Texas Instruments | TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation | Application notes | Texas Instruments TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation Application notes

Texas Instruments TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation Application notes
Application Report
SPRACG5 – May 2018
TI mmWave Radar sensor RF PCB Design, Manufacturing
and Validation Guide
Chethan Kumar Y.B., Anil Kumar KV, and Randy Rosales
ABSTRACT
This application report helps TI mmWave Radar sensor designers navigate the series of tasks and key
concerns when designing, manufacturing and validating a new mmWave sensor board. This document is
only concerned with the RF portions of the design. It is beneficial for PCB designers that do not have
experience with RF PCB design at mmWave frequencies. This document is applicable to sensor designs
using IWR/ AWR mmWave Radar chips.
1
2
3
4
5
6
Contents
Introduction ...................................................................................................................
RF PCB Selection and Fabrication .......................................................................................
Integrating the Antenna .....................................................................................................
Thermal Design ..............................................................................................................
Enclosures and Radome ....................................................................................................
References ...................................................................................................................
2
2
5
7
7
8
List of Figures
1
AWR1642 EVM Board Stackup ............................................................................................ 2
2
AWR1642 BGA to PCB Transition and GCPW Dimensions (drawing not to scale) ................................ 3
3
Example of Coupon Structure on the AWR1642 Booster Pack EVM
................................................
5
List of Tables
Trademarks
Teflon is a registered trademark of Chemours.
All other trademarks are the property of their respective owners.
SPRACG5 – May 2018
Submit Documentation Feedback
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
1
Introduction
1
www.ti.com
Introduction
The goal of this application report is to familiarize you with the hardware design aspects of the radar
system using TI Radar chips. However, depending on the application, sensor designers need to decide for
themselves how many of these steps and to what extent they are followed based on time available for
design/simulation, lab test time and sensor validation required.
Section 2 covers the aspects of PCB manufacturing concerns. This includes the selection of the RF PCB
material, discussion of the CAD to CAM RF design documentation, and how to evaluate PCB fabricators
for RF fabrication quality.
Section 3 covers the RF PCB design. Also, simulation flow and key concerns are discussed, which
includes a brief overview of the key antenna design requirements and how they map to the radar equation
budgets.
Section 4 covers thermal considerations, followed by enclosure and Radome design aspects.
2
RF PCB Selection and Fabrication
PCB fabrication concerns from the RF perspective are covered in this section. This includes a discussion
of CAD to CAM RF design documentation and how to evaluate PCB fabricators for RF fabrication quality.
The goal here is to describe the key points to bring up and align on with a selected PCB fabricator to
achieve the first pass success when fabricating the mmWave PCB.
2.1
PCB RF Design
This section discusses a typical PCB to Ball Grid Array (BGA) transition and Grounded Coplanar
Waveguide (GCPW) structures using the example of the AWR1642 EVM board. The BGA to PCB
transition in the EVM board is compatible with all of the 77 GHz mmWave sensor devices.
The above mentioned board was designed with RO4835 + FR4 hybrid stackup. It could also be designed
with a stackup using RO3003 or any other RF-friendly substrate.
The choice of the stackup is based on the tradeoff between electrical performance and substrate
availability and manufacturing yield. For example, the Rogers RO3003 stackup (along with rolled copper
foil) yields lower loss and better phase repeatability. Rogers RO4835 LoPro, on the other hand, has better
manufacturing yield while it has slightly inferior electrical properties.
2.1.1
PCB Stackup
This section discusses the PCB stackup of the sensor board. As an example, the AWR1642 EVM
BoosterPack board uses a hybrid stackup. Rogers RO4835 LoPro core is used between metal layers 1
and 2. The remaining layers 2 through 6 are etched on FR4 core and prepreg substrates. The stackup is
shown in Figure 1.
Figure 1. AWR1642 EVM Board Stackup
For RO3003 based boards, the stackup is the same as Figure 1 except that the RO4835 LoPro 4mil
substrate is replaced with RO3003 5mil substrate.
2
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
SPRACG5 – May 2018
Submit Documentation Feedback
RF PCB Selection and Fabrication
www.ti.com
2.1.2
Package to PCB transition
To get an optimal match between the device RF ball and PCB trace, the package to PCB transition layout
needs to be designed appropriately. TI has built Rogers-based EVM boards and recommends the
customer who uses Rogers materials, to use TI’s recommended transition. This transition allows the
package to match to a 50 Ω transmission line at the edge of the package (approximately 1.3 mm from the
center of the signal pad). If the customer chooses to use a different PCB substrate, the package to PCB
transition needs to be re-designed, which is beyond the scope of this application report.
