Simcom 0912142009007 Quad-band GSM/GPRS module User Manual Modular Guide

Shanghai Simcom Ltd. Quad-band GSM/GPRS module Modular Guide

Contents

Modular Guide

SMT Module RF Reference
Design Guide
AN_ SMT Module RF Reference Design Guide
_V1.01
Document Title: SMT Module RF Reference Design Guide
Version: 1.01
Date: 2010-1-27
Status: Release
Document Control ID: AN_SMT Module RF Reference Design Guide_V1.01
General Notes
SIMCOM offers this information as a service to its users, to support application and engineering
efforts that use the products designed by SIMCOM. The information provided is based upon
requirements specifically provided to SIMCOM by the users. SIMCOM has not undertaken any
independent search for additional relevant information, including any information that may be in
the user’s possession. Furthermore, system validation of this product designed by SIMCOM
within a larger electronic system remains the responsibility of the user or the user’s system
integrator. All specifications supplied herein are subject to change.
Copyright
This document contains proprietary technical information which is the property of SIMCOM
Limited., copying of this document and giving it to others and the using or communication of the
contents thereof, are forbidden without express authority. Offenders are liable to the payment of
damages. All rights reserved in the event of grant of a patent or the registration of a utility model
or design. All specification supplied herein are subject to change without notice at any time.
Copyright © Shanghai SIMCOM Wireless Solutions Ltd. 2010
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 1
SMT Module RF Reference Design Guide
1 Introduction....................................................................................................................................2
2 Circuit design .................................................................................................................................2
2.1 Power supply circuit design ................................................................................................2
2.2 Antenna matching circuit design.........................................................................................3
3 Consideration in components placement........................................................................................4
4 Stacking up of multi-layers PCB....................................................................................................5
Stack-up of two-layers PCB......................................................................................................5
Stack-up of four-layers PCB .....................................................................................................6
Stack-up of six-layers PCB .......................................................................................................6
Stack-up of eight-layers PCB....................................................................................................7
5 Impedance control of RF trace.......................................................................................................7
6 Consideration in PCB layout........................................................................................................10
Appendix......................................................................................................................................... 11
Two-layers PCB ...................................................................................................................... 11
Four-layers PCB......................................................................................................................12
Six-layers PCB........................................................................................................................13
Eight-layers PCB.....................................................................................................................16
Version History
Data Version
Description of change Author
2010-1-20 01.01 Origin Ye Haibing,
Wang Guoqiang
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 2
1 Introduction
This document describes the important points about RF that should be taken into account in
client’s application design. As SMT module can be integrated with a wide range of applications,
the application notes are described in detail.
SMT module is a new and key product which is provided by SIMCom inc. This type module
become very popular soon after it is released for its easy integration, good reliability. But bad RF
design will lead to serious RF problems. In order to improve the RF performance, this document is
formed to give the customer some design guides in RF design of SMT type module integration.
Based on such considerations, at the later section, this document will describe some key issues that
should be paid more attention to.
NOTE: this document can apply for all SMT Modules, for example, SIM300D, SIM340D,
SIM300W, SIM340W, SIM500W, SIM540W, SIM700D, SIM900, SIM900A, SIM900D, and
so on. SIM900 is selected as a demonstration in the last sections.
2 Circuit design
When the customer begins to integrate the SMT type module into their product, the first thing to
be considered is the circuit design. In this section, we will focus on the circuit design which is
related to the RF performance. This section is divided into two sub-parts, the first is the power
supply circuit design; the second is the antenna matching circuit design.
2.1 Power supply circuit design
Because the SMT module is a high power consuming communication system, and the maximum
working power will up to 2watt in worst case, so, this will form a large voltage drop at the
module’s power supply port. To make the SMT module have a stabilized working condition, we
recommended a large tantalum capacitor (100uF or more capacity is recommended) shunted to the
module’s power supply port. To get better noise decoupling performance, some additional small
