Flip Chip Ball Grid Array Package

Reference Guide

Literature Number: SPRU811A

May 2005
 IMPORTANT NOTICE

Texas Instruments Incorporated and its subsidiaries (TI) reserve the right to make corrections, modifications,
enhancements, improvements, and other changes to its products and services at any time and to discontinue
any product or service without notice. Customers should obtain the latest relevant information before placing
orders and should verify that such information is current and complete. All products are sold subject to TI’s terms
and conditions of sale supplied at the time of order acknowledgment.

TI warrants performance of its hardware products to the specifications applicable at the time of sale in
accordance with TI’s standard warranty. Testing and other quality control techniques are used to the extent TI
deems necessary to support this warranty. Except where mandated by government requirements, testing of all
parameters of each product is not necessarily performed.

TI assumes no liability for applications assistance or customer product design. Customers are responsible for
their products and applications using TI components. To minimize the risks associated with customer products
and applications, customers should provide adequate design and operating safeguards.

TI does not warrant or represent that any license, either express or implied, is granted under any TI patent right,
copyright, mask work right, or other TI intellectual property right relating to any combination, machine, or process
in which TI products or services are used. Information published by TI regarding third-party products or services
does not constitute a license from TI to use such products or services or a warranty or endorsement thereof.
Use of such information 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.

Reproduction of information in TI data books or data sheets is permissible only if reproduction is without
alteration and is accompanied by all associated warranties, conditions, limitations, and notices. Reproduction
of this information with alteration is an unfair and deceptive business practice. TI is not responsible or liable for
such altered documentation.

Resale of TI products or services with statements different from or beyond the parameters stated by TI for that
product or service voids all express and any implied warranties for the associated TI product or service and
is an unfair and deceptive business practice. TI is not responsible or liable for any such statements.

Following are URLs where you can obtain information on other Texas Instruments products and application
solutions:

Products Applications
Amplifiers amplifier.ti.com Audio www.ti.com/audio
Data Converters dataconverter.ti.com Automotive www.ti.com/automotive
DSP dsp.ti.com Broadband www.ti.com/broadband
Interface interface.ti.com Digital Control www.ti.com/digitalcontrol
Logic logic.ti.com Military www.ti.com/military
Power Mgmt power.ti.com Optical Networking www.ti.com/opticalnetwork
Microcontrollers microcontroller.ti.com Security www.ti.com/security
Telephony www.ti.com/telephony
Video & Imaging www.ti.com/video
Wireless www.ti.com/wireless

Mailing Address: Texas Instruments

Post Office Box 655303 Dallas, Texas 75265

Copyright  2004, Texas Instruments Incorporated

 Contents

Contents

1 Abstract . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

2 Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8
2.1 Package Drawing Outline . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9

3 Design Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
3.1 Reliability . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
3.1.1 Daisy-Chained Units . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
3.1.2 Package Level . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
3.1.3 Board Level Reliability . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
3.1.4 Reliability Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
3.1.5 Electrical Modeling and Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
3.1.6 Thermal Modeling and Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
3.2 PCB Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
3.2.1 Land and Solder Mask . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
3.2.2 Signal Line Space and Trace Width . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
3.2.3 Routing and Vias . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
3.2.4 Pad Surface Finish . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
3.2.5 PCB Stack and Thermal Vias . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
3.3 System Level Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32
3.3.1 Thermal Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

4 SMT Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
4.1 Handling, Storage, Preparation and Bake . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38
4.2 Solder Paste Printing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
4.2.1 Stencil Design, Aperture, Material of Construction . . . . . . . . . . . . . . . . . . . . . . . . 39
4.2.2 Soldering Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
4.2.3 Coplanarity (Warpage) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
4.3 Component Placement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43
4.4 Solder Reflow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44
4.5 Defluxing (Cleaning) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47

5 Repair and Rework . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48

5.1 TI Recommendation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48

6 Mechanical Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51
6.1 External Heat Sink Attach . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51

3
Contents

7 Troubleshooting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53
7.1 Non-Destructive Failure Analysis at the SMT Level . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
7.2 Destructive Failure Analysis at the SMT Level . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59
7.3 Component Removal for Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60

8 Other Items . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62
8.1 Moisture Sensitivity of Surface Mount and BGA Packages . . . . . . . . . . . . . . . . . . . . . . . . 62
8.1.1 Recommended Baking Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63
8.1.2 Handling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66
8.1.3 Floor Life . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68
8.2 Packing Methodologies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69
8.2.1 Tray Packing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69
8.3 Electrostatic Discharge Sensitive Devices (ESDS) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70

9 Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70

4
 Figures

Figures
1. Typical Flip Chip BGA Package (Cross-Sectional View) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8
2. Flip Chip BGA Package Footprint – Mechanical Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
3. Daisy-Chain Test Configuration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
4. Typical Flow of Heat in a Flip Chip BGA Package Without Heat Sink . . . . . . . . . . . . . . . . . . 13
5. Heat Flow Analysis for Device Thermal Modeling With Heatsink . . . . . . . . . . . . . . . . . . . . . . 15
6. NSMD and SMD Pads – Top View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
7. NSMD and SMD Pads – Cross-Sectional View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
8. NSMD Versus SMD Lands Pads as Package is Mounted on
PCB—Cross-Sectional View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
9. Solder Ball Areas Susceptible to Stress Caused by Non-Optimized Package
Pad/PCB Land Ratio . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
10. Trace Routing Space . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21
11. Cross-Section of Different Via Types for Signal Transfer Through PCB . . . . . . . . . . . . . . . . 22
12. Connection Between Vias, Via Capture Pads, Surface Lands, and Stringers . . . . . . . . . . . 23
13. Space Between Surface Land Pads for a 0.45 mm NSMD Pad . . . . . . . . . . . . . . . . . . . . . . . 23
14. Via Capture Pad Layout for Escape Routing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24
15. Typical and Premium Via Capture Pad Sizes (in mils) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
16. PCB Escape Routing for a 0.8 mm BGA Pitch Using Laser-Drilled Blind Vias . . . . . . . . . . 27
17. Impact of Number of Thermal vias Versus Die (Chip) Area . . . . . . . . . . . . . . . . . . . . . . . . . . . 30
18. Impact of Number of 0.33-mm (0.013 inch) Diameter Thermal Vias Versus Die
(Chip) Area . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31
19. Thermal Management Options for Flip Chip BGA Packages . . . . . . . . . . . . . . . . . . . . . . . . . 32
20. Compact Package Model in a System-Level Thermal Simulation . . . . . . . . . . . . . . . . . . . . . 34
21. Typical SMT Assembly Process Flow for Flip Chip BGA Packages . . . . . . . . . . . . . . . . . . . . 35
22. Ideal Reflow Profile for Eutectic Solder . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46
23. Recommended Lead-Free Reflow Profile for SnAgCu Solder Paste . . . . . . . . . . . . . . . . . . . 47
24. Thermal Reflow Profile . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50
25. Major Thermal Conduction Paths to Optimize Thermal Dissipation . . . . . . . . . . . . . . . . . . . . 51
26. Schematic of a Die-Substrate-PCB System Showing Circuit Loop for TDR
Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58
27. Schematic of TDR Waveforms for a Flip Chip BGA Package. . . . . . . . . . . . . . . . . . . . . . . . . 59
28. JEDEC Shipping Trays . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69
29. Typical Tray Stack . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70

5
Tables

Tables
1 Flip Chip BGA Package Qualification Test Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
2 Optimum PCB Land Diameters for Flip Chip BGA Pad Pitches . . . . . . . . . . . . . . . . . . . . . . . 20
3 Number of Traces Routed Based on Space and Trace Line Width . . . . . . . . . . . . . . . . . . . . 21
4 Via Types for Signal Transfer Through PCB Layers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
5 Formula for Via Layouts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
6 Typical Via Capture Pad Sizes Used by PCB Vendors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26
7 Solder Paste Types Used for Surface Mounting of BGA Devices . . . . . . . . . . . . . . . . . . . . . 40
8 Typical Stages and Characteristics on a Reflow Profile . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45
9 Typical Defects Found During SMT Assembly and Probable Causes . . . . . . . . . . . . . . . . . 53
10 X-Ray Versus Optical Inspection Defect Detection (Courtesy of Metcal) . . . . . . . . . . . . . . 57
11 Moisture Classification Level and Floor Life . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68

6
 Flip Chip Ball Grid Array Package

1 Abstract
Texas Instruments (TI) Flip Chip Ball Grid Array (BGA) packages provide the
design flexibility to incorporate higher signal density and overall IC
functionality into a smaller die and package footprint.

Flip chip BGA packages can be mounted using standard printed circuit board
(PCB) assembly techniques, and can be removed and replaced using
standard repair procedures.

This document provides application guidelines for effective flip chip BGA
device handling and management, including board design rules, board
assembly parameters, rework process, thermal management,
troubleshooting, and other critical factors.

SPRU811 Flip Chip Ball Grid Array Package 7

Introduction

2 Introduction
The term flip chip describes the method of electrically connecting the die to the
package substrate. Flip chip microelectronic assembly is the direct electrical
connection of face-down (or flipped) integrated circuit (IC) chips onto
substrates, circuit boards, or carriers, using conductive bumps on the chip
bond pads.

In contrast to wire-bonding technology, the interconnection between the die

and carrier in flip chip packaging occurs when using a conductive bump placed
directly on the die surface. The bumped die is then flipped and placed face
down so that the bumps connect directly to the carrier.

Figure 1 shows a cross-section of a typical flip chip BGA package.

Figure 1. Typical Flip Chip BGA Package (Cross-Sectional View)

Lid Underfill Die FC bump Die/lid attach adhesive

Solder ball Chip capacitor Organic

substrate

Flip chip components are predominantly semiconductor devices; however,

components such as passive filters, detector arrays, and MEMs devices are
now used in flip chip form.

A more descriptive term, direct chip attach (DCA), is used when the chip is
directly attached to the printed circuit board or carrier by the conductive
bumps.

The advantages of flip chip interconnect include reduced signal inductance,

power/ground inductance, and package footprint, along with higher signal
density and die shrink.

TI’s flip chip BGA packages are assembled on either two-metal layer or
multi-layered, high-density organic laminate or ceramic substrates, and used
extensively in ASIC, HPA, and DSP applications. Package handling and
management is critical for successful operation in the field.

8 Flip Chip Ball Grid Array Package SPRU811

 Introduction

2.1 Package Drawing Outline

The flip chip BGA package outline drawing provides important mechanical
design data, including package dimensions (length, width, and thickness) and
solder ball number, size, and pitch.

Package mechanical drawings can be obtained directly from TI’s database by

simply specifying the package descriptor. Figure 2 shows the mechanical
dimensions for a 288-ball package coinciding with TI’s package designator
288GTS.

NOTE: Figure 2 is provided for reference only. Please refer to TI’s package
database for the latest dimensional data for the 288GTS package.

Figure 2. Flip Chip BGA Package Footprint – Mechanical Drawing

GTS (S−PBGA−N288) Plastic Ball Grid Array
23,10
SQ
22,90 21,00 TYP
21,10 1,00
SQ
20,90
0,50

AB
AA
Y
W
V
U
T
R 1,00
P
N
M
L
K
J 0,50
A1 Corner H
G
F
E
D
C
B
A
1 3 5 7 9 11 13 15 17 19 21
2 4 6 8 10 12 14 16 18 20 22
Bottom View

2,80 MAX
1,90 NOM

Seating Plane

0,70
0,10 0,60 0,15
0,50 NOM 0,50
0,40

4205308/B 01/04
NOTES: A. All linear dimensions are in millimeters
B. Drawing subject to change without notice
C. Flip chip application only
D. Falls within JEDEC MO−034B

SPRU811 Flip Chip Ball Grid Array Package 9

Design Considerations

3 Design Considerations
Each flip chip BGA goes through rigorous qualification tests before the
package is released to production. The following sections discuss the various
tools that are used to predict package performance in an application.

3.1 Reliability

3.1.1 Daisy-Chained Units

Use daisy-chained units (mechanical samples) to gain experience in:

- Handling and mounting flip chip BGA packages for board-reliability testing
- Checking PCB electrical layouts
- Confirming the accuracy of the mounting equipment

Daisy-chained packages provide a continuous path through the package for

ease-of-testing. TI issues a net list for each package that correlates each ball
position to a corresponding die bump number.

Assembling a daisy-chained package on the PCB forms a complete circuit and

allows continuity testing. The circuit includes the following:

- Solder balls
- Metal pattern on the die
- Bumps
- Package interconnects/traces
- PCB traces

You can interconnect and test the entire package or only a quadrant. Figure 3
shows the test configuration.

Figure 3. Daisy-Chain Test Configuration

Tester
Chip

Solder balls

PCB

Copper traces Test pads

10 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Each flip chip BGA goes through rigorous qualification tests before the
package is released to production. Samples used in these tests are
preconditioned according to Joint Electronic Device Committee (JEDEC)
A113 at various levels. Table 1 summarizes typical package qualification tests.
Additional environmental or mechanical tests may be performed. Please refer
to the product data sheet for specific package reliability data.