Example:
Layout for an optimized AWR1642 BGA package to GCPW transition is shown below. These dimensions
are for stackups based on Rogers PCB substrates.
The 77 GHz TX/RX signal pads and signal traces are surrounded by continuous reference ground plane
on L1 and ground reference on L2. Three ground-stitching (L1-L2 ground) micro-vias are via-in-pad with
the surrounding AWR1642 BGA ground pads. There are four additional ground-stitching micro-vias that
are placed just outside the ground plane keep out radius of the signal pad. There is a circular ground
plane cutout placed underneath the RF signal pad on L2 that provides right impedance matching.
Together, with the anti-pad separation, these radial ground vias and L2 ground plane cutout, smoothly
transition the package BGA impedance to the GCPW PCB impedance around the AWR1642 RF operating
bands.
F/2
SIG
E
VSS
Ground Pad
x
330 um BGA pad diameter
VSS
VSS
L1 to L2, ground, microvia in pad
x
150 um drill diameter
x
300 um via L1 pad diameter
x
330 um BGA pad diameter
E
L2 'E Z}o
E
B C
xx
xxxx
xxxxxx
VSS
VSS
A/2
G
VSS
E
L1 to L2, ground, microvia
x
150 um drill diameter
x
300 um via L1 pad diameter
L1 o Πv
D = 525 um
E = 650 um
F = 900 um
G = 780 um
H = 800 um
J = 400 um
F
Signal Pad (TX or RX pad)
x
330 um BGA pad diameter
G/2
VSS
SIG
VSS
VSS
D
D
] [,[
A
RO3003
A = 717 um
B = 213 um
C = 102 um
RO4835
A = 871 um
B = 180 um
C = 171 um
] [:[
Figure 2. AWR1642 BGA to PCB Transition and GCPW Dimensions (drawing not to scale)
Note that dimensions A, B and C are different for the RO3003 stackup and the RO4835 LoPro stackup as
shown in Figure 2.
2.2
Assessing PCB Fabricator Experience With RF Substrates
Designers should discuss with their PCB vendor the vendor’s experience with fabricating PCB with highfrequency substrates. PCB substrate fabrication documentation covers material storage, handling, and
processing techniques. All of these recommendations must be followed to achieve consistent performance
when utilizing these materials. For details of fabrication using Rogers materials, see [1] and [2].
Sequential lamination of RF and non-RF substrate core and pre-preg material is typically required for
completing RF designs such as the BoosterPack EVM. Designers should discuss with their PCB vendor
the vendor’s experience and capabilities when fabricating mixed material hybrid stackups. Different core
and pre-preg materials typically have different curing requirements and procedures and may not always be
compatible.
2.3
Material Properties and Manufacturing Tolerances Affecting Critical RF Performance
RF signal paths exhibit high sensitivity to small geometry changes such as:
SPRACG5 – May 2018
Submit Documentation Feedback
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
3
RF PCB Selection and Fabrication
•
•
•
•
•
•
•
•
•
•
www.ti.com
Substrate thickness
Metal thickness
Metal roughness
Plating
Via placement tolerance
Etch tolerances (LDI vs. LPI masks)
Air gap tolerances
Solder-mask tolerance (LDI vs. LPI accuracy)
Sequential stack-up layer registration
Peel strength vs plating height
Substrate thickness directly determines performance of the RF structures. RO4835 LoPro and RO3003
substrates should maintain their designed thicknesses as received from Rogers. However, improper
handling or fabrication steps can damage these substrates causing delamination and other adverse
effects that will severely impair any RF structure performance.
Overall etch tolerances must be controlled so that the line widths, air gaps and planar antenna structures
stay close to their designed dimensions. TI recommends using the Laser Direct Imaging (LDI) etch-mask
over the more common Liquid Photoimageable (LPI) etch-mask because LDI enables fabrication with
tighter tolerances.
Solder-mask has different dielectric properties compared to the RF substrate and the free-space
surrounding the PCB. Solder-mask should typically be avoided over the RF transmission lines and
antenna. In the case of solder-mask near the RF BGA, it is critical that the solder-mask registration and
thickness must be tightly controlled. Changes in thickness or registration can have an effect on variability
of RF performance from PCB to PCB.
