PlasticMold Compound
ExposedThermalPadLocated
UnderneaththePackage
Die Attach(Epoxy)
IC(Silicon)
Leadframe(Copper Alloy)
Application Report
QFN Layout Guidelines
Yang Boon Quek ........................................................................................ HPL Audio Power Amplifiers
1 Introduction
Board layout and stencil information for most Texas Instruments (TI) Quad Flat No-Lead (QFN) devices is
provided in their data sheets. This document helps printed-circuit board (PCB) designers understand and
better use this information for optimal designs.
The QFN package is a thermally enhanced standard size IC package designed to eliminate the use of
bulky heat sinks and slugs. This package can be easily mounted using standard PCB assembly
techniques and can be removed and replaced using standard repair procedures.
The QFN package is designed so that the lead frame die pad (or thermal pad) is exposed on the bottom
of the IC (see Figure 1 ). This provides an extremely low thermal resistance ( θJC) path between the die and
the exterior of the package.
SLOA122 – July 2006
SLOA122 – July 2006 QFN Layout Guidelines 1
Submit Documentation Feedback
Figure 1. Section View of a QFN Package
www.ti.com
SolderMaskDefinedThermalPad,seeFigure4
FingerPads,seeFigure3
Board Layout
2 Board Layout
Figure 2 shows an example of the recommended board layout for an RGZ package.
Figure 2. Board Layout for an RGZ Package Finger Pads
TI recommends the use of rounded finger pads to prevent solder bridging. Surround each pad with a
0,07-mm wide solder mask. The recommended dimensions are shown in Figure 3 .
2.1 Solder Mask Defined Thermal Pad
The solder mask defined thermal pad is the exposed copper area not covered by solder mask. It must be
soldered directly to the thermal pad on the bottom of the IC. Figure 2 shows an example of the
recommended dimensions.
2.1.1 Copper Areas
Copper areas on and in a PCB act as heat sinks for the QFN device. Top copper areas should be covered
with solder mask leaving only the solder mask defined thermal pad exposed. The top copper areas should
be made as large as possible.
2 QFN Layout Guidelines SLOA122 – July 2006
Figure 3. Finger Pads Layout
Submit Documentation Feedback
www.ti.com
ThermalVia
WeborSpokeVia
NOTRecommended
Solid Via
Recommended
Exposed Copper–
0,05mm AroundVia
Inner or bottom layer copper planes also can be connected to thermal pad using vias and should be made
as large as possible. The thermal pad is usually tied to ground, and designers should verify the electrical
correctness when connecting the copper planes to the thermal pad.
Designers may leave the bottom copper plane exposed. However, studies have shown that this has
minimal impact on thermal performance.
2.1.2 Thermal Vias
TI recommends placing thermal vias in the solder mask defined thermal pad to transfer effectively the heat
from the top copper layer of the PCB to the inner or bottom copper layers.
TI provides the recommended layout of the thermal vias in most data sheets. The recommended via
diameter is 0,3 mm or less, and the recommended via spacing is 1 mm (see Figure 4 ).
Board Layout
Figure 4. Solder Mask Defined Thermal Pad
The thermal vias should make their connection to the internal ground plane with a complete connection
around the entire circumference of the plated through hole. Place a ring of exposed copper (0,05 mm
wide) around the vias at the bottom of the copper plane.
Do not cover the vias with solder mask which causes excessive voiding.
Do not use a thermal relief web or spoke connection which impedes the conduction path into the inner
copper layer(s) (see Figure 5 ).
Figure 5. Via Connection at the Bottom of the Copper Plane
SLOA122 – July 2006 QFN Layout Guidelines 3
Submit Documentation Feedback
www.ti.com
Copper Areas – makeaslargeaspossible
SolderMask
Defined
ThermalPad –
follow
dimensions
given
Thermal Via – follow spacing givenandkeepdiameters less
than orequalto 0.3mm
External Via
Rounded
Finger Pads
Voiding – keep
lessthan 50%
Onlyexternal
viasareused
Topcopper
areacovered
withsolder
mask
SolderMaskDefined
ThermalPad-exposed
copperarea
Board Layout
Figure 6. X-Ray – DRB Device
Vias may be plugged to prevent solder loss and protrusions. This often produces the best thermal
performances but is not necessary or recommended because of the increased cost of PCBs and because
solder tends to wet the upper surface first before filling the vias.
Vias also can be used in the copper area outside the solder mask defined thermal pad to help dissipate
heat through bottom or inner planes.
If thin PCBs or vias larger than 0,3 mm are used, designers may use only external vias to prevent solder
loss and protrusions (see Figure 7 ). Designers should note that this might reduce thermal performance
significantly and should be evaluated on their PCBs.
2.1.3 Solder Loss and Protrusions
Solder loss and protrusions result when excessive solder flowed through internal vias during reflow. These
usually happen when incorrect internal vias sizes and stencil openings are used.
Solder loss results in voiding and severely affects thermal conductivity. Designers are encouraged to x-ray
their reflowed boards to verify that at least 50% of thermal pad area is soldered (less than 50% voiding)
when using 0,127-mm thick stencils.
Figure 7. Example of Using Only External Vias in a DRB Package
Protrusions might cause misalignment in stencil on the reverse side of the PCB (see Figure 8 ).
4 QFN Layout Guidelines SLOA122 – July 2006
Submit Documentation Feedback
www.ti.com
Protrusion
2.1.4 Stencil
Board Layout
Figure 8. Protrusion at the Other Side of Board
Figure 9 shows an example of the recommended stencil openings and thickness. Follow stencil openings
and thickness recommended to ensure that the right amount of solder paste is used.
Figure 9. Recommended Stencil Openings and Thickness for RGZ Package
Use cross-hatching in the thermal pad stencil opening of a QFN device. This prevents excessive amount
of solder paste applied thus prevents solder bridging (see Figure 10 ).
SLOA122 – July 2006 QFN Layout Guidelines 5
Submit Documentation Feedback
www.ti.com
SolderpasteappliedNosolderpasteapplied
Cross-Hatching – Recommended
NoCross-Hatching – NotRecommended
Board Layout
2.1.5 Recommended Solder Paste
TI recommends the use of type 3 or finer solder paste when mounting a QFN.
2.2 Additional Information
For detailed information on the QFN package including thermal modeling considerations and repair
procedures, see (SLUA271 ) QFN/SON PCB attachment.
Figure 10. Thermal Pad Stencil Opening
6 QFN Layout Guidelines SLOA122 – July 2006
Submit Documentation Feedback
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
Low Power Wireless www.ti.com/lpw 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 2006, Texas Instruments Incorporated
Loading...