3.1.2 Package Level

Package reliability focuses on:

- Materials of construction
- Thermal flows
- Material adherence/delamination issues
- Resistance to high temperatures
- Moisture resistance
- Flip chip joint/interconnect

Table 1. Flip Chip BGA Package Qualification Test Summary

Test Environments Conditions

Highly-accelerated stress test (HAST) 85%RH/85_C
Autoclave 121_C, 15 psig

Temperature cycle, air-to-air −65/150_C, or

−55/125_C
−65/150_C, or
−40/125_C

Thermal shock, liquid-to-liquid −65/150_C, or

−55/125_C, or
−40/125_C

High temperature operating life (HTOL) 125_C, Op. voltage

HTOL‡ 140_C, Op. voltage

HTOL‡ 155_C, Op. voltage

Bake high temperature storage life (HTSL‡) 150_C

Board level/solder joint reliability temperature cycle −40/125_C, or

0/100_C

HAST 130_C
† RH = relative humidity
‡ One or more optional tests may be added to meet customer requirements.

SPRU811 Flip Chip Ball Grid Array Package 11

Design Considerations

3.1.3 Board Level Reliability

In addition to device/package testing, TI performs board-level reliability (BLR)

testing on flip chip BGA packages.

BLR testing includes:

- Assembling daisy-chained packages to testing boards and exposing them

to temperature cycles
- Taking electrical measurements in the initial state and then at intervals
after temperature cycles are run

Two important conclusions can be drawn from BLR testing:

- PCB land size should match the package pad size.

- Solder paste and flux is required for attachment to give optimal reliability.

3.1.4 Reliability Modeling

Reliability modeling is another important tool used to predict package

performance in an application. Thermal, electrical, and thermo-mechanical
modeling, verified by experimental results, provide insight into system
behavior. This modeling process also shortens package development time,
predicts system lifetimes, and provides an important analytical tool.

In applications such as BGAs, where interconnections are made through

solder balls, the useful life of the package usually depends on the useful life
of the solder itself. Because this area has been studied extensively, accurate
models exist, both for predicting solder behavior and for interpreting
accelerated life testing.

TI methodology includes extensive model refinement and constant

experimental verification. For a given package, a detailed 2D finite element
model (FEM) is constructed that performs 2D plain strain elastoplastic
analysis to predict areas of high stress.

These models also account for the thermal variation of material properties,
such as modulus of elasticity, coefficient of thermal expansion (CTE), and
Poisson’s ratio as a function of temperature. These allow the FEM to calculate
the thermo-mechanical plastic strains in the solder joints for a given thermal
loading.

Package and board-level stress analysis is performed using finite element

modeling, which provides full 3D nonlinear capabilities for package stress,
component warpage, and solder joint reliability studies.

12 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

3.1.5 Electrical Modeling and Analysis

Texas Instruments extensive package characterization capabilities include an
electrical measurements lab with time domain reflectometer/inductance
resistance capacitance (TDR/LRC) and network analysis capabilities.

Package electrical design (PACED), an internally-developed tool, performs

electrical modeling that provides 2.5D and full 3D capability for LRC models,
transmission lines, dielectrics, and SPICE deck outputs.

3.1.6 Thermal Modeling and Analysis

The high operating temperature of a device, caused by the combination of
ambient conditions and device power dissipation, is an important reliability
concern. For instance, instantaneous high temperature rises can possibly
cause catastrophic failure, as well as long-term degradation in the chip and
package materials, both of which may eventually lead to failure.

Most TI flip chip BGA devices are designed to operate reliably with a junction
temperature of no more than 105°C. To ensure this condition is met, thermal
modeling is used to estimate the performance and capability of IC packages.
Design changes can be made and thermally tested from a thermal model
before any time is spent on manufacturing.

Components with the most influence on the heat dissipation of a package can
also be determined. Models can approximate the performance of a package
under many different conditions.

Figure 4 shows the typical heat flow paths in a flip chip BGA package for a
typical system without an exposed heat spreader or heat sink.

Figure 4. Typical Flow of Heat in a Flip Chip BGA Package Without Heat Sink
80−90% of heat ~10−20% of heat

Thermal modeling is performed using ThermCAL, a TI internal thermal

simulation tool, and a third-party computer simulation package. Modeling
includes complex geometries, transient analysis, and anisotropic materials.
These capabilities provide a full range of thermal modeling, from device
through system level.

SPRU811 Flip Chip Ball Grid Array Package 13

Design Considerations

In addition, the flip chip BGA packages undergo extensive empirical thermal
characterization. The package thermal dissipation capabilities are physically
measured in an internal lab with JEDEC standard test conditions up to 1,000
watts.

The following metrics are commonly used to characterize flip chip BGA
packages in thermal design:

- RθJC: Resistance from die (junction) to the top of the package (case);
measured using an infinite heat sink on the top of the package. This metric
is useful primarily when the case of the package is connected to an
external heat sink.
- RθJB: Resistance from die to the bottom of the package (board, measured
1 mm from package), as defined in the Joint Electronic Device Committee
(JEDEC) standard, JESD 51−8. This metric includes some of the board
characteristics and their coupling with the package.
- RθJA: (JESD 51−2) Total resistance of the whole system from die to
ambient still air under standard conditions.
- RθJMA: (JESD 51−6) Total resistance of the whole system from die to
moving air under standard conditions.
- Psi-jt: Pseudo resistance from die to the top of the package (value varies
by environment).
- Psi–jb: Pseudo resistance from die to board (measured 1 mm from
package; value varies by environment).

Figure 5 shows the heat flow analysis for thermal modeling of a device with a
heat sink.

14 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Figure 5. Heat Flow Analysis for Device Thermal Modeling With Heatsink

Air Ta

Thermocouple Rsa Sink to air

attachment

Sink
Rcs Case to sink

Rjc
Case/sink joint
Tc Tj Junction to case
Junction

Case Rcb Case to board

Rb Board
Board

Power planes
and vias Rba Board to air

Air
Ta

3.2 PCB Design

The primary board design considerations include metal-pad sizes and
associated solder-mask openings. PCB pads/land patterns, which are used
for surface mount assembly, can be:

- Non-solder mask defined (NSMD) — The metal pad on the PCB (to which
a package BGA solder ball is attached) is smaller than the solder mask
opening.
- Solder mask defined (SMD) — The solder mask opening is smaller than
the metal pad.

Figure 6 and Figure 7 illustrate the metal-pad and associated solder-mask

openings.

SPRU811 Flip Chip Ball Grid Array Package 15

Design Considerations

Figure 6. NSMD and SMD Pads – Top View

Non-solder mask defined pad Solder mask defined pad

Figure 7. NSMD and SMD Pads – Cross-Sectional View

Solder mask Solder mask
Solder opening Copper Solder opening Copper
mask pad mask pad

The most common PCB material sets on which assembly can be performed
are:

- Standard epoxy glass substrate

- FR-4
- BT (bismaleimide triazine)

The mechanical properties of the PCB, such as its CTE, can be affected by the
number of metal layers, laminate materials, trace density, operating
environment, site population density, and other considerations.

The more flexible, thinner PCBs consequently show greater reliability during
thermal cycling. The industry standard PCB thickness ranges from 0.4 mm to
2.3 mm.

3.2.1 Land and Solder Mask

The design of the PCB and the flip chip BGA itself is important in achieving
good manufacturability and optimum reliability. When designing a PCB for
fine-pitch BGA packages, consider the following factors:

- Surface land pad dimension

- Via capture pad layout and dimension
- Signal line space and trace width
- Number of PCB layers

16 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Figure 8 shows the location of the package pad (A) and board lands (B).

Figure 8. NSMD Versus SMD Lands Pads as Package is Mounted on

PCB—Cross-Sectional View
A

BGA package

BGA solder ball

Solder mask

PCB

B
Copper
pad

Figure 9 illustrates why the layout and dimensions of the package pads and
the board lands are critical. Matching the diameters of the PCB pad to the
package side BGA pad helps form a symmetrical interconnect, and prevents
one end of the interconnect from exhibiting a higher stress condition than the
other.

SPRU811 Flip Chip Ball Grid Array Package 17

Design Considerations

Figure 9. Solder Ball Areas Susceptible to Stress Caused by Non-Optimized Package

Pad/PCB Land Ratio
Package

PCB

Package

PCB

Package

PCB

In fact, if the design of the PCB pad diameters are even slightly smaller than
the package side BGA pad diameter, the joint stress on the PCB side is
emphasized rather than on the typically weaker package BGA side.

The top view of Figure 9 shows a package pad that is larger than the PCB land.
In this case, the solder ball is prone to crack prematurely at the PCB interface.

In the middle view of Figure 9, the PCB land is larger than the package pad,
which leads to cracks at the package surface.

In the bottom view of Figure 9, where the ratio is almost 1:1, the stresses are
equalized and neither site is more susceptible to cracking than the other. This
is the preferred design.

Solder lands on the PCB are generally simple round pads. Solder lands are
either SMD or non-solder-mask-defined NSMD.

18 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Non-Solder-Mask-Defined (NSMD) Land

With NSMD-configured pads, there is a gap between the solder mask and the
circular contact pad (refer to Figure 6). With this configuration, the solder flows
over the top surface and the sides of the contact pad.

The additional NSMD soldering area results in a stronger mechanical bond.

In addition, the additional area allows NSMD pads to be smaller than SMD
pads. The smaller size is beneficial for system designers, as they allow more
room for escape trace routing.

Table 2 shows optimum land diameters for a current flip chip BGA pitch. For
PCB land definition, the NSMD land is recommended. Solder mask on the land
is considered a process defect.

A disadvantage of the NSMD land is that surrounding traces are also exposed
when trace routing is dense, and there is the potential for shorting circuits
during ball attach and reflow.

Solder-Mask-Defined (SMD) Land

With the SMD land, the copper pad is larger than the desired land area; the
opening size is defined by the opening in the solder mask material.

The SMD technique includes these advantages:

- More closely controlled size as a result of photo-imaging the stencils for

masks
- Better copper adhesion to the laminate

The chief disadvantage of this method is that the larger copper pad can make
routing more difficult.

SPRU811 Flip Chip Ball Grid Array Package 19

Design Considerations

Table 2. Optimum PCB Land Diameters for Flip Chip BGA Pad Pitches

Package Side
Solder Mask Defined (SMD) Land
Solder Mask Copper Stencil Stencil
Ball Pitch Opening Land Thickness Diameter
(mm) (mm) (mm) (mm) (mm)
0.80 0.45 0.52 0.15 0.35–0.40

1.00 0.55 0.65 0.15 0.45–0.50

PCB Side
Non-Solder Mask Defined (NSMD) Land

Copper Solder Mask Stencil Stencil

Ball Pitch Land Opening Thickness Diameter
(mm) (mm) (mm) (mm) (mm)

0.80 0.45 0.60 (see note) 0.15 0.35–0.40

1.00 0.55 0.70 (see note) 0.15 0.45–0.50

Note: The TI recommended number accounts for both size variation and mis-registration of the solder mask opening. Contact
your PCB supplier to ensure solder mask openings can be accommodated without risk of solder mask on the pad/land.

High CTE Ceramic Flip Chip BGA

The recommended solder pad geometry and solder mask opening for high-
CTE ceramic flip chip BGAs is 0.55 mm (21.7 mils) diameter with a non-solder
mask-defined (NSMD) BGA pad. A reasonable solder mask opening diameter
for this pad is 0.65 mm. Check the PCB fabricator’s Design for
Manufacturability guide before making a final decision regarding pad design.

NOTE: TI has successfully performed BLR temp cycling, 0°C-100°C, using these
PCB pad and solder mask opening sizes. If routing is a concern, a 0.5 mm (19.7
mils) pad may be considered without compromising solder joint reliability.

3.2.2 Signal Line Space and Trace Width

Many of today’s circuit board layouts are based on a maximum

100-µm-conductor line width and 200-µm spacing. To route between
0.8-mm-pitch balls, given a clearance of roughly 380 µm between ball lands,
only one signal can be routed between ball pads.

20 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

The ability to perform escape routing is determined by the width of the trace
and the minimum space required between traces. This width is calculated by
the following formula:

g = 39.37 – d

The number of traces that can be routed through this space is based on the
permitted line trace and space widths. Use the formula to determine the total
number of traces that can be routed through g.

Table 3. Number of Traces Routed Based on Space and Trace Line Width

Number of Traces Formula

1 G = [2x(space width)] + trace width
2 G = [3x(space width)] + [2x(trace width)]
3 G = [5x(space width) + [3x(trace width)]

By reducing the trace and space size, you can route more traces through g,
as shown in Figure 10. Increasing the number of traces reduces the required
number of PCB layers and decreases the overall cost. On the other hand, as
line width decreases, PCB cost may go up and quality may be sacrificed.

