Freescale SemiconductorApplication NoteDocument Number: AN3585Rev. 1.1, 07/2008PCB Layout Design Guidelines for RadioBoard Using the MC13853 LNA1AbstractRadio printed circuit boards (PCB) must effectivelyintegrate the devices and other elements while avoidingsignal transmission problems associated with RF linesand components interacting with each other. The purposeof this document is to provide general guidelines forsuccessful radio PCB design using the MC13853 LNA.The MC13853 has three bands, a low band and two highbands, in a QFN16 package.The most critical aspects of radio frequency (RF)circuitry are addressed and it is highly recommended tofollow these design guidelines to achieve best RFperformance.Note that these guidelines and example layout figures arebased on the RFX300-31 RF subsystem daughter cardsupporting WCDMA/EDGE 3G terminals. Freescale Semiconductor, Inc., 2007, 2008. All rights reserved.Contents1234567Abstract . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .1PCB Layers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .2Components and Placement Recommendations . . . . 3Trace Requirements . . . . . . . . . . . . . . . . . . . . . .14Grounding . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .17References . . . . . . . . . . . . . . . . . . . . . . . . . . . . .17Revision History . . . . . . . . . . . . . . . . . . . . . . . . .18

PCB Layers2PCB LayersThis section describes the PCB technology and PCB stack-up.2.1PCB Layer StructureIn this guideline, a classical PCB stack-up of 8 layers (2-4-2) is described. The PCB layering structure isshown in Figure 1, the PCB Layering Structure. The dielectric constant (εr) of the FR4 material used inthis example is 4.2.Figure 1. PCB Layering Structure2.2Layer RulesAn effective layer function assignment reaches best RF performances and significantly reduceselectromagnetic interference (EMI) problems. The RF circuit layout is the main concern for the layerfunction assignment. A solid ground plane next to the power distribution layers creates a set of low ESRcapacitors, thus reducing system noise. Each radio has its own specific constraint, but this is a basicreference for radio board design.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.12Freescale Semiconductor

Components and Placement RecommendationsTable 1. PCB Layer AssignmentLayerNumberLayer RuleRF Signals33.1Baseband Signals1Microstrips, Ground for striplinesComponent interconnections2Ground cutouts below microstrips and over striplinesVertical traces3Striplines, Ground for microstripsHorizontal traces, DC distribution4Main ground, Ground for striplinesMain ground5Ground, Ground over striplinesGround, DC distribution6Striplines, Sensitive traceHorizontal traces7Ground cutouts below striplinesVertical traces8Ground for striplinesComponent interconnectionsComponents and Placement RecommendationsComponent PlacementThe basic principle of component placement is to try and follow the natural signal flow: From the antennathrough the switch, the LNA, the SAW filter, the TRX to the BB.The following guidelines provide the basic ideas for component placement: Place the antenna, switch, Tx and Rx sections on the top of the radio board. Put the BB section to the bottom of the RF section. Place the PA close as possible to the Antenna Switch to minimize insertion loss. Place the MMM7210 and the PA in positions that ensure a direct and short as possible Tx path. Place the SAW filter close as possible to MMM7210 to minimize the distance of Rx differentiallines. When placing components, note the potential routing of circuits between subsystems, includingclocks and crystal circuits. Refer to Figure 2 for IC placement for a 2G 3G application on theRFX300-31 RF subsystem daughter card.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor3

Components and Placement LTERMMM721052 MHzFigure 2. RFX300-31 DCard Parts PlacementFigure 3 shows the LNA portion of the schematic of the Freescale RFX300-31 sub-system board with thecomponent designators shown. This can be used to locate the components in the subsequent layout figures.Note that components C346, L33, C342, L36, C341 and L38 are placeholders for notch filters on theinputs, if needed. Components C337, C340 and C339 are input shunt capacitor placeholders for each band,if needed. Figure 4 shows the general LNA and matching component locations, the top level ground layer,the microstrip traces between components, along with the input and output match areas circled. InFigure 5, the 50 ohm RF input lines and DC feed line are shown.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.14Freescale Semiconductor

Components and Placement RecommendationsHB2 INHB1 336C337LB INRFX300-31Rev EC339C334HB1 Emit21516LB EmitO OUTFigure 3. LNA and Matching Component Schematic for the RFX300-31 Sub-system BoardPCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor5

Components and Placement RecommendationsThree band RF inputmatch elementlocationsThree band RF outputmatch elementlocationsFigure 4. LNA and Matching Component LayoutPCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.16Freescale Semiconductor