Plating affects RF characteristics. Most common plating used in industry, Electroless Nickel-Immersion
Gold (ENIG), is not a good choice for mmWave boards due to its high losses. TI EVM uses immersion
silver plating that has lesser loss, comparatively. However, immersion silver is susceptible to oxidation on
prolonged exposure to air. This oxidation does not impact the RF performance. However, proper storage
of the PCB is recommended to reduce the oxidation. Over and under plating of top-layer copper can result
in phase and loss/reflection variations.
Number of types of vias determines the PCB process complexity. Higher number of types of vias typically
causes higher processing steps, which uses sequential lamination and can cause via registration error.
They also increase the PCB cost and lowers yield. Therefore, it is desirable to keep via types to a
minimum. TI mmWave BoosterPack designs use two types of vias.
Multiple types of via processing also increases the plating thickness. Thicker plating on traces that have
narrow widths causes the peel strength to be poorer. Thicker top layer geometry also has higher coupling
between the antenna elements, which is undesirable. Therefore, it is recommended to keep the top layer
metal plus plating thickness low. TI mmWave BoosterPack designs use a 0.5 oz base copper on the top
layer as shown in Figure 1.
The copper lamination will be of difference kinds. Rolled copper offers the lowest surface roughness and
the lowest loss. Electro-deposited (ED) copper has relatively higher roughness and loss.
The placement error on ground vias around the transmission line have detrimental impact on its
characteristics such as its impedance and bandwidth. Typically, in manufacturing, the via placement errors
can have different offsets in x and y-directions. Therefore, the impact on transmission lines or antenna
structures that are aligned to x-axis and y-axis can exhibit different characteristics.
There are many via-s on the PCB that are either on the pads or close to pads. These are filled with nonconductive epoxy and capped with copper plating to ensure flat surface.
4
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
SPRACG5 – May 2018
Submit Documentation Feedback
RF PCB Selection and Fabrication
www.ti.com
2.3.1
Determining Absolute Tolerance Limits
Absolute tolerance limits on each dimension and placement can only be derived from margin studies using
RF simulators and EM theory. The process involves sweeping various parameters, through tolerance limit
specified by the PCB manufacturer and determining how the parameter changes effects the performance
of the structure. For example, designers can simulate with different air gaps, via placement distances, line
widths and see the resulting change in GCPW impedance or antenna gain or directionality. Such studies
are beyond the scope of this application report.
2.4
RF Critical CAD to CAM Documentation and Verification
Designers are encouraged to clearly document the areas of the PCB that are RF design critical along with
the intended design dimensions for each of these locations. Controlled impedance trace dimensions and
stack-up thicknesses for high-speed digital signals are typically dictated and verified by a PCB fabricator.
However, RF design dimensions should be dictated completely by the PCB designer and verified after
fabrication.
In the case of these mmWave sensor designs, the areas around the RF signal BGA footprints, the RF
signal transmission-lines and the antennas must be carefully drilled and etched. Ideally, the tooling error
must be constrained to zero-mean error around the designed dimension. Typical PCB fabrication error
results in a low variance skew in one direction of the tolerance window. PCB designers need to discuss
methods with their fabricator for bringing this skew as close as possible to the designed dimensions.
It is recommended that PCB designers explicitly ask for a small sample run of PCB to be used for process
inspection purposes. Any problems meeting critical RF design dimensions can be dealt with before
proceeding to larger volume production. This process can be repeated until the zero-mean error between
fabricated and designed dimensions are achieved.
A report of critical RF design dimensions should be presented to the PCB fabricator as part of the the PCB
CAD and CAM board design documents and files. The PCB fabricator should be explicitly asked to verify
what the expected tolerances are going to be for each of the critical dimensions. It is recommended to
provide the RF coupon structure on the PCB/Panel. This helps in assessment of material property,
fabrication parameters etching tolerances, manufacturability variations in impedance, and so forth.
For example, AWR1642 BoosterPack EVM has transmission line coupon structures for probe as shown in
Figure 3.
Figure 3. Example of Coupon Structure on the AWR1642 Booster Pack EVM
3
Integrating the Antenna
This section is a brief overview of key antenna design requirements and how they map to radar equation
budgets and FMCW radar processing. This also includes a discussion on how to best re-use the
BoosterPack EVM designs with custom etched antenna.
Knowledge of basic antenna metrics is necessary for an mmWave sensor designer to understand the
antenna performance requirements needed for their sensor.