Figure 10. Trace Routing Space

Double trace routing Single trace routing

0.45 mm 0.45 mm

0.35 mm 0.35 mm

0.07 mm 0.12 mm

0.45 mm 0.45 mm

Via capture pad

Space
Trace

SPRU811 Flip Chip Ball Grid Array Package 21

Design Considerations

3.2.3 Routing and Vias

High Density Routing Techniques

Conventionally, pads are connected by wide copper traces to other devices or
to plated-through holes (PTH). As a rule, the mounting pads must be isolated
from the PTH. Placing the PTH interstitially to the land pads often achieves this
isolation.
As available BGA pitch space contracts, the space available for signal fan-out
also decreases. This poses a challenge when designing with BGA packages;
however, by using high-density routing, the PCB designer can minimize many
of these design and manufacturing challenges.
Vias are actual holes drilled through a multi-layer PCB to provide electrical
connections between various PCB layers. In SMT PCBs, vias provide
layer-to-layer connections. In some cases microvias (defined in the Via
Density section) are filled with reinforcing material. Table 4 lists the different
via types for PCB signal transferring.

Table 4. Via Types for Signal Transfer Through PCB Layers

Type Description
Through via An interconnection between the top and the bottom layer of the PCB; through vias can also
provide interconnections to inner PCB layers.

Blind via An interconnection from the top or bottom layer to an inner PCB layer

Embedded via An interconnection between any number of inner PCB layers

Figure 11 illustrates these vias.

Figure 11. Cross-Section of Different Via Types for Signal Transfer Through PCB
Through Blind Embedded
via via via

Connection to
PCB layer
PCB layers

22 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Although blind vias can be more expensive than through vias, overall costs can
be reduced because signal traces can be routed under a blind via, which
requires fewer PCB layers.
Through vias do not permit signals to be routed through lower layers, which
can increase overall costs by increasing the required number of PCB layers.
However, PCBs built using only through-hole vias can be economical due to
the reduced complexity in board manufacturing.

Stringers
Stringers are rectangular or square interconnect segments that electrically
connect via capture pads and surface land pads. Figure 12 shows the
connection between vias, via capture pads, surface land pads, and stringers.

Figure 12. Connection Between Vias, Via Capture Pads, Surface Lands, and Stringers
Via
Stringer Via capture pad

PCB land pads

Figure 13 shows the space available between surface land pads for a 0.40 mm
(15.75 mil) BGA pad.

Figure 13. Space Between Surface Land Pads for a 0.45 mm NSMD Pad
0.8 mm
0.35 mm

0.35 mm 0.68 mm 0.8 mm

0.45 mm

PCB land pads

SPRU811 Flip Chip Ball Grid Array Package 23

Design Considerations

Via Capture Pad Layout and Dimension

The size and layout of via capture pads affect the amount of space available
for escape routing. In general, the layout of via capture pads can be :
- Horizontal with the surface land pads
- Diagonal to the surface land pads

Figure 14 shows both inline and diagonal layouts.

Figure 14. Via Capture Pad Layout for Escape Routing

Horizontally Diagonally

0.8 mm 0.8 mm
c
a
b
b a

f d

0.35 mm e g 0.8 mm d

f c
0.45 mm 0.45 mm f

e g

f
Key:
Surface land pad c Minimum clearance between via
Via capture pad capture pad and surface land pad
d Via capture pad diameter
Vias
e Trace width
Stringer
f Space width
a Stringer length
g Area for escape routing (this area is
b Stringer width on a different PCB layer than the
surface land pads)

Consider the following factors when deciding to place the via capture pads
diagonally or inline with the surface land pads:
- Diameter of the via capture pad
- Stringer length
- Clearance between via capture pad and surface land pad

Use the information shown in Figure 14 and Table 5 to determine the PCB
layout. If your PCB design guidelines do not conform to either equation in
Table 5, contact your PCB supplier for assistance.

24 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Table 5. Formula for Via Layouts

Layout Formula
Horizontally a + c + d = 0.6 mm (23.62 mils)

Diagonally a + c + d = 1.0 mm (39.76 mils)

According to Table 5, you can place a larger via capture pad diagonally than
horizontally with the surface land pads. Via capture pad size also affects how
many traces can be routed on a PCB. Figure 15 shows sample layouts of
typical and premium via capture pads.

Figure 15. Typical and Premium Via Capture Pad Sizes (in mils)

Typical Premium

39.37 mil 39.37 mil

8.0 mil 5.0 mil 3.0 mil

4.0 mil 15.0 mil
27.0 mil 20.0 mil

Via
Via capture pad
Space
Trace

Note: 1mil = 0.0254 mm.

The typical layout shows a via capture pad size of 27 mil, a via size of 8 mil,
and an inner space/trace of 4 mil. Only one trace can be routed between the
vias. If more traces are required, you must reduce either the via capture pad
size or the space/trace size.

The premium layout shows a via capture pad size of 20 mil, a via size of 5 mil,
and an inner space/trace of 3 mil. This layout provides space enough to route
two traces between the vias.

Table 6 shows the typical and premium layout specifications used by most
PCB vendors.

SPRU811 Flip Chip Ball Grid Array Package 25

Design Considerations

Table 6. Typical Via Capture Pad Sizes Used by PCB Vendors

Typical Premium
Specification (mils) (mils)
Trace/space width 5/5 3/3

Drilled hole diameter 12 10

Finished via diameter 8 5

Via capture pad 25.5 20

Aspect ratio 7:1 10:1

Via Density
Via density can be a limiting factor when designing high-density boards. Via
density is defined as the number of vias in a particular board area. Using
smaller vias increases the routability of the board by requiring less board
space and increasing via density.
The microvia solves many of the problems associated with via density.
Microvias are often created using a laser to penetrate the first few layers of
dielectric. The layout designer can then route to the first internal board layer.
Typically, two layers (e.g., each 4 mil thick) can be laser-drilled, creating a
200-micron microvia diameter. In this case, routing to the first two internal
layers is possible.
In general, the number of PCB layers required to route signals is inversely
proportional to the number of traces between vias (i.e., the greater the number
of traces, the fewer the number of PCB layers required). You can estimate the
number of layers your PCB requires by first determining the following:
- Trace and space size
- Number of traces routed between the via capture pads
- Type of vias used

Choosing the correct via type and using fewer than the maximum number of
I/O pins can reduce the required number of layers.
Clearance is increased by placing the vias in the pad. However, a standard via
opening of 300 µm causes the solder to wick down into the via, and further
causes weak or even open solder joints. In addition, the capture pad is larger
than the solder pad.
Laser-drilled microvias can drill a hole of 100 µm in the board, which is reduced
to 50 µm after plating. The resulting via-hole diameter is reduced to the point
where the solder does not wick down the via.

26 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

A potential drawback to the laser-drilled microvia approach is that after plating,

vias that are too small can potentially trap air instead of being properly filled
with the PCB dielectric material. Therefore, the risk of reliability issues is
increased.

Figure 16 illustrates an example of escape routing for a 0.8 mm BGA pitch

using laser-drilled microvias. In this example, 0.15mm trace lines and spaces
allow escape routing of the first two BGA signal rows through the top PCB
layer. Because of the use of blind vias connecting the first two PCB layers,
escape routing from the third and fourth BGA signal rows can be done through
the second PCB layer. Therefore, signal routing can be accomplished in only
two PCB layers.

Figure 16. PCB Escape Routing for a 0.8 mm BGA Pitch Using Laser-Drilled Blind Vias
Row 4 Row 3 Row 2 Row 1

0.80 mm BGA pitch

0.45 mm pad

0.60 mm solder
mask opening
400 micron via
capture pad 150 micron trace line

200 micron via

1st (top) layer routing
2nd layer routing

SPRU811 Flip Chip Ball Grid Array Package 27

Design Considerations

3.2.4 Pad Surface Finish

Two commonly-used PCB pad surface finishes for surface mount devices are:

- Electroless Ni + immersion gold plating (ENIG)

- Cu OSP (organic solderability preservative)

ENIG is a versatile process and enables fabrication of high-density flip chip

BGA substrates needed for high−performance IC chips. ENIG is used
extensively in advanced IC packaging of microprocessors, ASIC, and DSP
components. Both finishes require the surface coating to be uniform,
conforming, and free of impurities to ensure a consistent, solderable system.

The ENIG finish consists of plating electroless nickel over the copper pad,
followed by a thin layer of immersion gold. The allowable stresses and
temperature excursions the PCB is subjected to throughout its lifetime,
determine the thickness of the electroless nickel layer. This thickness is
typically 5 µm nickel and about 0.05 µm for gold, to prevent brittle solder joints.

By its nature, ENIG plating forms brittle intermetallic compounds of nickel, tin,
and other elements in the plating after solder balls are attached to the package.
Certain conditions of high strain and high strain rates are known to cause ENIG
solder joints to fail. Therefore, you must avoid excessive shock and bending
of the PC board during assembly, handling, and testing of FCBGAs with ENIG
plating. Refer to section 4.1 for more on handling TI’s ENIG-plated
components.

The second recommended solderable finish consists of an organic

solderability preservative (OSP) coating over the copper-plated pad. The
organic coating assists in preserving the copper metallization for soldering.

The advantages of ENIG plating over Cu OSP are:

- Longer shelf life

- Permanent coverage of copper vias
- Resistance to oxidation during multiple-pass assembly
- Contamination resistance

Other alternative pad finishes which are available in the market today, are hot
air solder leveled (HASL), immersion silver, immersion tin, and electrolytic
Ni-Au. Industry efforts are focused on developing and qualifying lead-free
metallizations. Therefore, the continued acceptance of HASL and other
lead-based metallizations may become limited in the mMicroelectronics/PCB
manufacturing industry.

28 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

3.2.5 PCB Stack and Thermal Vias

Adequately designed thermal vias, along with an adequate number of thermal
balls, contributes to the thermal enhancement of both large and small flip chip
BGA packages. This section focuses on the design and value of thermal vias,
while section 3.3.1, Thermal Design, discusses overall thermal
considerations.

The thermal balls must attach to a thermal spreading plane or land in the PCB
with adequate area to convect and radiate the heat generated by the
component.

Thermal vias are the primary method of heat transfer from the PCB thermal
land to the internal copper planes or to other heat removal sources. Thermal
vias help to give a closer coupling of the device to the buried planes, which
results in more efficient heat spreading and more uniform temperature
distribution across the PCB. The larger effective cooling area around the
device also allows its heat to be more efficiently dissipated off the board
surfaces by convection and radiation.

The overall cooling effect can be significant, especially in smaller packages

with less substrate layers, where little heat spreading can occur in the package
itself.

Important factors in both the flip chip BGA package thermal performance and
the package-to-PCB assembly are:

- Number of thermal vias used

- Size of the thermal vias
- Construction of the thermal vias

Figure 17 and Figure 18 show how varying the number of thermal vias affect
PCB thermal resistance. Various sizes of die for two and four-layer PCBs are
used.

SPRU811 Flip Chip Ball Grid Array Package 29

 Design Considerations

Figure 17. Impact of Number of Thermal vias Versus Die (Chip) Area
JEDEC 2−layer board thermal resistance (JC)
comparison
60
1 via 10K die area
Board thermal resistance (JC)

50 50K die area

100K die area
40 150K die area
2 vias
(C/W)

30
Thermal vias diameter=13.0 mil
20

10 11 vias
11 vias 11 vias
17 vias
0
0 1 2 3 4 5 6 7 8 9 10
Thermal vias copper cross area (% of die area)
Note: Apply bare die to the JEDEC board.

30 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

Figure 18. Impact of Number of 0.33-mm (0.013 inch) Diameter Thermal Vias Versus Die
(Chip) Area

JEDEC 4−layer board thermal resistance (JC)

vs. thermal vias cross area
30
1 via 10K die area
50K die area
25 100K die area
Board thermal resistance (JC)

150K die area

2 vias
20
(C/W)

15
Thermal vias diameter=13.0 mil

10

11 vias 11 vias
22 vias 11 vias
5
17 vias
55 vias
0
0 1 2 3 4 5 6 7 8 9 10
Thermal vias cross area (% of die area)

Note: Apply bare die to the JEDEC board

The curves indicate that a point of diminishing returns occurs where additional
vias do not significantly improve the thermal transfer through the board.

The number of thermal vias will vary with each product assembled to the PCB,
depending on the amount of heat that must be moved away from the package
and the efficiency of the system heat-removal method.

To arrive at an optimum value for your board construction, you must perform
characterization of the heat-removal efficiency versus the thermal via copper
surface area. The number of vias required can then be determined for any new
design to achieve the desired thermal removal value.

In general, adding more metal through the PCB under the IC improves
operational heat transfer, but requires careful attention to uniform heating of
the board during assembly.

SPRU811 Flip Chip Ball Grid Array Package 31

Design Considerations

3.3 System Level Design

3.3.1 Thermal Design

Thermal design (design of the system to ensure adequate cooling of the

device) starts with an understanding of the different parts of the thermal
system. The first important factor is power dissipation from the device.

