33 R1 RESISTOR 2 JP3 2 1 C U3A 3 HEADER 3 OP09 ANALOG ISLAND 7 Figure 13. Schematic for Example PCB Board Using a Star Ground and Islands Using a dedicated ground run for each path reduces some EMI problems. This is difficult to implement, therefore designers need an additional step to create a surrounding ground plane. This ground plane is used to surround and isolate noisy circuit parts. This is effective on single-sided PCBs, but it is more effective as the layers increase; then a true, continuous ground plane becomes possible. In boards with two or more layers, this continuous ground plane can be further divided into partitioned islands with the ground connections from each island joined at a star ground. This reduces the return impedance and allows for adjacent routing of the signal and return paths. See Figure 14 for an example of a 2-layer board using a Z8. The bottom layer is used for ground islands and the top layer is the routing layer and component side. Figure 13 is the schematic for Figure 14. The high-frequency filters and RC/Ferrite beads are used in various parts of the circuit, preventing noise from entering one part of the board from another. The four islands are: ESD, Digital, Analog, and Output. The arrows on the PCB board in Figure 14 indicate the return current flow from the four islands. The side of JP2, which does not have a trace, is connected to the ground plane. Note the return current is separated into pathways returning to ground. Checklist For Improved EMI Performance The following checklist helps the PCB designer resolve most EMI design problems. Segregate digital circuits and analog circuits. Follow common impedance layout procedures when planning grounding and power distribution. Connect the oscillator directly to the Z8/Z8Plus GND pin, using a short, direct trace. Do not use a shared trace. Use a ceramic-bypass capacitor (.01 to 0.1µF) at the Z8/Z8Plus s VCC and GND pin connection. Use short leads and short traces. Locate electrolytic capacitors on VCC at the power connector before splitting analog and digital VCC. Assign each digital IC its own decoupling capacitor, and place them in close proximity. Separate digital and analog functions in external packages whenever possible. Use short traces and small loops for driven digital outputs. Add filtering for noisy repetitive output signals. Use a series damping resistor (22 to 47Ω) or inductor placed at the output pin. 10 AN Z8X1099

11 Use EMI ferrite beads to replace less effective devices such as series R or L. This reduces I/O signal interference. Use beads specifically designed for EMI suppression, placing output signal beads at the driving pin, and input beads at the input connector. Locate pull-up resistors at the corresponding signal driving output pin, not at the input pin. This minimizes loop area. Use small loop areas for good ESD and external EMI immunity. This minimizes ESD ground input problems. Locate an ESD ground at the I/O connector with an ideal length-to-width ratio of 3:1. Do not exceed a 5:1 ratio. Terminate the ESD ground to the chassis ground. If no chassis ground exists, terminate the ESD ground to the power input ground at the connector. Use a 1-10nF decoupling capacitor right at the device connector. TConnect the ground to ESD ground. Use a series R device to limit EDS current Use ESD techniques for improved OTP-mode pin operation: Minimize circuit loop areas and provide diode clamps to VCC. Place a clamping diode on the Z8/Z8Plus, EPM, OE, CE and VPP. Place these diodes close to the Z8 to reduce induced noise. Verify correct pin placement by checking pin diagram in the product specification. Terminate unused inputs. This reduces noise coupling that affects device performance. AN Z8X

12 Digital Island Output Island Analog Island ESD Island Figure 14. Sample PCB Board From Circuit Schematic 12 AN Z8X1099