SPRACG5 – May 2018
Submit Documentation Feedback
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
5
Integrating the Antenna
3.1
www.ti.com
Radar Equation and Link Budgeting
All FMCW mmWave sensors work on the underlying principle that a transmitting antenna can radiate out
an RF “Chirp” signal and an associated receiver antenna can detect the resulting chirp echo reflected from
a target. The received chirp reflection is mixed with the transmitted chirp and the resulting IF signal is
sampled to determine range, angle and velocity of the target. Programming Chirp Parameters in TI Radar
Devices [4] covers the process of how to combine with proper chirp configurations.
If too little energy is radiated from the transmit antenna, or too little energy is incident to the target, or too
little energy is incident to the receive antenna, the sensor ADC will not have enough IF amplitude to
resolve the target above the noise floor and target detection will fail. Significant signal to noise ratio, or
SNR, is required to resolve the target in the resulting IF FFT spectrum.
All of these parameters are combined in the “Radar Equation” to help designers perform a radio link
budget analysis. For details of the link budget analysis, see [4].
The Radar equation that gives the range of a target is shown in Equation 1.
Range MAX = 4
PTX ´ DRX ´ DTX ´ c 2 ´ sT arg et ´ NChirps ´ TR
fC2 ´ (4p)3 ´ kT ´ NF ´ SNRdet ect
(1)
where:
• PTX: The transmitted output power, incident to the antenna in Watts.
• DTX,DRX: The transmit and receive antenna directionality, respectively. This takes into account antenna
efficiency as well as directional gain – unit-less gain.
• c: Speed of light in free-space in meters/second.
• σTarget: The radar cross section (RCS), which is a unit-less gain factor relating incident power to
reflected power of a target object.
• fC: Means frequency of the chirp ramp in Hz.
• NChirps: Number of chirps in a chirp frame
• TR: Chirp ramp time in seconds
• k: Boltzman’s constant – 1.38 x 10-23 J/K
• T: Temperature in Kelvin
• NF: Is the Noise Factor of the receiver path. This coefficient takes into account the noise introduced by
the stages of the receive signal path like the low-noise amplifier (LNA), low-pass and high-pass filtering
and the ADC sampling.
• SNRdetect: Minimum signal to noise ratio for detection of the target. This is expressed in absolute ratio.
In terms of antenna and transmission-line design, there are only a few terms that can be optimized for the
radar equation: PTX, DTX and DRX. All of the other terms are determined by the chirp parameters, target,
environment or mmWave sensor device native performance.
The power delivered to the antenna, PTX, is a function of programmed transmit power backoff, PCB
transmission-line losses and transmission-line to antenna reflections and BGA to transmission-line
reflections. Maximizing PTX is the goal. Therefore, minimizing losses and reflections along the RF path to
the antenna and maximizing programmed transmit power is important. The mean chirp frequency, fC, is a
function of chirp configuration, but it should be taken into account during the antenna design phase if
possible so that the bandwidth of the antenna can be optimized around the intended chirp bandwidth.
Directivity DTX and DRX are entirely a function of the antenna design and transmission-line design.
3.2
Custom Antenna Design Options
Depending on the amount of experience with the mmWave RF design, mmWave sensor designers have a
few options when it comes to acquiring application-specific antennas. Starting with the requirements
derived from the sections above and constraints of the TI supported RF substrate stack-ups, designers
can:
• Create their own antenna
• Have a third-party RF design firm create an antenna
6
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
SPRACG5 – May 2018
Submit Documentation Feedback
Thermal Design
www.ti.com
•
Use one of the TI provided reference antenna designs
If a designer is familiar enough with the antenna design concepts and simulation tools, then the best way
to start a custom antenna design is to reference the TI mmWave Radar BoosterPack EVM boards. These
boards can serve as a reference RF layout design that can be extended to work with a custom designed
antenna.
The general flow is to assume the same layer-1 RF substrate of the stackup and then completely re-use
the BGA to PCB transition footprint and GCPW transmission-line RF fan-out. The custom antenna is then
designed and a transmission-line feed path can be laid out to interface the antenna to the GCPW fan-out
for best impedance and phase match to the antenna. The recommended process for third-party designers
is the same.
If one of the TI provided reference antenna meets the design requirements, then no re-design is
necessary and these can be integrated into the new design.