Figure 19 shows a rough estimate of the thermal designs required to support

different power dissipation levels. If the device power dissipation is mid- or
high-range, see section 6.1, External Heat Sink Attach, for recommendations
on external heat sinks.

Figure 19. Thermal Management Options for Flip Chip BGA Packages

Bare package with Bare package; may be

Low end
moderate air used with moderate
1−6 watts
8−12°C/Watt airflow within a system

Package used with

Passive H/S various forms of
Low end + air
1−6 watts passive heatsinks
5−10°C/Watt and heat spreader
techniques

Package used with

Active heatsink active heatsinks
Low end 2−3°C/Watt
1−6 watts TEC and board level
or better heat spreader
techniques

The second factor in thermal design is ensuring that the flip chip BGA package
is properly designed to provide the needed thermal performance. The number
one thermal enhancement for both large and small flip chip BGA packages is
an adequate number of thermal balls, in conjunction with adequately designed
thermal vias, in both the flip chip BGA interposer and system-level PCB.

These thermal balls are most effective when attached to a spreading plane in
the PCB with an adequate area to convect and radiate the heat from the
component to the environment.

Other thermal enhancements include adding planes in the substrate and using
heat spreaders above the die.

32 Flip Chip Ball Grid Array Package SPRU811

 Design Considerations

The third factor in thermal design is system-level requirements. Thermal

analysis must incorporate system-level characteristics, such as:

- Number of neighboring devices

- Location on the PCB
- Ambient temperature conditions
- Use of external heat sinks
- Airflow

To accomplish this, you can use the data and models discussed in section
3.1.6, Thermal Modeling and Analysis, in several ways:

- Using JEDEC standard thermal metrics, such as θJA or θJMA, to compare

a given device to a device that operates in the same environment.

NOTE: These standard values should not be used to make absolute calculations of
the junction temperature, because the difference between the device environment
and JEDEC environment will cause error.

- Using package thermal resistance values to estimate the junction

temperature based on a reference temperature.
J Use the JEDEC θJB value only if the board temperature near the
package can be held constant.
J Use the θJC value only if the part will have a conduction cooling
mechanism (such as a heat sink) attached to the top of the package.

- Including a compact or detailed package model in a system-level thermal

simulation (see Figure 20).

SPRU811 Flip Chip Ball Grid Array Package 33

Design Considerations

Figure 20. Compact Package Model in a System-Level Thermal Simulation

Note: Planes show temperature profile. Streamlines show airflow. Graphic by Flomerics, Ltd.

34 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

4 SMT Assembly
Surface-mount technology (SMT) has evolved over the past decade from an
art into a science with the development of design guidelines and rules.
Although these guidelines are specific enough to incorporate many shared
conclusions, they are general enough to allow flexibility in board layouts,
solder pastes, stencils, fixturing, and reflow profiles.

Most assembly operations have found flip chip BGA packages to be robust and
manufacturing-friendly, and able to fit easily within existing processes and
profiles. Flip chip BGA packages do not require special handling in package
form; however, as with any printed circuit assembly, extraordinary care should
be taken to avoid unnecessary bending, flexing, or bowing of the PCB which
could result in damage to the solder joints. Furthermore, as ball pitch becomes
smaller, layout methodology and accuracy of placement become more critical.

The major process steps involved in flip chip BGA assembly are:

- Solder paste printing using a stencil-printing process

- Component placement
- Reflow

Solder paste inspection, cleaning, and X-ray inspection are optional and
depend on the materials/process used. Figure 21 shows the assembly
process flow.

Figure 21. Typical SMT Assembly Process Flow for Flip Chip BGA Packages

Solder paste Reflow

printing

Solder paste Cleaning

inspection

X−ray inspection
Pick and place
(chip caps)

Test Rework
Fine pitch
component placement
System assembly

SPRU811 Flip Chip Ball Grid Array Package 35

SMT Assembly

Design for Manufacturability (DFM)

A well-designed board that follows the basic SMT considerations greatly
improves the cost, cycle time, and quality of the end product. Board design
should comprehend the SMT-automated equipment used for assembly,
including minimum and maximum dimensional limits, and placement
accuracy.

Many board shapes can be accommodated, but the front of the board should
have a straight and square edge to help machine sensors detect it.
Odd-shaped or small boards can be assembled, but require panelization or
special tooling to process inline.

In general, the more irregular the board is —non-rectangular with cutouts—

the more expensive the assembly cost will be.

Fiducials, the optical alignment targets that align the module to the automated
equipment, should allow vision-assisted equipment to accommodate the
shrink and stretch of the raw board during processing.

Fiducials define the coordinate system for all automated equipment, such as
printing and pick-and-place. The following guidelines are useful for ensuring
ease-of-assembly and high yield:

- Automated equipment requires a minimum of two and preferably three

fiducials.

- A wide range of fiducial shapes and sizes can be used. Among the most
useful is a circle 1.6 mm in diameter with an annulus of 3.175 mm/3.71
mm. The outer ring is optional, but no other feature may be within 0.76 mm
of the fiducial.

- The most useful placement for the fiducials is an L configuration that is

orthogonal to optimize the stretch/shrink algorithms. When possible, the
lower left fiducial should be the design origin (coordinate 0,0). It is also
common to position the package pin 1 (A1) corner in the corner without the
fiducial.

- All components should be within 101.6 mm of a fiducial to guarantee

accuracy of placement. For large boards or panels, a fourth fiducial should
be added.

If the edges of the boards are to be used for conveyer transfer, a cleared zone
of at least 3.17 mm should be allowed. Normally, the longest edges of the
board are used for this purpose, and the actual width depends on equipment
capability. Although no component lands or fiducials can be present in this
area, breakaway tabs may be present in this area.

36 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

By using the longest edges for support on the conveyor rails, board sag due
to self-weight is reduced considerably on large PCB designs with numerous
components. On smaller boards, it may not be as critical.

Inter-package spacing is a key aspect of DFM. The question of how close

together components can be placed is a critical one. The following component
layout considerations are recommendations based on TI experience:

- There should be a minimum of 0.508 mm of space between land areas of

adjacent components to reduce the risk of shorting.

- The recommended minimum spacing between SMD discrete component

bodies is equal to the height of the tallest component. This allows for a 45°
soldering angle in case manual work is needed.

- Polarization symbols should be provided for discrete SMDs (diodes,

capacitors, etc.) next to the positive pin.

- Pin-1 indicators or features are needed to determine the keying of SMD

components.

- Space between lands (under components) on the backside discrete

components should be a minimum of 0.33 mm. No open vias may occupy
this space. The direction of backside discretes for wave solder should be
perpendicular to the direction through the wave.

- Do not place SMT components on the bottom side that exceed 200 grams
per square inch of contact area with the board.

- If space permits, symbolize all reference designators within the land

pattern of the respective components.

- It is preferable to have all components oriented in well-ordered columns

and rows.

- Group similar components together whenever possible.

- Allow room for testing.

SPRU811 Flip Chip Ball Grid Array Package 37

SMT Assembly

4.1 Handling, Storage, Preparation and Bake

Many factors contribute to a high-yield assembly process. The following lists
a few of the key focus areas and their contributing factors:

- Solder paste quality

J Must have uniform viscosity and texture

J Must be free of foreign material
J Must be used before expiration date
J Must be maintained at the proper shipment and storage temperature
J Must be protected from drying out on the solder stencil

- PCB quality

J Must have a clean, flat, plated or coated solder land area

J Attachment surface must be clean and free of solder mask residue

- Placement accuracy

J Tight tolerances are usually required.

J Alignment marks (fiducials) on the PCB help verify that parts are
correctly placed.

- Solder reflow profile

J Solder reflow temperature is dependent on the PCB design, PCB

thickness, type of components, component density, and the
recommended profile of the solder paste being used.
J A reflow profile must be developed for each PCB using various
packages.

- Solder volume ensures optimum contact of all intended solder

connections.

Certain conditions of high strain and high strain rates are known to cause ENIG
solder joints to fail. Therefore, we must use care to avoid excessive shock and
bending of the PC board during assembly, handling, and testing of FCBGAs
with ENIG plating. Examples of severe mechanical loading that produce high
strain and strain rates during PCB assembly are in-circuit test (ICT), manual
connector insertion, PCB edge-guide snap-off, two-sided assembly, and
mechanical assembly. TI recommends that appropriate strain and strain-rate
characterization on the PCB assembly process be performed prior to
assembly of a new PCB design. Additional care should be taken to avoid steps

38 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

where severe mechanical loads could potentially impact the reliability of the
ENIG solder joint.

TI has determined PCB thickness to be an important element in the reliability

of ENIG solder joints. To that point, TI has determined PCB thicknesses of
0.093 inches to be acceptable. Use of PCBs of lesser thickness should be fully
evaluated using the assembly process, testing and system integration
procedures to be used by the customer or contract manufacturer. PCB
thickness greater than 0.093 inches may have a deleterious effect on
long−term cyclic temperature performance. Therefore, the customer should
select a PCB thickness that is suitable to resist damage to the package during
PCB assembly, and ensure long−term reliability for its intended field
application.

4.2 Solder Paste Printing

Solder paste printing, the first step in the surface mount assembly process,
plays a critical role in reflow soldering and successful device mounting. The
paste acts as an adhesive before reflow and may even help align skewed parts
during soldering. The paste contains flux, solvent, suspending agent, and
solder of the desired composition.

Characteristics such as viscosity, dispensing, printing, flux activity, flow, ease

of cleaning, and spread are key considerations in selecting a particular paste.
Susceptibility of the paste to solder ball formation and wetting characteristics
are also important selection criteria.

In most cases, solder paste is applied by stenciling on the solder pads before
component placement. Stencils are etched stainless steel or brass sheets. A
rubber or metal squeegee blade forces the paste through stencil openings that
precisely match the land patterns on the PCB.

Stencils are essentially the industry standard for applying solder paste.
Screens with emulsion masks can be used, but stencils provide more crisp and
accurate print deposits, especially for fine-pitch or high pin-count BGAs.

Printing paste onto the component minimizes flux contamination on the board
and eliminates the possibility of solder contamination into vias because of poor
stencil cleanliness.

4.2.1 Stencil Design, Aperture, Material of Construction

Stencils used for BGA assembly are normally made of stainless steel. The
stencil aperture should be designed based on such characteristics as BGA ball
size, pad size, and stencil thickness.

SPRU811 Flip Chip Ball Grid Array Package 39

SMT Assembly

Normally, round apertures are used in the stencils for BGAs. The
pad-to-stencil aperture ratio is normally kept at 1:1. For fine pitch devices,
including fine pitch (= or < 1.0mm pitch) BGA packages, the stencil opening
may be reduced by 25−50 µm to allow for PCB-to-stencil misalignment. Thus,
this will prevent shorting of the solder to other balls. The sidewalls of the
aperture may be tapered for easier release of the paste.

Stencil thickness for BGAs normally range from 0.1 mm – 0.2 mm, depending
on the other fine pitch components on the board.

The practice for BGA stencils is to maintain a 3−1 aspect ratio; for example,
a 1.0-mm pitch BGA might use a 0.5-mm opening on a 0.15-mm thick stencil.

4.2.1.1 Solder Paste Type

Solder paste includes three main categories:

- Rosin mildly activated (RMA)

- Water-soluble organic acid (OA)
- No-clean

Each of these solder paste types may be used to mount flip chip BGA
packages. However, precautions should be taken to ensure water-soluble flux
residues are removed following reflow. Alternatively, system-level reliability
testing may be performed to ensure the acceptability of the flux residue for the
system application.

Table 7 lists the advantages and disadvantages of each category. Choosing

a solder paste category depends on the application and the product type.

Table 7. Solder Paste Types Used for Surface Mounting of BGA Devices
Type Advantages Disadvantages
RMA Stable chemistry Needs chemical solvent or saponification for cleaning
Good properties

OA Cleaned using pure water Humidity sensitive, seen as: short shelf and working life,
solder ball tendency
Very easily cleaned
Water leaches lead into waste stream

No- No cleaning process, equipment, or May leave some visible residue behind
clean chemicals
Eliminates effluent issues

40 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

4.2.2 Soldering Process

Similar to selecting auto-placement machines, selecting the type of soldering
process required depends on the type of components to be soldered, and
whether surface mount and through-hole parts will be combined.

The reflow method is used if all components are surface-mount types.

However, reflow soldering for surface-mount components followed by wave
soldering for through-hole mount components, is used for a combination of
through-hole and surface-mount components.

4.2.2.1 Infrared/Convective Reflow Soldering

The two basic types of reflow processes are:

- Focused (radiant)
- Non-focused (convective)

Focused IR (or lamp IR) uses quartz lamps that produce radiant energy to heat
the product.

In non-focused or diffused IR, the heat energy is transferred from heaters by

convection. A gradual heating of the assembly is necessary to drive off
volatiles from the solder paste. The gradual heating is accomplished by
various independently-controlled top and bottom heating zones. After an
appropriate time in preheat, the assembly is raised to the reflow temperature
for soldering, and then cooled.