13 MINIMIZING LINE INDUCTANCE Understanding Parasitic L Controlling trace inductance (L) is critical in reducing noise voltage swing. In Figure 15, parasitic L is measured by varying connections and trace widths. This experiment setup is used in several designs and shows the differences in traces and connections. Figure 15. Parasitic L Measurement Setup a a. Gary Cummings, System EMI, ESD & EFT Workshop, December 1997 Figure 15 illustrates: The connection between C and D simulates a capacitor with 0 internal inductance, connected on a 2-sided PCB. Measurements are made with a di/dt generator. I=0 to 40A and di/dt rate is 100A / second. Measuring induced V L between A to B and C to D permits calculation of L= V L / (di/dt). PCB Signal Routing Effects Inductance The designs examined using the experiment setup described in Figure 15 are shown in Figure 16. In this figure, the trace widths, trace placements, and connections have been varied to show the varying effects of inductance on the layout design. a. IBID Figure 16. Different Designs Used in Measuring Parasitic Inductance a AN Z8X

14 Several conclusions can be made from the designs: Compare a & b. Orienting capacitors to current flow reduces inductance. Compare b & c. Multiple links have less L than one link between traces. Compare d & e. For lowest L, a signal track must be aligned above its return track on the opposite side. This is an example of how well ground planes work. Compare c & e. Decrease local di/dt density & L by enlarging copper tracks. These experiment conclusions can aid the designer in decreasing the parasitic inductance of traces. OTHER EMI PROTECTION Understanding ESD And EFT Consider two other EMI problems during the layout of the PCB board, ESD (Electro-Static Discharge), and EFT (Electrical Fast Transient). ESD (Electro-Static Discharge) is a circuit phenomenon that occurs in two ways: direct discharge and indirect discharge. Direct discharge occurs when a human finger touches exposed conductors. Indirect discharge causes an ESD malfunction when a nearby ESD event radiates energy, which couples into the system. EDS events usually have: Voltage levels of 2,000-15,000V Peak currents of 10-30A Discharge current rise time of (t r ) of 1-3nS ESD frequency of MHz. Because of these characteristics, high frequency design techniques are essential for good ESD immunity. EFT (Electrical Fast Transient) are upsets caused by power line noise bursts (due to motors), relay contact arcing (due to switching inductive loads), and any switching of a inductive load. EFT is different from ESD because the noise originates from the power line that supplies the on-board devices. EFT noise enters a system in two ways: radiated upset or conducted upset. Radiated upset is the proximity of a power line and a coupled signal. Conducted upset is power-line noise being conducted to sensitive areas of the circuit. ESD Direct Discharge Into Circuit As explained above, direct discharge is typical of a charged human coming in contact with exposed conductors. During layout, examine the PCB board for any possibility of exposed conductors. Exposed conductors should be protected. Areas to examine: Battery and Power Supply Contacts Switches, Buttons, and membrane keypads LED leads and speaker leads Metal screws too close to circuitry Signal I/O connectors and cables PCB conductors near edge of board Exposed conductors Conductors close to openings or seams in the product housing. ESD easily enters when the gap from the probe to a conductor is too small. To prevent direct discharge ESD, take these steps; they are listed in order of importance: Prevent ESD by using physical separation such as air gaps or dielectric barriers Bypass capacitors on I/O to absorb ESD at entry point. Place these capacitors at the connector interface. Place separate ESD ground connected to chassis ground (best) or input power ground at power connector. Place series resistance on I/O lines (100Ω to 1000Ω) to limit ESD peak current Pay special attention to critical Z8 circuits oscillator, OTP pins, and interrupt inputs by ensuring small circuit area and clamping diodes to VCC Use ESD I/O filters with series ferrite bead L and ceramic C to Ground Use continuous metal shields Group the protected I/O pins together, and use a large ESD ground for ceramic bypass capacitors. Use copper length-to-width ratio of 5:1 or less for minimum L. See Figure 17 for a graphical representation of a PCB case and possible ESD paths. See Figure 18 for a sample layout method to prevent ESD discharge. 14 AN Z8X1099

