Board Mounting Considerations for ULLGA Packages

AND8317
Board Mounting
Considerations for ULLGA
Packages
Prepared by: Phillip Celaya
ON Semiconductor
http://onsemi.com
Introduction
Printed Circuit Board (PCB) Design
Ultra Leadframe Land Grid Array (ULLGA) packages are
often the package of choice for optimizing device electrical
performance. They are light weight, thin and minimize the
use of board space. To take advantage of ULLGA
packaging, special preparations and guidelines have to be
followed to ensure proper mounting of the device onto the
PCB. This document outlines many of the processes and
board design considerations for mounting the 6- and 8-Pin
ULLGAs for 3 different pad pitches.
SMD and NSMD Pad Configurations
The Solder Masked Defined (SMD) and Non-Solder
masked Defined (NSMD) pad configurations are commonly
used for surface mount ULLGA packages.
With SMD configured pads, the solder mask covers the
outside perimeter of the rectangular contact pads. With this
configuration, the solder flows over the top surface of the
contact pad, and is prevented from flowing along the sides
of the pads by the solder mask.
With NSMD configured pads, there is a gap between the
solder mask and the rectangular contact pad. With this
configuration, the solder flows over the top surface and the
sides of the contact pad.
Since all of the 6- and 8-Pin ULLGA packages are
considered fine pitch (<0.5mm), it is recommended that
NSMD pads be used. The soldermask openings should be a
window design larger than the footprint.
Au Wire
Mold Compound
DIE
Recommended PCB Pad Design
Figure 2 shows the recommended board pad dimensions
for 6-Pin and 8-Pin ULLGAs using the NSMD design
configurations for the 0.35mm pitch packages.
Figure 3 shows the overlay of the package footprint on top
of the recommended PCB footprint for the 0.35 mm pitch
packages. Figures 4 and 5 show the recommended PCB
footprints and package overlay on top of recommended PCB
design for the 6-Pin ULLGA package for both the 0.4 and
0.5mm pitch packages.
Figure 6 and 7 show the recommended PCB footprint and
package overlay on top of recommended PCB design for the
8-Pin ULLGA packages for both the 0.40 and 0.50 mm pitch
packages.
Thin Metal Pads
Figure 1. Cross Section of ULLGA Package
Package Overview
ULLGA packages are very similar to Quad Flat No Lead
(QFN) and Dual Flat No Lead (DFN) packages. The major
difference being that the ULLGA does not have a copper
leadframe for the interconnect pads. Figure 1 is an example
of a cross section showing a ULLGA package.
The ULLGA in general is a thinner package than the
QFN/DFN type package.
© Semiconductor Components Industries, LLC, 2008
January, 2008 - Rev. 1
1
Publication Order Number:
AND8317/D
AND8317
6X
0.22
5X
0.48
8X
0.22
7X
0.48
1.18
1.18
1
0.53
1
0.53
0.35
PITCH
0.35
PITCH
Package Size: 1.0 x 1.0 mm
Package Size: 1.45 x 1.0 mm
Figure 2. Recommended PCB Pad Design for 6- and 8-Pin ULLGA Packages at 0.35 mm Pitch
6X
0.17
6X
0.10
8X
0.17
8X
0.10
1.18
1.18
8X
0.08
6X
0.08
1
1
0.35
PITCH
0.35
PITCH
Figure 3. Package Footprint Overlayed on Recommended PCB Pad Design for 0.35 mm pitch 6- & 8-Pin ULLGA
6X
0.26
5X
0.49
6X
0.30
5X
0.49
1.24
0.53
1.24
1
0.53
1
0.40
PITCH
0.50
PITCH
Package Size: 1.2 x 1.0 mm
Package Size: 1.45 x 1.0 mm
Figure 4. Recommended PCB Pad Design for 6-Pin ULLGA Packages at 0.4 and 0.5 mm Pitch
http://onsemi.com
2
AND8317
6X
0.20
6X
0.13
6X
0.25
6X
0.13
1.24
1.24
6X
0.05
6X
0.05
1
1
0.50
PITCH
0.40
PITCH
Package Size: 1.2 x 1.0 mm
Package Size: 1.45 x 1.0 mm
Figure 5. Package Footprint Overlayed on Recommended PCB Pad Design for 6-Pin ULLGA at 0.4 and 0.5 mm Pitch
8X
0.26
7X
0.49
8X
0.30
7X
0.49
1.24
1.24
1
0.53
1
0.53
0.40
PITCH
0.50
PITCH
Package Size: 1.6 x 1.0 mm
Package Size: 1.95 x 1.0 mm
Figure 6. Recommended PCB Pad Design for 8-Pin ULLGA Packages at 0.4 and 0.5 mm Pitch
8X
0.20
8X
0.13
8X
0.25
8X
0.13
1.24
1.24
8X
0.05
8X
0.05
1
1
0.50
PITCH
0.40
PITCH
Package Size: 1.6 x 1.0 mm
Package Size: 1.95 x 1.0 mm
Figure 7. Package Footprint Overlayed on Recommended PCB Pad Design for 8-Pin ULLGA
http://onsemi.com
3
AND8317
The recommended PCB pad footprints were also designed
so that competitor's packages would also be able to be
mounted without changing the PCB pad design. Figure 8
shows the package footprint of the SOT891 package
overlayed on top of the recommended PCB pad design for
the 1.0x1.0mm, 6-pin ULLGA package.