The industry standard and most-widely accepted reflow method, forced

convection, is more suitable for SMT packages. Forced convection reflow
offers better heat transfer from hot air that is constantly being replenished in
large volume, thus supplying more consistent heating. Although large mass
devices on the PCB heat more slowly than low mass devices, the difference
is small enough that all parts have nearly the same heat cycle.

4.2.3 Coplanarity (Warpage)

Coplanarity is defined as the maximum distance from the highest ball to a
seating plane. This plane is formed by the three balls that the package would
rest on if placed on a perfectly flat surface. PCB coplanarity requirements are
directly related to the package size.

Most responsible PCB vendors take precautions to be well below the

0.010-mm specification recommended in the industry standard specifications.
The JEDEC standard for maximum allowable non-coplanarity is 0.15 mm
(5.91 mils), regardless of package size or pin count.

SPRU811 Flip Chip Ball Grid Array Package 41

SMT Assembly

BGA warpage is a serious concern affecting solder joint reliability. The

assembly yields of mounting BGA components are influenced by the PCB
properties and process control procedures followed by the manufacturer of the
PCB.
PCB material is a mixture of fiberglass and resin with copper tracks and vias,
as well as a solder-resist coating on top. All of these materials expand at
different rates during heating. If heating is unevenly applied, different sections
of the same material will expand at different rates.
This stress can lead to permanent distortion of the material. Warpage, which
is usually a result of the PCB buckling, can make it impossible to solder a new
device in the position where rework occurred. When this happens, the PCB is
a reject.
To better understand packages, researchers have tried to measure warpage
level directly by using simulation to evaluate package warpage in terms of
design and manufacturing factors. However, simulation requires verification,
including adjustments for assumptions made during analysis. For that reason,
three-dimensional measuring of the total deformation of complex objects,
rather than relative deformation, is necessary.
Shrinking pitch increases the likelihood that contact pressure at burn-in
temperatures will damage or mark the softened solder balls, leading to
coplanarity problems during assembly. For that reason, TI sockets grab the
side of the ball with a tweezing action, leaving the critical bottom area
untouched.
The lack of coplanarity is the result of two elements:
- Warpage of the overmolded substrate
- Differential substrate pad-to-solder ball heights

The substrate warpage is typically the major contributor to any lack of

coplanarity; the solder ball heights are relatively uniform. At room temperature,
the typical flip chip BGA has a slight upward curvature.
TI determines the coplanarity per the JEDEC standard, scanning all of the
BGA bumps and determining the relative positions of their height in space.
Software takes into account the center of mass of the part and then determines
which three or more balls the device would rest on. The distance from the
remaining ball tips to a plane formed by these three seating balls.
An automated system determines the following:
- Coplanarity to a best-fit plane
- Ball volumes
- Absence of balls
- Deviation of ball tips from the expected x-y grid

42 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

A more expensive and flexible system that also performs printed solder paste
height inspection is available.
In the case of the BGA package, where heating balls in the center of the
underside of the device is much slower, applying all of the heating to the top
of the board is not wise. Too much heating of the PCB in that area would cause
warpage.
Therefore, the PCB must also be heated from the underside to a given
temperature (depending on the board properties); preferably 80°C–145°C.
This temperature should be attained prior to the package itself reaching solder
reflow temperature. This would help minimize the rate of defects during the
assembly process.

4.3 Component Placement

To meet accuracy requirements, auto-placement machines are used to place
surface-mount components on the PCB. The type of parts to be placed and
their volume dictate the selection of the appropriate auto-placement machine.
These types of auto-placement machines are available on the market today:
- Inline
- Simultaneous
- Sequential
- Sequential/simultaneous
Inline placement equipment employs a series of fixed-position placement
stations. Each station places its respective component as the PCB moves
down the line. These machines can be very fast by ganging several in
sequence.
Simultaneous placement equipment places an entire array of components
onto the PCB at the same time.
Sequential placement machines are the most common high-speed machines
used in the industry and typically utilize a software-controlled X-Y moving table
system. Components are individually placed on the PCB in succession.
Sequential/simultaneous placement equipment features a software-controlled
X-Y moving table system. Components are individually placed on the PCB
from multiple heads in succession. Simultaneous firing of heads is possible.
Each of the four categories includes many models of auto-placement
equipment. Selection criteria should include:
- The kinds of parts to be handled
- Whether parts come in tube, trays, or tape and reel
- Whether the machine can accommodate future changes in other shipping
media

SPRU811 Flip Chip Ball Grid Array Package 43

SMT Assembly

Selection and evaluation of tapes from various vendors for compatibility with
the selected machine is very important. Off-line programming, teach mode,
and edit capability, as well as CAD/CAM compatibility, can be very desirable,
especially if a company has already developed a CAD/CAM database.
Special features, such as vision capability, adhesive application, component
testing, PCB handling, and capability for additional expansion may be of
interest for many applications.
Vision capability is especially helpful to accurately place fine-pitch BGA
packages. Machine reliability, accuracy of placement, and easy maintenance
are important to all users.

4.4 Solder Reflow

Solder reflow conditions are the next critical step in the mounting process. The
reflow process includes the following steps:
1) Solvent in the solder paste evaporates
2) Flux cleans the metal surfaces
3) Solder particles melt
4) Surfaces become wet from the wicking of molten solder
5) Solder balls collapse
6) Solder solidifies into a strong metallurgical bond
The desired end result is a uniform solder structure strongly bonded to both
the PCB and the package with small or no voids, and a smooth, even fillet at
both ends. Conversely, when all the steps do not carefully fit together, voids,
gaps, uneven joint thickness, discontinuities, and insufficient fillet can occur.
Although the exact cycle used depends on the reflow system and paste
composition, all successful cycles have several key points in common:
- The cycle includes a warm-up period sufficient to safely evaporate the
solvent. This can be done with a pre-heat, a bake, or (more commonly) a
hold in the cycle at evaporation temperatures.
If there is less solvent in the paste (such as in a high-viscosity,
high-metal-content paste), the hold can be shorter. However, if the hold is
not long enough to remove all of the solvent or too fast to allow it to
evaporate, undesired results may be obtained, ranging from
solder-particle splatter to trapped gases that can cause voids and
embrittlement. A significant number of reliability problems with solder
joints can be avoided with the warm-up step, which needs careful
attention.
- Successful reflow cycles include uniform heating across the package and
the board. Uneven solder thickness and non-uniform solder joints may be
an indicator that the profile needs adjustment.

44 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

A problem also occurs when different sized components are reflowed at

the same time. When profiling an oven, ensure that the indicated
temperatures represent what the most difficult-to-reflow parts are
experiencing. These problems are more pronounced with some reflow
methods, such as infrared (IR) reflow, than with others, such as forced
hot-air convection.

- Finally, successful reflow cycles strike a balance among temperature,

timing, and length of cycle. Mistiming can lead to excessive fluxing
activation, oxidation, excessive voiding, or even damage to the package.
Heating the paste too hot and too fast before it melts can also dry the
paste, which leads to poor wetting. Process development is needed to
optimize reflow profiles for each solder paste/flux combination.

Table 8 lists the typical stages and characteristics on a reflow profile.

Table 8. Typical Stages and Characteristics on a Reflow Profile

Reflow Zones Characteristics Process window
Pre-heat Initial heating of the component/board, to 1.5°C–3°C/second,
avoid thermal gradients 120°C–40°C peak temp

Soak Flux activation zone, volatiles in paste 60–180 seconds soak,

evaporate, facilitates removal of oxides 120°C–70°C peak temp (follow solder paste
manufacturer recommendation)

Reflow Solder melting/collapse occurs above 60–90 seconds above 183°C, 220°C ± 5°C
183°C, solidification on cooling below 183°C peak component temperature

Cool down Assembly cooling zone 2°C–3°C/second to room temp

Figure 22 shows an ideal Sn63:Pb37 solder reflow profile for fine pitch
package surface mounting on a FR-4 PCB. Nitrogen-purged, convection
reflow is advantageous during this assembly to minimize the possibility of
solder ball formation under the package body.

SPRU811 Flip Chip Ball Grid Array Package 45

SMT Assembly

Figure 22. Ideal Reflow Profile for Eutectic Solder

Ideal reflow profile

Temperature ( oC) 300

200

100

0
0 100 200 300
Time (sec)

Note: This is an ideal profile, and actual conditions obtained in any specific reflow oven will vary. This profile is based on convec-
tion or RF plus forced convection heating.

Although this profile corresponds to the ramp to 140°C-soak-ramp to peak

temperature-cool-down profile, the faster triangular ramp to peak
temperature-cool-down profile is also often used.

In general, you should establish detailed thermal reflow profiling to ensure that
all of the solder joints in the package have completely reflowed. The profile
board must be similar to the actual production board in that the PCB thickness
and construction must be representative, and If possible, simulate the effect
of other surrounding components, especially high-thermal mass components.

X-ray inspection of the solder joint after SMT assembly is strongly

recommended to ensure that ball shorting has not occurred, and that solder
joint voiding is within acceptable limits.

Figure 23 shows the recommended reflow profile for SnAgCu solder. This
profile is provided as a reference. The same recommendations apply for
defining a thermal reflow profile that best suits your system board
characteristics.

46 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

Figure 23. Recommended Lead-Free Reflow Profile for SnAgCu Solder Paste

Peak temperature
260 °C max
260
Temperature ( oC)

235
225
200
30−60 sec.
150
90 +/− 30 sec.

1−5 degC/sec

Time
Reflow temperature is defined at package top

4.5 Defluxing (Cleaning)

In general, cleaning SMT assemblies is harder than that of conventional
assemblies because of smaller gaps between surface-mount components
and the PCB surface. The smaller gap can entrap flux, which can cause
corrosion and lead to reliability problems.
Thus, the cleaning process depends on the following:
- Spacing between component solder balls
- Spacing between component and substrate
- Source of flux residue
- Type of flux
- Soldering process
Rosin mildly activated (RMA) cleaning requires chemicals to clean up the
waste.
Water-soluble organic acid (OA) cleaning uses water that must flush down the
drain. However, lead is often found in the waste water in this chemistry and
creates an environmental concern.
No-clean is generally the preferred solder process because it eliminates
cleaning altogether, which further eliminates environmental issues and
reduces capital costs.
See section 4.2.1.1 for further discussion of solder paste type.
A key SMT issue is determining the cleanliness of SMT assemblies. An
Omega meter or Ionograph are two commonly used tools for assessing
average board cleanliness.

SPRU811 Flip Chip Ball Grid Array Package 47

SMT Assembly

The industry also uses surface insulation resistance (SIR) surface mount
boards. These boards check for ionic contaminates left on the PCB by
measuring the electrical resistance between adjacent traces or circuits.

5 Repair and Rework

Repair and rework of SMT assemblies is easier than for conventional
components. A number of tools can remove components, including hot-air
machines for removing active surface mount components.

As with any rework tool, a key issue in using hot-air machines is preventing
thermal damage to the component or adjacent components. Regardless of
which tool is used, all of the controlling desoldering/soldering variables should
be studied, including the number of times a component can be removed and
replaced, and desoldering temperature and time.

It is also helpful to preheat the board assembly to 150°F–200°F for 15 to 20

minutes before rework. This will prevent thermal damage such as measling or
white spots of the boards, and to avoid pressure on the pads during the rework
operation.

To prevent moisture-induced damage, SMT components may require

bake-out prior to removal from the board.

Preparing PCBs and Packages for Rework

Both the PCB and SMT devices to be reworked can absorb moisture from the
ambient air, which can cause internal expansion and damage to the PCB
and/or device during heating to the de-soldering temperature. Therefore, you
must always bake PCBs and devices prior to any rework.

The recommended temperature depends on the maximum temperature that

the devices and PCB can withstand without damage. Generally, the
recommended bake conditions for FCBGA packages are 8 to 24 hours at
105°C−125°C.

5.1 TI Recommendation
Reworking flip chip BGA packages attached to PCB assemblies using solder
or epoxy attachment can present significant challenges, depending on the
starting point at which the rework is to be accomplished.

Tests of rework procedures to date indicate that component removal from the
PCB is successful with all of the conventional techniques used in the industry
today.

48 Flip Chip Ball Grid Array Package SPRU811

 SMT Assembly

TI follows the following steps for solder attached components in the rework or
repair process:

1) Unsolder the old component from the board.

2) Remove any remaining solder from the part location.
3) Clean the PCB assembly.
4) Tin the lands on the PCB or apply solder paste to the lands on the PCB.
5) Target, align, and place new component on the PCB.
6) Reflow the new component on the PCB.
7) Clean the PCB assembly.

High CTE Ceramic Reflow Rework

For component rework in large I/O BGAs, you must use solder paste and a
mini-stencil for high-assembly yields; that is, avoid a flux-only process.