15 Figure 17. Suggested ESD Barriers for PCB Cases Figure 18. Layout Methods to Stop Direct ESD Discharge AN Z8X

16 ESD Indirect Discharge Into Circuit Indirect Discharge is caused by a radiated upset, and this event is caused in two ways: Pickup occurs in a connected I/O device or peripheral (display, plugged-in I/O cable, etc.) which is then conducted into the product to cause upset or Pickup occurs within the product itself. For example, an oscillator with a long ground return path to the microcontroller ground pin. To prevent Indirect Discharge into a product, reduce the circuit loop areas, ensuring low inductance grounding and signal routing. Voltage is induced easily on larger circuit loops. Table 4 shows the effects of loop area on induced voltages. Note that 10 cm 2 is not an overly large loop area but the effects are large! Table 3. Effects of Loop Area on Induced Voltage Loop Area Induced Voltage 1 cm 2 2 Volts 5 cm 2 10 volts 10 cm 2 20 Volts Figure 19 is an example of a large circuit loop, causing large induced voltages. By re-routing the power and ground lines to the Z8, the new loop area is significantly reduced and is shown in Figure cm 14 cm GND +5V 10µF Power Cap VCC Z8 GND 7 cm 5 cm Enclosed Loop = (51*14)-(7*5) = 679 cm 2 Figure 19. Example of a Large Loop Area 16 AN Z8X1099

17 51 cm 0.2 cm 7 cm 14 cm GND +5V 10µF Power Cap Z8 VCC GND 7 cm 5 cm Enclosed Loop = (51*0.2)+(7*0.2)+(7*0.2) = 13.0 cm 2 Figure 20. Example of a Large Loop Area EFT Design Guidelines Follow these guidelines to reduce the effects of EFT noise: Use small MCU circuit loops to prevent radiated upset. Examine these circuits: the Z8 VCC/GND loop, the oscillator/gnd loop, and the external interrupt circuit loops. Separate the Z8 power distribution and ground loops from its low voltage circuitry, AC powered loads, and noisy switched loads, such as motors and relays. Do this when MCU is not isolated from AC mains Locate ceramic decoupling capacitor close to MCU pins. Add series ferrite bead between VCC source and MCU to dampen spikes. SUMMARY Implementing the guidelines in this application note improves the quality and reduces noise susceptibility in most PCB boards. Most problems are solved by using the simple design steps covered in the first part of this note. High-speed problems need to be more thoroughly examined than other parts of the circuit. 1 Gerald L. Ginsberg, Printed Circuits Design, pp ,85 2 Design Standard for Rigid Printed Boards and Rigid Printed Board Assemblies, ANSI/IPC-D-275, September 1991, The Institute for interconnecting and Packaging electronic circuits, Lincolnwood, Ill. 3 Gerald L. Ginsberg, Printed Circuits Design, pp Gary Cummings, System EMI, ESD & EFT Workshop, December IBID AN Z8X

18 Information Integrity The information contained within this document has been verified according to the general principles of electrical and mechanical engineering. Any applicable source code illustrated in the document was either written by an authorized ZiLOG employee or licensed consultant. Permission to use these codes in any form, besides the intended application, must be approved through a license agreement between both parties. ZiLOG will not be responsible for any code(s) used beyond the intended application. Contact the local ZiLOG Sales Office to obtain necessary license agreements. Document Disclaimer 1999 by ZiLOG, Inc. All rights reserved. Information in this publication concerning the devices, applications, or technology described is intended to suggest possible uses and may be superseded. ZiLOG, INC. DOES NOT ASSUME LIABILITY FOR OR PROVIDE A REPRESENTATION OF ACCURACY OF THE INFORMATION, DEVICES, OR TECHNOLOGY DESCRIBED IN THIS DOCUMENT. ZiLOG ALSO DOES NOT ASSUME LIABILITY FOR INTELLECTUAL PROPERTY INFRINGEMENT RELATED IN ANY MANNER TO USE OF INFORMATION, DEVICES, OR TECHNOLOGY DESCRIBED HEREIN OR OTHERWISE. Except with the express written approval ZiLOG, use of information, devices, or technology as critical components of life support systems is not authorized. No licenses or other rights are conveyed, implicitly or otherwise, by this document under any intellectual property rights. 18 AN Z8X1099