4
Thermal Design
This section discusses the thermal aspects of the system design. The need for effective heat dissipation is
to keep the die temperature within the operational and reliable limits. Some of the various ways to manage
heat dissipation from the Radar device are listed below:
• Limiting the chirp duty cycle and limiting the power dissipation in the device
• Using multiple copper layers in the board with large GND planes and having enough number of
thermal vias below the device directly connecting the device GND balls to the PCB GND planes
• Using heat-sink that touches the device top or bottom of the board, directly below the device
The thermal parameters of the device are provided in the device-specific data sheet. For more details on
the definition of these parameters and their use, see [3].
Thermal simulation of the sensor system with heat sink or enclosures is recommended during the
mechanical design of the system.
Heat-sink option: A very effective way to conduct heat away from device is to use heat-sink. The heatsink can be either on device side (top heat-sink) or on side opposite to the device (bottom heat-sink) or
both. In a simple form, the top heat-sink can be a sufficiently large metal piece that makes good thermal
contact with the device top. If the antenna is etched on the same side as the device, care should be taken
to see that the metal heat-sink does not distort the antenna characteristics. The bottom heat-sink is also a
piece of metal or protrusion from the enclosure that touches the board directly below the device on the
side of the PCB opposite to the device. While using bottom heat-sink, care should be taken to see that the
metal does not touch any capacitors or other components that may cause electrical short.
5
Enclosures and Radome
Radome is a cover or enclosure in order to protect Radar antennas from environmental influences. It
functions as a structural and weatherproof enclosure to the antenna in such a manner that it has least
interference with the transmission from it. It is derived from the expression Radar and Dome. Covers will
have some influence on the shape of radiation pattern or Field of view and achievable maximum distance.
Radars can see through plastic and glass of any color. While designing housing, pay attention to the
aspects being discussed in Section 5.1.1 and Section 5.1.2.
The objective of an efficient Radome design is to reduce reflections at its surface and transmit the signal
with minimum loss and beam distortion. For a general-purpose enclosure that covers the radiating side of
the sensor, the material should have a uniform thickness and must also have a good surface smoothness.
In some cases, a Radome could be constructed as a lens that alters the beam characteristics intentionally.
Such Radoms/lens need to be designed using electro-magnetic simulation tools in conjunction with the
antenna.
5.1
Guideline for Radome Design
Some key important parameters in a typical Radome design are its wall thickness and its distance to the
antenna.
SPRACG5 – May 2018
Submit Documentation Feedback
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
7
References
5.1.1
www.ti.com
Consideration for Radome Wall Thickness
Thickness of the Radome plays a key role in arriving at the optimum performance of the mmWave sensor.
Wavelength in the Radome becomes shorter in the material than in free air. The wavelength in the
material is a function of its dielectric constant. The goal is to make the wall thickness equal to the integer
multiple of the wavelength in the material. This is to make sure that the Radome becomes nearly
transparent for the mmWave signals.
t = n * lm / 2
(2)
where:
lm =
C
f ´ er
(3)
where:
• t: thickness of Radome wall
• n: 1,2,3…
• λm: wavelength in Radome material
• c: speed of light
• f : mean carrier frequency used
• εr: relative permittivity
Material with lower Dk and Df (dielectric constant and loss tangent) are recommended. Typical materials
used in Radome are Polycarbonate, Teflon® (PTFE), Polystyrene, and so forth. Typically, with Radome
and Antenna, simulations are done to see there is very little degradation in the Radiation pattern.
5.1.2
Consideration for Antenna to Radome Distance
The optimal distance between the antenna and the Radome helps to minimize the effects of reflections
caused by the Radome. These effects become minimal if the waves returned at the antenna are in phase
with the transmitted waves.
D = n.l0 / 2
(4)
where:
• n: 1,2,3…
• D: optimal distance between Radome and Antenna
• λ0: wavelength in air
6
References
1.
2.
3.
4.
8
RO3000® and RO3200™ Series High Frequency Laminates
RO4003C™/RO4350B™/RO4835™ Laminates Circuit Processing Guidelines
Semiconductor and IC Package Thermal Metrics
Programming Chirp Parameters in TI Radar Devices
TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation
Guide
Copyright © 2018, Texas Instruments Incorporated
SPRACG5 – May 2018
Submit Documentation Feedback
IMPORTANT NOTICE FOR TI DESIGN INFORMATION AND RESOURCES
Texas Instruments Incorporated (‘TI”) technical, application or other design advice, services or information, including, but not limited to,
reference designs and materials relating to evaluation modules, (collectively, “TI Resources”) are intended to assist designers who are
developing applications that incorporate TI products; by downloading, accessing or using any particular TI Resource in any way, you
(individually or, if you are acting on behalf of a company, your company) agree to use it solely for this purpose and subject to the terms of
this Notice.