After site cleaning or dressing (using a solder wick or solder vacuum tool) and
paste printing, component assembly is done at a rework station equipped with
a hot-air nozzle and an arrangement for bottom-side heating (global preheat
with an IR heater; local preheat using nozzle).

An appropriate nozzle size should be selected (or custom-built, if not

available) to ensure uniform heating across the entire unit (corner-to-center)
during the reflow process.

It is highly recommended that bottom-side preheat be used to:

- Avoid the high thermal gradients that can damage the PCB and cause
localized warpage.
- Prevent over-heating-related damage to the component itself and to
adjacent components.

As was done for convection oven SMT assembly, detailed thermal reflow
profiling must be performed to develop a reflow profile with similar
characteristics as the SMT profile. Figure 24 shows an example of a thermal
reflow profile.

SPRU811 Flip Chip Ball Grid Array Package 49

 SMT Assembly

Figure 24. Thermal Reflow Profile

Rework profile 1
350
Top heater
Bottom heater
300 PWB
Corner
Temperature ( o C)

Center
250 Reflow

200

150

100

50

0
0 50 100 150 200 250 300 350
Time (sec)

50 Flip Chip Ball Grid Array Package SPRU811

 Mechanical Assembly

6 Mechanical Assembly

6.1 External Heat Sink Attach

This section applies to application of thermal management solutions for
FCBGA packages where package-level cooling alone has been deemed
insufficient.

There are package considerations that can improve the effectiveness of

external heat sinks, which are attached to the top of the package. In this case,
the thermal conduction path between the die and the top of the package is
more critical than the conduction path to the PCB (see Figure 25).

In fact, for very high-power designs, the thermal paths to the PCB can be
completely neglected in analysis because of the small fraction of heat they can
dissipate. The package can be thermally enhanced by the appropriate
selection of the following:

- Lid with high thermal conductivity

- Thin die attach with high thermal conductivity
- Thickness of the die (depending on the uniformity of the power distribution
on the die)

Figure 25. Major Thermal Conduction Paths to Optimize Thermal Dissipation

For moderate power dissipation (less than 6 watts), using passive heat sinks
and heat spreaders attached with thermally conductive double-sided tapes or
retainers, can offer quick thermal solutions in these packages.

A number of heat-sink vendors supply these passive heat sinks and heat
spreaders in low profiles. The airflow profile over the part (i.e., unidirectional,
circling, varying) should also be considered.

In cases of moderate power dissipation, connecting the package to a metal

chassis may also be an effective option. A gap filler material provides a
conduction path between the top of the package and the metal chassis. This
can be a effective lower-cost option in low-profile, low-airflow systems.

SPRU811 Flip Chip Ball Grid Array Package 51

Mechanical Assembly

Lightweight finned external passive heat sinks can be effective for dissipating
10 watts or more in the larger packages. However, an area of concern with
these heat sinks is that the more efficient versions tend to be tall and heavy
and, in some cases, spring-loaded to provide a high-pressure contact between
the heat sink and the top of the package.

This compressive loading should be considered in the reliability of the

package. To help prevent component joint fatigue from heat sink-induced
stress cracks, use fixtures that transfer the mounting stress to a circuit board.

The diagonals of some of these heat sinks can be designed with extensions
to allow direct connection to the board. Back plates can reduce the bending
stress on the board. TI recommends keeping the compressive loading by a
heat sink or other attachment below 0.015 lbfper BGA ball.

Active heat sinks can include simple heat sink configurations incorporating a
mini fan, heat pipe, or even Peltier thermoelectric coolers (TECs) with a fan
to carry away any heat that is generated. Before applying a TEC in heat
management, consult with experts. These devices can be reversed, can
damage components, and have condensation-related issues.

52 Flip Chip Ball Grid Array Package SPRU811

 Troubleshooting

7 Troubleshooting
This section provides guidelines for identifying the most common problems
that can arise during the mounting of flip chip BGA packages. The following
common defects are associated with BGA packages:

- Bridging
- Opens
- Missing solder balls
- Misalignment
- Solder voids
- Cracking
- Partially soldered joints
- Contamination
- Excess flux residue
- Ratcheting (i.e., balls that accidentally move during reflow or cooling and
sit at an angle relative to the device)
- General faults in the surface structure of solder balls

The problem with reliably and accurately identifying these defects is that they
won’t necessarily look the same as their SMT equivalents. Furthermore,
solder joints tend to look different on inner rows compared to outer ones.

Table 9 summarizes the most common defects found during SMT assembly
and their probable causes.

Table 9. Typical Defects Found During SMT Assembly and Probable Causes

Observation Explanation Probable Causes

Insufficient or no Poor fusing between solder - Uneven land and BGA temperatures
solder joint paste and BGA land - Solder ball coplanarity
- Insufficient wetting time
- Insufficient or old solder paste
- Peak reflow solder ball temperature too low
- Poor solderability of solder balls or lands

Bridges and Solder connecting or partially - Excessive solder paste

icicles connecting adjacent BGA - Excessive component placement pressure.
balls or lands - Excessive component and/or PCB warpage during
SMT assembly
- Solder paste misplacement
- Solder paste integrity
- PCB vibrations during soldering
- Land metallization integrity
- Excessively large voids in solder balls

SPRU811 Flip Chip Ball Grid Array Package 53

Troubleshooting

Table 9. Typical Defects Found During SMT Assembly and Probable Causes
(Continued)
Observation Explanation Probable Causes
Dewetting Solder does not adhere to - Poor solderability of lands
ball or land; lifting of BGA - Poor solderability of balls
balls - Solder paste integrity
- Land plating integrity
- Apparent dewetting when excessive PCB warpage oc-
curs while solder balls are at a temperature greater
than 160_C
- Excessive package and/or PCB warpage during SMT
assembly – leads to non contact with PCB lands

Solder balls Solder agglomerates on land - Solder paste displacement

or in adjacent PCB area - Solder paste integrity
- Insufficient pre-heat
- Solder splattered due to excessive heating rate

Package integrity Excessive expansion of - Excessive humidity during exposure of the devices to
failure such absorbed moisture has ambient
doming or separated internal package - Out of bag time was exceeded
cracking parts and deformed the - Excessive exposure time of devices to ambient time
plastic body - Excessive humidity absorption of devices during trans-
port or before dispatch

Voids in BGA Voids in the BGA ball, which - Plugged via under pad
device could be near the PCB/solder - Inadequate reflow parameters (temperature, time)
ball interface or near the - Trapped flux in the solder paste, which may be caused
component substrate/solder by a significant excess of the following: hot reflow pro-
ball interface. X-rays on the file, small past powder size, high paste solvent volatili-
cross-sectioned part could be ty, high paste metal content
used to detect the voids.

Other important SMT recommendations are:

- The thermal profile selected and set up should be consistent with the
properties of the solder paste used.
- The solder paste must not dry out too much during the time that the PCB
is stored prior to reflow.
- The solder paste must not slump excessively.
- The size and distribution of solder balls in the paste must be compatible
with stencil-printer minimum dimensions.
- The solder paste balls must not be excessively oxidized or deviate from
a spherical shape.
- The quantity deposited by the printing machine must be reproducible.
Inspection and measurement may improve the prediction of the optimum
stencil cleaning interval and paste replacement interval.

54 Flip Chip Ball Grid Array Package SPRU811

 Troubleshooting

- The pre-flow time and temperature must achieve activation of the flux but
not excessively deplete the flux content; else adequate cleaning action
prior to solder joint formation may not occur.
- The peak temperature must not be so high that the flux is burned, if it has
to be cleaned off afterwards, nor must it allow the solder to wick up the
solder balls of components and so starve the joints. The temperature
difference between solder balls and lands also influences this effect.

7.1 Non-Destructive Failure Analysis at the SMT Level

Array packages typically account for approximately 10% of all devices
analyzed during PCB inspection, but this percentage is increasing.

Unlike the connections on conventional SMT devices, the connections on an

array package are hidden beneath the package. Thus, traditional automatic
optical inspection (AOI) systems cannot inspect the joints after reflow,
because the cameras cannot detect them through the body of the package.

Additionally, the AOI systems cannot be adapted to view from the side
because of the extremely low standoff heights and invariably ultra-close
proximity of adjacent components.

The most commonly-used, non-destructive techniques recommended by TI

for defect identification at the SMT level are:

- X-rays
- Electrical curve tracing
- Time domain reflectometry (TDR)
- Scanning acoustic microscopy (SAM)

Endoscopic optical Inspection is also available.

Real Time X-Rays

X-ray inspection can be used during assembly process development and for
failure analysis. Because of the atomic density of the lead in the solder joints,
and standard-resolution, real-time X-ray systems can only reveal shorts and
missing or double balls that are readily observable.

More subtle joint assembly defects, such as voids, total wetting of the
motherboard pad (full or partial opens), and solder splattering/balling, require
more sophisticated detection systems.

As with any array package, perimeter joints can be readily inspected; however,
interior joints are much more difficult to inspect. X-ray laminography systems
can be used for inner joint inspections.

SPRU811 Flip Chip Ball Grid Array Package 55

Troubleshooting

Endoscopic Optical Inspection

Endoscope technology is adapted from the medical industry, where robust

mechanisms were developed to look inside the human body at joints and
tissue. In electronics assembly, endoscope techniques allow full inspection of
the underside of low standoff array packages (down to 0.05 mm and 0.8 mm
of space between devices).

With endoscopic systems, it is possible to see:

- Approximately 100 percent of outside balls

- 60–80 percent of second row balls
- 30–40 percent of third row balls
- 5–20 percent of fourth to sixth row balls
- Outside edges of any remaining balls

Technicians used to inspecting SMT solder joints might not recognize the
partially obscured rows of solder ball joints the first time they look under a BGA.
If they have used an X-ray inspection, their boards might have passed
inspections of solder balls located in the right place; no excess solder, and no
bridging.

Yet when they look beneath the same boards using the endoscope method,
they will see what an X-ray cannot reveal: a landscape of green colored
residues or debris, indicating an excess flux or contamination problem. This
is an extremely common scenario.

X-ray inspection systems look down through an array package to pick out the
shape of higher density material, such as solder joints. The images contain
essential information about the soldering process, in particular faults, such as
bridges, misalignment and voids that visibly alter the overall shape of a solder
ball. However, equally serious defects, such as opens, cold solder joints,
excess flux, and excessive contamination can be more difficult to discern,
even with high-resolution equipment.

Therefore, an X-ray cannot provide a complete assessment of solder joint

quality and all of the potential defects of an array device. X-ray inspection is
also considerably more expensive than benchtop endoscopic optical
inspection systems. Nevertheless, benchtop endoscopic optical inspection
systems are not intended to directly replace X-ray inspection systems, which
have their own strengths (in particular, automated throughput speed).

56 Flip Chip Ball Grid Array Package SPRU811

 Troubleshooting

Table 10 lists defects that optical inspection cannot identify.

Table 10. X-Ray Versus Optical Inspection Defect Detection

(Courtesy of Metcal)

X-Ray Optical
View Inspection Inspection
Placement Yes Yes

Bridging Yes Yes

Show Voids Yes −

Cold Solder Joints Possible † Yes

Reflow Problems Possible † Yes

Empties Possible † Yes

Excess Flux − Yes

Contamination − Yes
† With extensive training

Optical inspection is better suited to R&D and low-to-medium volume,

high-mix manufacturing environments. X-rays makes better inline solutions in
high volume, low mix environments.

Optical inspection reliably detects the vast majority of problems quickly and
easily. X-ray inspection is the next step up for manufacturers with volumes that
justify the amount of capital investment required, although optical is still
required to guarantee process quality. Combining both techniques provides
full inspection coverage. In high-volume processes, this means using X-ray
inspection supported by off-line optical inspection sampling.

Scanning Acoustic Microscopy (SAM)

The scanning acoustic microscope (SAM) has also emerged as a valuable

evaluation tool for failure analysis. C-mode SAM (C-SAM) can demonstrate
non-destructive package analysis while imaging the internal features of the
package.

Ultrasonic waves are very sensitive, particularly when they encounter density
variations at surfaces; for example, variations such as voids or delamination
similar to air gaps.

C-SAM images of voids, cracks, disbands, and delamination provide high

contrast and are easily distinguished from the background. The most
important feature of this type of analysis is that it is non-destructive and

SPRU811 Flip Chip Ball Grid Array Package 57

Troubleshooting

provides the failure analyst with opportunities for additional electrical testing,
if required.

Time Domain Reflectometry (TDR)

TDR is increasingly utilized as a failure analysis tool in the semiconductor

industry. TDR can provide fast, non-destructive analysis of packaged
integrated circuits. With one measurement, TDR analysis can provide instant
identification of the general region of the fail site, and whether it exists in the
die, substrate, interconnect region, or in the PCB.

The way TDR works in general is as follows: a digital sampling oscilloscope

with a TDR module supplies a fast rise-time voltage edge to the signal pin of
interest, and then records the subsequent voltage edge reflections. The time
delay between the incident and reflected electrical signals is analyzed to
characterize the electrical path of the signal pin.