ceramic capacitors can be added combined with the large capacitor.
If the SMT module is powered by a DC-DC in the customer’s design, to avoid the module’s RF
performance is affected by the switching frequency of the DC-DC, for example, modulation
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 3
spectrum, switching spectrum, a series large current ferrite bead(with rated current minimum 2A)
should be added at the power supply port. The recommended power supply circuit is shown as
below:
R1
C3
55
SIM900
56
VBAT
VBAT C2 C1
VBAT
22pF 100nF 100uF
Figure1 Power Supply Circuit
VBAT 57
In this circuit, by default, the component R1 should be a 0ohm resistor with 0805 size. When the
module is powered by DC-DC, and the module’s RF performance is affected by the DC-DC’s
switching frequency, R1 can be changed to a large current ferrite bead to filter the noise.
2.2 Antenna matching circuit design
Because the module is working under 50ohm system in RF part, so, to get the best RF
performance, the SMT module’s load impedance should be tuned to 50ohm. But in fact, the most
antenna’s port impedance is not a purely 50ohm, so, to meet the 50ohm requirement, an additional
antenna matching circuit should be needed. Furthermore, to facilitate the antenna debugging and
certification testing of RF performance, we suggested the customer add a RF test connector in
series between the module’s RF port and the antenna matching circuit. The recommended antenna
matching circuit is shown as below:
In the Figure2, the components, R4, C5 and C6 make up a pi-type matching circuit structure. If
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 4
add the optional component R3, then a T-type matching circuit structure will be made up with
another two components R4 and C5. But usually, a pi-type matching circuit is enough in antenna
tuning process. The component J2 is a RF test Port, used for conduct RF test. The traces in Bold
type must be 50 ohm impedance controlled when layout a design.
For the RF test connector, we suggested the customer use the part vended by Murata, its part
number is MM8430-2610.
3 Consideration in components placement
In PCB design, a good placement of components will help the improving of the product’s
performance. The following are some thumbs should be followed.
1）The SMT module should be placed far away from the noise source circuit, such as high speed
digital circuit, etc. if this requirement cannot be met, the noise source circuit should be shielded
perfectly. This will help to reduce the interference between the SMT module and the noise source
circuit.
2）The placement of SMT module should make the module’s RF port close to the antenna’s feed
pad. This will make the length of RF trace between the module’s RF port and antenna as short as
possible, and consequently.
3）The decoupling capacitor of module’s power supply should be placed close to the VBAT pads,
this will help the improvement of decoupling.
The best placement and some bad placements are shown as below:
SIM900
Figure3 Good Placement
Antenna
Matching circuit
and Antenna area
Power Supply
Noise Source
(high speed
digital circuit, or
others)
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 5
VBAT
VBAT
VBAT
55
57
56
RF_IN
60 GND
GND61
59
Figure3 is the best placement; antenna part is near RF_IN pad, power supply is near VBAT pad,
noise source is far away the Sim900.
Figure4, Figure5, Figure6 are bad placements. Figure4, power supply and antenna part are crossed;
Figure5, noise source is near to Sim900; Figure6 antenna part is far away from RF_IN pad of
sim900.
4 Stacking up of multi-layers PCB
For EMC performance consideration, once the working frequency in the customer’s product is
over than 5MHz, or the rise-up/fall-down period of digital signal is less than 5ns, then multi-layers
PCB should be considered. Now, the more common multi-layer PCB structure is four-layers,
six-layers and eight-layers PCB, etc. If the customer’s product is designed in multi-layers PCB
technology, then the stack-up design of multi-layers PCB will become very important. The
following will show some typical stack-up design of multi-layers PCB, but each design has its
own advantages and disadvantages.
Note: In the following table, S1 indicates the first signal layer, S2 indicates the second signal
layer, and so on.
Stack-up of two-layers PCB
Top layer Bottom layer
Case A S1+POWER+GND S2+POWER+GND
Table1 Stack-up of two-layers PCB
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 6
Two-layers PCB is the lowest cost solution, but this solution has the worst EMC performance, and
it is not appropriate in high speed design, because in this solution, the ground integrity, the
crosstalk between signal traces is very bad.
Stack-up of four-layers PCB
Top layer Second layer Third layer Bottom layer
Case A GND S1+POWER S2+POWER GND
Case B S1 GND POWER S2
Table2 Stack-up of four-layers PCB
Case A, should be the best case in four-layers PCB board design. In this case, the outer layer is
ground layer, which have some help in shielding the EMI signals; and also, the power supply layer
is very close to the ground layer, so the power supply resistance is smaller, and the EMC
performance will be very good. But if the density of devices on the PCB is very high, then this
type PCB stack-up should not be used to design, because the ground integrity can not be assured
under high density design, and the signal quality in second layer will be very bad. In this situation,
Case B is the most common way usually.
Stack-up of six-layers PCB
Top layer
Second
layer
Third
layer
Fourth
layer
Fifth layer
Bottom
layer
Case A S1 GND S2 S3 POWER S4
Case B S1 S2 GND POWER S3 S4
Case C S1 GND S2 POWER GND S3
Case D GND S1 POWER GND S2 GND
Table3 Stack-up of six-layers PCB
Six-layers PCB gives more design flexibility than a four-layers PCB, but it takes some work to
make it ideal in EMC terms.
Case A in the above table, is the usually common way. In this case, S1 is a better signal routing