TI’s provision of TI Resources does not expand or otherwise alter TI’s applicable published warranties or warranty disclaimers for TI
products, and no additional obligations or liabilities arise from TI providing such TI Resources. TI reserves the right to make corrections,
enhancements, improvements and other changes to its TI Resources.
You understand and agree that you remain responsible for using your independent analysis, evaluation and judgment in designing your
applications and that you have full and exclusive responsibility to assure the safety of your applications and compliance of your applications
(and of all TI products used in or for your applications) with all applicable regulations, laws and other applicable requirements. You
represent that, with respect to your applications, you have all the necessary expertise to create and implement safeguards that (1)
anticipate dangerous consequences of failures, (2) monitor failures and their consequences, and (3) lessen the likelihood of failures that
might cause harm and take appropriate actions. You agree that prior to using or distributing any applications that include TI products, you
will thoroughly test such applications and the functionality of such TI products as used in such applications. TI has not conducted any
testing other than that specifically described in the published documentation for a particular TI Resource.
You are authorized to use, copy and modify any individual TI Resource only in connection with the development of applications that include
the TI product(s) identified in such TI Resource. NO OTHER LICENSE, EXPRESS OR IMPLIED, BY ESTOPPEL OR OTHERWISE TO
ANY OTHER TI INTELLECTUAL PROPERTY RIGHT, AND NO LICENSE TO ANY TECHNOLOGY OR INTELLECTUAL PROPERTY
RIGHT OF TI OR ANY THIRD PARTY IS GRANTED HEREIN, including but not limited to any patent right, copyright, mask work right, or
other intellectual property right relating to any combination, machine, or process in which TI products or services are used. Information
regarding or referencing third-party products or services does not constitute a license to use such products or services, or a warranty or
endorsement thereof. Use of TI Resources may require a license from a third party under the patents or other intellectual property of the
third party, or a license from TI under the patents or other intellectual property of TI.
TI RESOURCES ARE PROVIDED “AS IS” AND WITH ALL FAULTS. TI DISCLAIMS ALL OTHER WARRANTIES OR
REPRESENTATIONS, EXPRESS OR IMPLIED, REGARDING TI RESOURCES OR USE THEREOF, INCLUDING BUT NOT LIMITED TO
ACCURACY OR COMPLETENESS, TITLE, ANY EPIDEMIC FAILURE WARRANTY AND ANY IMPLIED WARRANTIES OF
MERCHANTABILITY, FITNESS FOR A PARTICULAR PURPOSE, AND NON-INFRINGEMENT OF ANY THIRD PARTY INTELLECTUAL
PROPERTY RIGHTS.
TI SHALL NOT BE LIABLE FOR AND SHALL NOT DEFEND OR INDEMNIFY YOU AGAINST ANY CLAIM, INCLUDING BUT NOT
LIMITED TO ANY INFRINGEMENT CLAIM THAT RELATES TO OR IS BASED ON ANY COMBINATION OF PRODUCTS EVEN IF
DESCRIBED IN TI RESOURCES OR OTHERWISE. IN NO EVENT SHALL TI BE LIABLE FOR ANY ACTUAL, DIRECT, SPECIAL,
COLLATERAL, INDIRECT, PUNITIVE, INCIDENTAL, CONSEQUENTIAL OR EXEMPLARY DAMAGES IN CONNECTION WITH OR
ARISING OUT OF TI RESOURCES OR USE THEREOF, AND REGARDLESS OF WHETHER TI HAS BEEN ADVISED OF THE
POSSIBILITY OF SUCH DAMAGES.
You agree to fully indemnify TI and its representatives against any damages, costs, losses, and/or liabilities arising out of your noncompliance with the terms and provisions of this Notice.
This Notice applies to TI Resources. Additional terms apply to the use and purchase of certain types of materials, TI products and services.
These include; without limitation, TI’s standard terms for semiconductor products http://www.ti.com/sc/docs/stdterms.htm), evaluation
modules, and samples (http://www.ti.com/sc/docs/sampterms.htm).
Mailing Address: Texas Instruments, Post Office Box 655303, Dallas, Texas 75265
Copyright © 2018, Texas Instruments Incorporated
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Related manuals

Download PDF

advertising