Figure 9 shows the 6-pin DFN package footprint
overlayed on top of the recommended PCB pad design for
the 1.45x1.0 mm package size.
Figure 10 shows the recommended land pattern design of
a BGA package and how the 6-pin ULLGA would fit onto
this pattern. Note, we do not recommend placing a BGA
package onto the recommended ULLGA pad design since
the large pad sizes could cause solder starvation since there
would be limited amount of solder in the solder ball of the
package.
6X
0.22
5X
0.48
6X
0.20
5X
0.30
1.18
0.53
1.24
1
1
0.35
0.35
PITCH
0.50
PITCH
Figure 8. SOT891 Package Overlayed on Top
of Recommended ULLGA PCB Pad Design
Figure 9. DFN Footprint Overlayed on Top of
Recommended ULLGA PCB Pad Design
6X
Solder Land
0.225 mm Dia
ON Semiconductor
Package Footprint
SM Opening 0.35 mm Dia
Figure 10. ON Semiconductor Package Footprint Overlayed onto BGA Footprint
http://onsemi.com
4
AND8317
SMT Process Recommendations
Plating of the PCB Pads
Solder Stencil Design
There are two common plated solderable metallizations
which are used for PCB surface mount devices. In either
case, it is imperative that the plating is uniform, conforming,
and free of impurities to ensure a consistent solderable
system.
The first metallization consists of plating electroless
nickel over the copper pad, followed by immersion gold.
The allowable stresses and the temperature excursions the
board will be subjected to throughout its lifetime will
determine the thickness of the electroless nickel layer. Gold
thickness is recommended to be 0.15 mm $ 0.05 mm.
Having excessive gold in the solder joint can create gold
embrittlement, which may affect the reliability of the joint.
The second recommended solderable metallization is the
use of an Organic Solderability Preservative coating (OSP)
over the copper plated pad. The organic coating assists in
preserving the copper metallization for soldering.
PITCH
0.350
6X
0.218
0.700
The solder is typically patterned onto the PCB by using a
127 to 104 mm (0.005 to 0.004 in) thick stencil screen. The
stencil type should be laser-cut stainless steel and
electropolished.
The stencil aperture opening sizes should be oblong
shaped openings. The sizes of these openings are shown
below in Figures 11 and 12 for the various pad pitches of the
ULLGA packages.
This screen is designed and manufactured to only allow a
specific amount of solder to be placed on the bond pads. It
is recommended that the side walls of the screen openings
be tapered approximately 5 degrees to facilitate the release
of the paste when the screen is removed from the PCB.
PITCH
0.400
6X
0.189
0.700
6X
0.170
12X
R0.086
PITCH
0.500
6X
0.139
0.700
6X
0.200
12X
R0.100
12X
R0.125
6X
0.250
Figure 11. Recommended Stencil Designs for 6-Pin ULLGA Packages with Different Pitches
PITCH
0.350
8X
0.218
0.700
PITCH
0.400
8X
0.189
0.700
8X
0.170
16X
R0.086
PITCH
0.500
8X
0.139
0.700
8X
0.200
16X
R0.100
8X
0.250
16X
R0.125
Figure 12. Recommended Stencil Designs for 8-Pin ULLGA Packages with Different Pitches
Solder Type
recommended especially since ULLGA pads pitches are
very small and do not allow much spacing between pads.
The use of low-air force nozzles are recommended to reduce
the risk of shorting during the SMT process. A force of
50-70 grams is recommended when placing the packages
onto the PCB board.
Either type 4 or 5 solder paste is recommended for surface
mount applications. Solder paste must be a no-clean type
paste. ULLGAs once mounted to the PCB board, will have
no stand-off height between the package and the PCB board.
Therefore, cleaning under the package is not an option.