layer, and S2 somewhat less. But this case has a disadvantage that this stack-up has very little
distributed capacitance between its ground and power planes.
Case B has good EMC characteristics, because this stack-up has good noise decoupling between
the power plane and ground for the big distributed capacitance.
Case C is the better stack-up, in this case, S1, S2 and S3 are good signal routing layer, the power
decoupling is good for the big distributed capacitance between the ground and power planes.
Case D is the best stack-up, the EMC performance will be good, but the disadvantage is that the
routing layer is less than other type stack-up.
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 7
Stack-up of eight-layers PCB
Top
layer
Second
layer
Third
layer
Forth
layer
Fifth
layer
Sixth
layer
Seventh
layer
Bottom
layer
A S1 S2 GND S3 S4 POWER
S5 S6
B S1 S2 S3 GND POWER
S4 S5 S6
C S1 GND S2 S3 S4 S5 POWER
S6
D S1 GND S2 S3 GND POWER
S4 S5
E S1 GND S2 GND S3 POWER
S4 S5
F S1 GND S2 GND POWER
S3 GND S4
Table4 Stack-up of eight-layers PCB
Eight-layers PCB gives more design flexibility than a six-layers PCB, but it takes some work to
make it ideal in EMC terms.
If the design needs 6 signal routing layers, then case A will be the best stack-up design, but this
type stack-up should not be used in high speed digital circuit design.
If the product design needs 5 signal routing layers, case E will be the best. In this case, S1, S2 and
S3 are good signal routing layer, and the power decoupling is good.
If the design needs 4 signal routing layers, case F will be the best. In this case, every signal routing
layers are good. In all the case, the signal trace routed in adjacent signal routing layers should be
orthogonal.
5 Impedance control of RF trace
Because the module’s RF part is working in a 50ohm system, so its output load impedance should
be 50ohm, to meet this requirement, the all RF signal trace should be impedance controlled, and
its characteristic impedance should be 50ohm.
The RF trace impedance can be controlled through using different trace geometry. There are more
than thirty different types of transmission line which can easily be created on a PCB. Twelve of
them are shown in figure 7
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 8
Figure7 twelve typical PCB transmission line
Usually, Surface Mircostrip Transmission Line and offset Strip Transmission Line are the most
common structures. In 50ohm RF system, through adjusting the width of RF traces and the
spacing to the reference GND, the impedance of RF traces can be controlled to 50Ohm.The
appendix will show some illustration in impedance controlled RF trace designing.
The customer may use software tool to calculate the impedance of RF trace, for example CITS25,
released by POLAR, the website is http://www.polarinstruments.com/, or APPCAD released by
AGILENT, the website is http://www.hp.woodshot.com.
Here are two examples about using CITS25 to calculate, Surface Mircostrip Transmission Line
and Offset strip Transmission Line correspondingly. Based on stack up of six-layers PCB
(thickness =1.0mm) shown in appendix.
Surface Mircostrip Transmission Line, the height is 298um (25+70+203=298um), the thickness is
25um, the result width (w) is 584um, as shown in figure8.
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 9
Figure8 Surface Mircostrip Calculate
Offset Strip Transmission Line，the height between two reference GND is 418um (203+35+180 =
418um), the height between RF trace and reference GND is 180um, the result width is 135um. as
shown in figure9.
Figure9 Offset Strip line Calculate
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 10
6 Consideration in PCB layout
In product’s PCB design, a good PCB layout will help the improvement of the whole product
performance, including reliability, EMC performance, etc. The following are some considerations
for referenced:
a） The Layer1.under SMT module test port should be copper keep out , layer2 should be GND;
b） The Layer2 under SMT module RF_IN pad should be copper keep out , layer3 should be
GND;
c） The Layer1.Layer2 under RF test connector should be copper keep out, layer3 should be GND;
the space to GND plane should more than 0.5mm.
d） RF trace between SMT module RF pad with the RF test connector, RF trace between RF test
connector with the antenna matching circuit, RF trace between the antenna matching circuit
with the antenna feed PAD all should be controlled to 50 Ohm
e） Avoid to layout any high speed signal under RF trace, if high speed signal is needed, a GND
plane is needed between these two signals.
f） All layers under the antenna feed pad should be copper keep out. Or, the space between
antenna feed pad with the GND under feed pad should be more than 1mm.
g） Do not layout RF trace in orthogonal.
h） When layout surface Mircostrip Transmission Line or offset Strip Transmission Line , 3W
rule should be followed, that means the space between reference GND with RF trace should
three times more than the width of RF trace.
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 11
Appendix
The following are some illustration of impedance controlled RF trace designing. It is should be
noted that the RF trace’s width and spacing to the reference ground is combined to specific PCB
stack-up(the PCB’s thickness, clearance between every layer).
Two-layers PCB
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 12
Four-layers PCB
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 13
Six-layers PCB
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 14
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 15
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 16
Eight-layers PCB
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 17
SMT Module RF Reference Design Guide
SMT Module RF Reference Design Guide 18
Contact us:
Shanghai SIMCOM Wireless Solutions Ltd
Add: SIM Technology Building, No. 633, JinZhong Road, Shanghai,PRChina 200335
Tel: +86 21 32523300
Fax: +86 21 32523200
URL:www.sim.com

Navigation menu