TDR analysis offers the following advantages:

- Provides results within minutes

- Accurately detects the fail site
- Amenable to automation
- Non-destructive technique

TDR can be used as a complementary technique to X-ray and SAM analysis.

Figure 26 and Figure 27 illustrate TDR schematics for die-substrate-PCB and
waveforms for flip chip BGA, respectively.

Figure 26. Schematic of a Die-Substrate-PCB System Showing Circuit Loop for TDR
Analysis

Die
Solder bumps

Substrate

Solder balls

PCB

Location 2 Location 3

Location 1

Connector

58 Flip Chip Ball Grid Array Package SPRU811

 Troubleshooting

Figure 27. Schematic of TDR Waveforms for a Flip Chip BGA Package.
0.1
Probe tip
Substrate only
Flip chip package
0
Voltage (V)

−0.1

−0.2

−0.3
0 200 400 600 800 1000
Time (ps)

Interconnect and die

Substrate

7.2 Destructive Failure Analysis at the SMT Level

The techniques described below can be used to physically and visually
confirm failures, which have been previously identified by non-destructive
means.

Dye-and-Pry

The dye-and-pry technique is a destructive failure analysis technique

commonly used to determine the following problems:

- Any non-wetting of the BGA balls to the PCB pads

- Any cracks within the BGA ball or at BGA/PCB pad interface or at
BGA/device pad interface

This technique can be applied while the device is still mounted on the PCB.

Example: To investigate whether a defect exists at the BGA-PCB

interconnect, apply the dye around the solder joint area and on the solder joint
itself, making sure it penetrates and marks the area of interest. After the dye
has dried, pry the device off of the PCB and observe if there are any areas
where cracks or non-wetted surfaces exist.

SPRU811 Flip Chip Ball Grid Array Package 59

Troubleshooting

Microsectioning/Parallel Lapping

In addition to dry-and-pry, component/PCB microsectioning or parallel lapping

can be used to help identify the root cause of failure of a mounted component.
This technique requires a significant level of training and expertise in order to
prevent any further damage induced during cross-sectioning (i.e.,
grinding/polishing wheels), or that might destroy any evidence leading to the
potential root cause(s) of failure.

Both techniques mentioned above should be applied only after all other
non-destructive techniques have been exhausted in efforts to identify the root
cause of failure. Destructive techniques will damage the part(s) being
analyzed to the point of rendering them functionally useless.

7.3 Component Removal for Analysis

The following steps are needed to remove a component for analysis:

1) Remove the BGA package with a hot gas tool that is usually fitted with a
custom head sized to the BGA package. Proper sizing of the gas head
reduces the thermal impact on adjacent packages.

Correct tool settings depend on the tool being used, the package being
removed, and the PCB. Determining the settings is an exercise in profiling,
similar to initial reflow.

2) Use a profile assembly with thermocouples mounted in solder joints to

determine tool settings that ensure proper reflow of all solder joints.
Monitor both the top and bottom of the PCB.

3) To remove the component from the PCB, use a vacuum nozzle within or
integral to the hot gas head. When the part is hot enough for removal, that
is, solder is molten, you can use vacuum wands or pens (either integral
to the machine or attached as a hand-held accessory) to remove
components from the PCB assembly.

The gentle nature of a vacuum lift usually prevents damage to surface

mount pads. Although the vacuum grip is just strong enough to overcome
the surface tension of molten solder and to lift the component away, the
grip will not hold if solid solder connections remain, except with very fine
pitch solder balls and tiny pads.

4) To avoid damage to the profile card when profiling, shut the vacuum off so
the component is not removed. Control the pressure of the head down
onto the component during removal. If pressure is applied after the solder

60 Flip Chip Ball Grid Array Package SPRU811

 Troubleshooting

balls are melted, the solder will be pressed between the plates of substrate
and PCB, resulting in bridging that must be removed manually. Two
possible solutions are to:
J Establish the head height prior to reflow and control the stroke.
J Place shims under the edges of the component to prevent collapse.

5) Consider the effects on other components. If other SMT packages are

near the package being reworked, monitor their solder joint temperature.
If the temperature approaches reflow temperatures, shielding may be
necessary.

Preheating the PCB assembly is good practice when reworking BGA

packages and offers the following advantages:

- Reduces the heating time required using the rework head. If one PCB
assembly can be preheated while another is reworked, cycle time can be
greatly reduced.

- Achieves more uniform profiles. Preheating reduces the temperature

spread between center and edge solder joints by bringing the baseline
temperature closer to the reflow temperature.

- Minimizes PCB warpage. Because warpage is caused by the higher local

temperature at the surrounding area, raising the PCB assembly
temperature minimizes the mismatch and reduces warpage.

- Reduces problems with adjacent components by allowing shorter gas

heat times or lower temperatures to be used, thus reducing the risk of
affecting neighboring solder joints.

SPRU811 Flip Chip Ball Grid Array Package 61

Other Items

8 Other Items

8.1 Moisture Sensitivity of Surface Mount and BGA Packages

Most plastic BGA (PBGA) components are highly sensitive to moisture
exposure before the reflow temperature exposure. Maintaining proper control
of moisture uptake in components is critical in preventing “pop corning” of the
package body or encapsulation material.

Before shipping, flip chip BGA packages are baked dry and enclosed in a
sealed desiccant bag with a desiccant pouch and a humidity indicator card
(HIC). Most flip chip BGA components are classified as level three or level four
for moisture sensitivity per the IPC/JEDEC Spec J-STD-020, Moisture/Reflow
Sensitivity Calculation of Plastic Surface Mount Devices.

With most surface mount components, if the units absorb moisture beyond
their out-of-bag times for their moisture rating, damage can occur during the
reflow process. Package preconditioning methods and moisture sensitivity
requirements are explained in section 8.1.1, Recommended Baking Conditions.

Before opening the shipping bag and attempting solder reflow, you should
understand the moisture sensitivity of the packages to maintain a minimal
out-of-bag time and ensure the highest possible package reliability for the final
product.

If the previously bagged product cannot be mounted before the elapsed

out-of-bag time for that product, you can re-bake the parts. Another option is
to store the opened units in a nitrogen cabinet or dry box until needed. Placing
units in a dry box effectively stops the clock.

Packaged devices continue to gain moisture even after board mounting.

Components needing rework must be completely processed through all
thermal exposures before the original out-of bag limits are reached.

If this is not possible, or the time allotment is not strictly followed, you must
bake-out of the completed boards before subjecting the components to the
heat of the rework process.

Products being removed from boards returned from the field for failure
analysis must be baked dry before heat exposure. If this step is skipped,
massive damage to the component results, rendering useless efforts to
determine the cause of failure.

Moisture-sensitive SMDs packed in tubes, trays, or reels are first dried during
the assembly process and then sealed in damp-proof bags with a desiccant
and humidity indicator card.

62 Flip Chip Ball Grid Array Package SPRU811

 Other Items

The corresponding moisture sensitivity level (MSL) is printed on the product

label. A warning label on the product packing summarizes the safe handling
instructions and product usage.

After opening the dry bag, the moisture indicator must not exceed 20 percent.
The product must be exposed to the surface mount soldering process within
the time specified for the corresponding MSL. Storage conditions must be
30_C/60 percent relative humidity, maximum shelf life period.

If parts cannot be used in the specified shelf life period, they can be placed in
a dry box (<20 percent) or resealed hermetically before the period is expired.
It is advisable to indicate the new shelf life on the packing label as a difference
between the original shelf life and the time they have already been exposed
to ambient conditions.

In two cases, the SMDs must be redried according to the instructions given in
the following section 8.1.1, Recommended Baking Conditions:

- When the humidity indicator shows a moisture content higher than 20

percent
- When the parts are removed from dry-pack and not used within the
specified period

8.1.1 Recommended Baking Conditions

Dry-bake is required to ensure that a package has the minimum amount of
moisture possible at the moment it is packed for shipping. The low moisture
guarantees the reliability of the part during the mounting process.

When a part is qualified for reliability to a certain MSL, it assumes the part
starts from a dry condition. From that, a moisture exposure level is assigned.

J-STD-020B defines the conditions to obtain a dry package as 24 hours @

125°C. Package dryness may be achieved in shorter times and lower
temperatures depending on package dimensions and materials.

Dry-bake is performed only once and only if devices are transferred to plastic
or metal carriers that are able to withstand 125°C (bake-able carriers).

For plastic SMDs with a package thickness of 1.4 mm–1.7 mm (i.e., TQFP,
SSOP), baking time can be reduced to 12 hours. For plastic SMDs where the
package thickness is 1 mm or less (i.e., TSOP, TSSOP), baking time can be
reduced to six hours.

For devices left in their tubes, reels, or trays, the recommended dry-bake is
40°C/<5% RH for 192 hours. After drying, seal in damp-proof bag with a
desiccant and humidity indicator card.

SPRU811 Flip Chip Ball Grid Array Package 63

Other Items

In SMT, semiconductor devices are soldered on the surface of PCBs using

three techniques:

- Wave soldering
- Vapor phase soldering
- Infrared (IR) soldering

Soldering temperature ranges between 210°C and 260°C; therefore for a

relatively long time (longer than 120 seconds) this condition exceeds the
maximum working temperature of 150°C for plastic encapsulated devices.

In the early use of SMT, the high-temperature shock damaged a wide number
of SMDs. The “pop corn effect” on SMDs caused by high-temperature damage
became one of the most studied issues for specialists of electronic packaging
and surface mounting.

After several years of continuous progress, the “pop corn effect” is now
understood and a number of solutions have been developed. The effect can
be explained as follows:

1) During surface mount soldering, the combined effect of high temperature

and moisture absorbed in the encapsulation can generate excessive
mechanical stress inside the package.
The stress is caused by internal moisture pressure at the soldering
temperature and can be reduced by minimizing the moisture content of the
SMD before soldering on the board.

2) Mechanical stress caused by the absorbed moisture can cause damage

to the package, such as cracks and delamination. The stress is more
critical in large semiconductor chips and in thin packages, depending also
on the thermo-mechanical properties of the encapsulation materials at the
surface mount process temperature.

3) In some cases, when cracks and delamination affect critical areas like die
surface and wire bonding, long-term reliability may be compromised.

To withstand the stress associated with the surface mount process, the
industry developed new package structures and molding compounds. The
robustness of SMDs has been greatly improved in the last few years.

However, a number of SMDs still require moisture content in the encapsulation

to be minimized before the devices are subjected to the soldering process.

Shipping and storing sensitive SMDs in damp-proof bags that are hermetically
sealed reduce SMDs’ moisture content. These bags can control moisture
absorption and maintain devices in a dry environment until used.

64 Flip Chip Ball Grid Array Package SPRU811

 Other Items

The shelf life of the device must be quantified after removal from the hermetic
bag (that is, the time left to the SMT operator for mounting the units, once the
damp-proof protection is removed). For practical reasons, shelf life is
requested to be as long as possible, in excess of several days.

JEDEC J-STD, published by JEDEC and by the Institute for Interconnecting

and Packaging Electronic Circuits (IPC), defines up to six MSLs and their
associated shelf life at a specified ambient humidity and temperature. These
conditions represent the typical environment in the factory. Refer to the JEDEC
publication for further definition of moisture sensitivity levels.

The MSLs are defined as follows:

- MSL 1: Units are not moisture sensitive and can be exposed to ambient
moisture indefinitely. Because no dry-pack is needed, they are shipped in
non-hermetic shielding bags.
- MSL 2: Units have a shelf life of one year at 30°C/60% RH after removal
from dry-pack.
- MSL 3: Units have a shelf life of one week (168h) at 30°C/60% RH after
removal from dry-pack.
- MSL 4: Units have a shelf life of 72 hours at 30°C/60% RH after removal
from dry-pack.
- MSL 5: Units have a shelf life of 24-48 hours at 30°C/60% RH after removal
from dry-pack.
- MSL 6: Units are very sensitive to moisture, must be dried at 125°C/24
hours, and used immediately within 6 hours.

With most surface mount components, if the units are allowed to absorb
moisture beyond the shelf (or floor) life for their moisture rating, damage can
occur during the reflow process.

Before opening the shipping bag and attempting solder reflow, you should
understand the moisture sensitivity of the packages to maintain a minimal
out-of-bag time and ensure the highest possible package reliability for the final
product.

If the previously bagged product cannot be mounted before the elapsed

out-of-bag time for that product, you can re-bake the parts. Another option is
to store the opened units in a nitrogen cabinet or dry box until needed. Placing
units in a dry box effectively stops the clock. Packages continue to gain
moisture even after board mounting.

Components that need to be reworked must be completely processed through

all thermal exposures before the original shelf-life limits are reached. If this is
not possible, or the time allotment is not strictly tracked, the boards must be
baked before subjecting the components to the heat of the rework process.