Package Placement
Pick and place equipment with the standard tolerance of
$0.10 mm or better is recommended. Lower force may be
http://onsemi.com
5
AND8317
Solder Reflow
determined, and is available, by the manufacture of the paste
since the chemistry and viscosity of the flux matrix will vary.
These variations will require small changes in the profile in
order to achieve an optimized process.
In general, the peak temperature of the profile should be
between 210-225°C for Eutectic Solder profiles and
250-260°C for Pb-Free solder profiles.
Once the package is placed on the PC board along with the
solder paste, a standard surface mount reflow process can be
used to mount the part. Forced convection reflow in nitrogen
is recommended.
An example of a standard Pb-free profile is shown in
Figure 13. The exact recommended reflow profile will be
AC CHARACTERISTICS
Profile Features
Pb-Free Assembly
Average Ramp-up Rate (Tsmax to Tp)
3°C/Second Max
Preheat
Temperature Min (Tsmin)
Temperature Max (Tsmax)
Time (tsmin to tsmax)
150°C
200°C
60-180 Seconds
Time Maintained Above
Temperature (TT)
Time (tT)
217°C
60-150 Seconds
Peak Classification Temperature (Tp)
260°C +5/-09
Time Within 55°C of Actual Peak Temperature (tp)
20-40 Seconds
Ramp Down Rate
6°C/Second Max
Time 25°C to Peak Temperature
8 Minutes Max
TEMPERATURE ⇒
Tp
TL
25
t 25°C to Peak
TIME ⇒
Figure 13. Typical Pb-Free Solder Heating Profile
Solder Joint Inspection
for this procedure since the airflow and temperature
gradients can be carefully controlled. Nitrogen atmosphere
is typically used to control the pads from oxidizing. It is also
recommended that the PC board be placed in an oven at
125°C for 12 hours prior to heating the parts to remove
excess moisture from the packages.
Once the solder joints are heated above their liquidus
temperature, the package can be removed and the pads on the
PC board cleaned. The solder paste is again dispensed and
a new package can be reflowed onto the PC board.
The inspection of the solder joints is commonly
performed with the use of an X-ray inspection system. With
this tool, one can locate defects such as shorts between pads,
open contacts, voids within the solder as well as any
extraneous solder.
Rework Process
It is important to minimize the chance of overheating
neighboring devices during the removal of the package since
these devices are typically in close proximity to other
packages, Standard SMT rework systems are recommended
http://onsemi.com
6
AND8317
ON Semiconductor and
are registered trademarks of Semiconductor Components Industries, LLC (SCILLC). SCILLC reserves the right to make changes without further notice
to any products herein. SCILLC makes no warranty, representation or guarantee regarding the suitability of its products for any particular purpose, nor does SCILLC assume any liability
arising out of the application or use of any product or circuit, and specifically disclaims any and all liability, including without limitation special, consequential or incidental damages.
“Typical” parameters which may be provided in SCILLC data sheets and/or specifications can and do vary in different applications and actual performance may vary over time. All
operating parameters, including “Typicals” must be validated for each customer application by customer's technical experts. SCILLC does not convey any license under its patent rights
nor the rights of others. SCILLC products are not designed, intended, or authorized for use as components in systems intended for surgical implant into the body, or other applications
intended to support or sustain life, or for any other application in which the failure of the SCILLC product could create a situation where personal injury or death may occur. Should
Buyer purchase or use SCILLC products for any such unintended or unauthorized application, Buyer shall indemnify and hold SCILLC and its officers, employees, subsidiaries, affiliates,
and distributors harmless against all claims, costs, damages, and expenses, and reasonable attorney fees arising out of, directly or indirectly, any claim of personal injury or death
associated with such unintended or unauthorized use, even if such claim alleges that SCILLC was negligent regarding the design or manufacture of the part. SCILLC is an Equal
Opportunity/Affirmative Action Employer. This literature is subject to all applicable copyright laws and is not for resale in any manner.
PUBLICATION ORDERING INFORMATION
LITERATURE FULFILLMENT:
Literature Distribution Center for ON Semiconductor
P
.O. Box 5163, Denver, Colorado 80217 USA
Phone: 303-675-2175 or 800-344-3860 Toll Free USA/Canada
Fax: 303-675-2176 or 800-344-3867 Toll Free USA/Canada
Email: [email protected]
N. American Technical Support: 800-282-9855 Toll Free
USA/Canada
Europe, Middle East and Africa Technical Support:
Phone: 421 33 790 2910
Japan Customer Focus Center
Phone: 81-3-5773-3850
http://onsemi.com
7
ON Semiconductor Website: www.onsemi.com
Order Literature: http://www.onsemi.com/orderlit
For additional information, please contact your local
Sales Representative
AND8317/D
Similar pages