SPRU811 Flip Chip Ball Grid Array Package 65

Other Items

To remove devices from boards, which have been returned from the field for
failure analysis, the boards must be baked before rework heat exposure. If the
boards are not baked, massive damage to the component results, rendering
useless any further efforts at determining the cause of failure.

8.1.2 Handling
The following steps detail the handling procedures to use with plastic surface
mount devices (PSMDs) packed in desiccant bags and intended for surface
mount applications. Follow these handling guidelines to ensure that
components maintain their as-shipped dry state, alleviating package cracking
and other moisture-related, stress-induced concerns.

1) Incoming inspection. On receipt, inspect shipments for a seal date within

the last six months. Verify bag integrity to ensure the absence of holes,
gouges, tears, or punctures of any kind that expose either the contents or
an inner layer of the bag.
Review the barcode label for conformance to the purchase order, but do
not open the bag until the contents are ready to be used (either inspected
or board-mounted).
Please see Table 11 Moisture Classification Level and Floor Life for details
on allowable exposure times once devices are removed from the bag or
exposed to the ambient. You can also refer to the MSL definitions in
section 8.1.1, Recommended Baking Conditions.

2) Storage conditions/shelf life. The SMT operator receives components in

the sealed moisture barrier bag (MBB) between 0 and 6 months after the
seal date indicated on the Desiccant Barcode label on the bag.
The sealed bag and enclosed desiccant are designed to provide a
minimum of 12 months of storage from the seal date in an environment as
extreme as 40°C and 90% relative humidity. The SMT operator has at
least six months of shelf life available on the components without the need
to rebake them.
If the worst-case storage conditions (time, temperature, or relative
humidity) are exceeded and you must verify whether inventory has been
affected, a bag can be opened and the HIC checked for expiration.
If the HIC has not expired, new desiccant can be added and the bag
resealed. If the HIC has expired, perform one of the following procedures
on the devices:
J Re-bake and use in manufacturing within the guidelines outlined in the
section 8.1.2, step 6, Re-Baking.
J Re-bake and reseal in an MBB with fresh desiccant.

66 Flip Chip Ball Grid Array Package SPRU811

 Other Items

J Re-bake and store in an environment of = 10% RH before using them

in a surface mount process.
3) Opening MBBs. To open a moisture barrier bag when the contents are
ready to be used or inspected, cut across the top of the bag as close to the
seal as possible, being careful not to damage the enclosed materials.
By cutting close to the seal, you allow as much room as possible for
resealing. After the bag is open, follow the guidelines for ambient
exposure time in section 8.1.3, Floor Life, to ensure that the devices are
maintained below the critical moisture level.
4) Manufacturing Conditions/Floor Life. TI classifies SMDs according to
levels of moisture sensitivity based on exposure time and environment.
The latest information in the literature indicates that percent weight gain
moisture content is not useful other than for evaluation.
Different package types/die attach area/lead count combinations have
different levels of absorbed moisture at which floor life limitations are
exceeded. Therefore, TI recommends that units be classified by allowable
exposure times. The label on the MBB lists the moisture sensitivity level
and the allowable floor life.
5) In-Process Storage. TI highly recommends having dry storage capability
available for units that will not be used within the allowable exposure time.
A desiccator with dry nitrogen or air (= 5 percent RH source) is suggested
for such storage.
6) Re-Baking. PSMDs should be re-baked only if they have been exposed
to excessive moisture by exceeding the recommended ambient exposure
time or by expiration of the HIC.
7) Resealing Moisture Barrier Bags. If resealing an MBB is needed for any
reason, TI recommends the following guidelines to ensure that the bag
seal does not allow moisture into the bag.
J The integrity of the seal is vital to the storage life of the devices. Make
sure the seal area does not deviate from a seal pressure of 60–70 psi
and a seal time of 3-4 seconds at approximately 225°C.
J Once the barrier bag is open, TI recommends that components be
surface mounted and reflowed within the time indicated on the MBB
label. This time is based on a manufacturing environment not more
extreme than 30°C/60% RH and a maximum component body
temperature during solder reflow of 220°C.
If the components cannot be mounted within this time, they should be
put in a dry storage environment immediately or sealed in a MBB with
fresh desiccant as soon as possible.

SPRU811 Flip Chip Ball Grid Array Package 67

Other Items

In either case, the remaining allowable shelf time must be reduced by

the time the units are out of the MBB or dry storage environment.

For more information on handling moisture sensitive devices, see the

IPC/JEDEC J-STD-033A document or contact your local TI Sales Office.

8.1.3 Floor Life

Table 11 lists the floor life of SMDs. Floor life is modified by environmental
conditions other than +30°C/60% RH. Use to determine the maximum
allowable time before re-bake is necessary.

If partial lots are used, the remaining devices must be resealed in an MBB or
placed in a dry atmosphere cabinet at <10% RH within 1 hour of MBB opening.

Refer to J-STD-033 for floor life under conditions other than +30°C/60% RH.

Table 11. Moisture Classification Level and Floor Life

Floor Life (Out of Bag) at Factory Ambient of 3 30°C/60% RH or

Level as Stated
1 Unlimited at ≤ 30°C/85%RH

2 1 year

2a 4 weeks

3 168 hours

4 72 hours

5 48

5a 24

6 Mandatory bake before use. After bake, must be reflowed within the
time limit specified on the label.

68 Flip Chip Ball Grid Array Package SPRU811

 Other Items

8.2 Packing Methodologies

The Texas Instruments Semiconductor Group uses three packing
methodologies to prepare semiconductor devices for shipment to end users,
stick magazine, tray, and tape and reel. (For more information, see the
application report, Semiconductor Packing Methodology, literature number
SZZA021B.)

8.2.1 Tray Packing

Flip chip BGA packages are packed in trays.
The IC shipping tray contains the components during component-assembly
operations, during transport and storage from the component manufacturing
plant to the customer’s board-assembly site, and when feeding components
to automatic-placement machines for surface mounting on board assemblies.
The tray is designed for components that require component isolation during
shipping, handling, or processing. Trays are stacked and bound together to
form standard packing configurations.
Trays are constructed of carbon-powder or fiber materials selected according
to the maximum temperature rating of the specific tray. TI trays designed for
components requiring exposure to high temperatures (moisture-sensitive
components) have temperature ratings of 150_C or more.
Trays are molded into rectangular JEDEC standard outlines containing
matrices of uniformly spaced pockets (see Figure 28). The pocket protects the
component during shipping and handling. The spacing provides exact
component locations for standard industry automated-assembly equipment
used for pick-and-place in board-assembly processes.

Figure 28. JEDEC Shipping Trays

Trays are packed and shipped in multiples of single trays stacked and bound
together for rigidity. An empty cover tray is added to the top of the loaded and

SPRU811 Flip Chip Ball Grid Array Package 69

Other Items

stacked trays. Typical tray stack configurations are five full trays and one cover
tray (5 + 1) and ten full trays and one cover tray (10 + 1) (see Figure 29).

Figure 29. Typical Tray Stack

8.3 Electrostatic Discharge Sensitive Devices (ESDS)

All electronic components can be damaged by electrostatic discharge (ESD)
throughout their life cycle. Static charge is produced whenever there is
movement. ESD controls help to reduce charge generation, potential
differences between objects (grounding), neutralize charges (ionizers), and to
remove field effects.
Devices assembled in flip chip BGA packages should be considered
ESD-sensitive. Care in handling should be used when processing FCBGA
packages.

9 Summary
Designing highly reliable systems using flip chip BGA packages is possible
with a good understanding of the manufacturing process, and the impact each
design element has on the PCB design.
For reliability, careful attention should be provided for the physical
characteristics of the copper lands on the PCB. Matching the land diameter on
the PCB to that on the BGA package ensures a robust solder connection.
When designing with fine-pitch BGA devices, provide special attention to
signal routing. Several methods are available to connect the balls of the BGA
to the inner layers of the PCB. Microvia and buried via technology allows more
space on each PCB layer for signal routing. Keep in mind the advantages and
disadvantages of having more routing space versus PCB manufacturing cost.
In addition to properly designing the PCB, it is necessary to keep the following
factors in mind:

70 Flip Chip Ball Grid Array Package SPRU811

 Other Items

- Understand the reflow process which best fits your PCB system mounting
requirements. Follow the provided reflow profile and compare closely to
the solder paste manufacturer’s recommended reflow profile.

- Conduct appropriate strain and strain rate characterization on the PCB

assembly process prior to component-mounting on a new PCB design.

- Avoid excessive shock and bending of the PC board during assembly,

handling, and testing of FCBGAs.

Finally, always follow the directions provided for handling moisture-sensitive

devices. Make sure to keep the required documentation readily available to
avoid potential disruptions associated with moisture−induced problems.

SPRU811 Flip Chip Ball Grid Array Package 71

 IMPORTANT NOTICE
Texas Instruments Incorporated and its subsidiaries (TI) reserve the right to make corrections, enhancements, improvements and other
changes to its semiconductor products and services per JESD46, latest issue, and to discontinue any product or service per JESD48, latest
issue. Buyers should obtain the latest relevant information before placing orders and should verify that such information is current and
complete. All semiconductor products (also referred to herein as “components”) are sold subject to TI’s terms and conditions of sale
supplied at the time of order acknowledgment.
TI warrants performance of its components to the specifications applicable at the time of sale, in accordance with the warranty in TI’s terms
and conditions of sale of semiconductor products. Testing and other quality control techniques are used to the extent TI deems necessary
to support this warranty. Except where mandated by applicable law, testing of all parameters of each component is not necessarily
performed.
TI assumes no liability for applications assistance or the design of Buyers’ products. Buyers are responsible for their products and
applications using TI components. To minimize the risks associated with Buyers’ products and applications, Buyers should provide
adequate design and operating safeguards.
TI does not warrant or represent that any license, either express or implied, is granted under any patent right, copyright, mask work right, or
other intellectual property right relating to any combination, machine, or process in which TI components or services are used. Information
published by TI regarding third-party products or services does not constitute a license to use such products or services or a warranty or
endorsement thereof. Use of such information 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.
Reproduction of significant portions of TI information in TI data books or data sheets is permissible only if reproduction is without alteration
and is accompanied by all associated warranties, conditions, limitations, and notices. TI is not responsible or liable for such altered
documentation. Information of third parties may be subject to additional restrictions.
Resale of TI components or services with statements different from or beyond the parameters stated by TI for that component or service
voids all express and any implied warranties for the associated TI component or service and is an unfair and deceptive business practice.
TI is not responsible or liable for any such statements.
Buyer acknowledges and agrees that it is solely responsible for compliance with all legal, regulatory and safety-related requirements
concerning its products, and any use of TI components in its applications, notwithstanding any applications-related information or support
that may be provided by TI. Buyer represents and agrees that it has all the necessary expertise to create and implement safeguards which
anticipate dangerous consequences of failures, monitor failures and their consequences, lessen the likelihood of failures that might cause
harm and take appropriate remedial actions. Buyer will fully indemnify TI and its representatives against any damages arising out of the use
of any TI components in safety-critical applications.
In some cases, TI components may be promoted specifically to facilitate safety-related applications. With such components, TI’s goal is to
help enable customers to design and create their own end-product solutions that meet applicable functional safety standards and
requirements. Nonetheless, such components are subject to these terms.
No TI components are authorized for use in FDA Class III (or similar life-critical medical equipment) unless authorized officers of the parties
have executed a special agreement specifically governing such use.
Only those TI components which TI has specifically designated as military grade or “enhanced plastic” are designed and intended for use in
military/aerospace applications or environments. Buyer acknowledges and agrees that any military or aerospace use of TI components
which have not been so designated is solely at the Buyer's risk, and that Buyer is solely responsible for compliance with all legal and
regulatory requirements in connection with such use.
TI has specifically designated certain components as meeting ISO/TS16949 requirements, mainly for automotive use. In any case of use of
non-designated products, TI will not be responsible for any failure to meet ISO/TS16949.
Products Applications
Audio www.ti.com/audio Automotive and Transportation www.ti.com/automotive
Amplifiers amplifier.ti.com Communications and Telecom www.ti.com/communications
Data Converters dataconverter.ti.com Computers and Peripherals www.ti.com/computers
DLP® Products www.dlp.com Consumer Electronics www.ti.com/consumer-apps
DSP dsp.ti.com Energy and Lighting www.ti.com/energy
Clocks and Timers www.ti.com/clocks Industrial www.ti.com/industrial
Interface interface.ti.com Medical www.ti.com/medical
Logic logic.ti.com Security www.ti.com/security
Power Mgmt power.ti.com Space, Avionics and Defense www.ti.com/space-avionics-defense
Microcontrollers microcontroller.ti.com Video and Imaging www.ti.com/video
RFID www.ti-rfid.com
OMAP Applications Processors www.ti.com/omap TI E2E Community e2e.ti.com
Wireless Connectivity www.ti.com/wirelessconnectivity

Mailing Address: Texas Instruments, Post Office Box 655303, Dallas, Texas 75265
Copyright © 2014, Texas Instruments Incorporated