Components and Placement Recommendations50 ohm StriplineRF Input LinesLNA Pin 1DC Feed LineFigure 5. LNA and Matching Component Layout Showing RF Lines and DC Feed Line3.2 3.3Component RecommendationsSelect low ESR capacitors for IC decoupling. Ceramic NPO material capacitors are preferred.Select the proper RF bypass capacitor value to place on supply and control line. For 0402 RFbypass capacitors use 33pFFor 0402 size inductors, the Murata LQG15HS series is recommended.LB Component PlacementsOn the MBC13853 QFN16 package, pin 1 is the LB RFin pin. The components of the LB input matchshould be arranged outward from pin 1, as shown in Figure 6. They should also be arranged so they arespaced as far away as practical from the HB1 RFin matching elements. The HB1 emitter pin between theLBin and HB1in pins provides additional spacing. The LB matching component closest to the package isa capacitor, which is rotated away from the package. This is followed by the input inductor, which is alsooriented so that it is rotated perpendicular to the HB1 inductor. The RF 50 ohm input line connects to theinductor, along with placeholders for two notch filter elements to ground.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor7

Components and Placement RecommendationsLB input matchingcomponentsLB inductor rotated90 degrees from theHB1 inductorHB1 emitter pinHB1 input matchingcomponentsFigure 6. LNA Input MatchingFigure 7 shows the LB output match. RFout is on pin 15 of the package. The matching components on thispin are arranged to follow the direction towards the SAW filter and away from the RFin trace andcomponents and also away from LB emitter pin 16. This is especially true of the feed inductor. It is movedout away from the LB emitter connection using a microstrip trace. RF and AC bypass capacitors should beplaced close to the feed inductor.In Figure 7, the RFX300-31 rev. E layout shows the LB emitter pin 16 connected through a trace directlyto ground, as is done for the HB1 and HB2 emitter pins. From a performance standpoint, it is best to notconnect the LB emitter pin directly to ground. The preferred method is to connect the LB emitter pin toground using a 0 ohm resistor. Either a 402 or 201 size resistor can be used with nearly equivalentperformance. Connecting the LB emitter pin directly to ground results in lower IM2 and IP3 performance.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.18Freescale Semiconductor

Components and Placement RecommendationsLB Emitter should beconnected to ground usinga 0 ohm resistor, not directlyto ground as shownLB Feed InductorSeries Capacitor andResistorFigure 7. LB Emitter on Pin 16 and Output Matching on Pin 153.4HB1 Component PlacementPin 2 on the QFN16 package is the HB1 emitter. This pin is connected directly to ground as shown inFigure 8. Bringing the ground plane to this pin also serves to isolate the LB RFin components and tracefrom the HB1 components and trace. Placing vias to the internal ground planes is recommended. In thislayout two vias are used with a trace between them that also helps isolate the LBin and HB1in paths andcomponents.As with the LB RFin path, the HB1 RFin path must also be designed so as to be moved as far from theHB2 RFin trace and components as can be made feasible so as to maximize the isolation between the twohigh band RF signal paths, as shown in Figure 8. In this layout, the HB2 trace leaves the package pin at a45 degree angle. Also important is to have the match inductor oriented at 90 degrees relative to the matchinductor used for the HB2 RF in path, so as to minimize mutual coupling between the two. Pin 2 is theHB1 emitter and should be connected directly to ground. Nearby vias to internal ground planes arerecommended. The shunt capacitor matching component should have a short, low inductive path from theground side to the HB1 emitter pin.In Figure 9 the HB1 output matching is shown. Note the placement of pads for a short between the linesclose to the package pins to allow for an output sharing configuration. The HB1 DC feed inductor is placedas close to the HB1 output pin as possible.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor9

Components and Placement RecommendationsThe HB1 RFout line on pin 11 is designed so as to maximize the spacing from the HB2 RFout trace byhaving the components emanating away from the HB2 components.Ground trace extendsbetween the HB1 andHB2 input componentsHB1 series inductor isperpendicular to both theLB series inductor and theHB2 series inductorThe shunt capacitor is rotatedwith the ground end closest tothe HB1 emitter groundHB1 emitter to ground layerswith two vias.Trace connected to ground atboth ends also helps isolateLBin and HB1in linesFigure 8. HB1 input MatchingHB1 feed inductororiented away from HB2line and placed as closeto the HB1 output pin aspossibleDNP jumperplacement for outputsharing optionMatching componentscontinue outwards awayfrom the HB2components andtowards the SFMFigure 9. HB1 Output MatchingPCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.110Freescale Semiconductor

Components and Placement Recommendations3.5HB2 Component PlacementPin 4 of the QFN16 package is the HB2 RFin pin. The match components and RFin line should be arrangedto be spaced as far as possible away from the HB1 RFin components to maximize isolation between thetwo RF paths, as shown in Figure 10.Pin 5 is the HB2 emitter and should be connected directly to ground. Nearby vias to internal ground planesare recommended.The HB2 output inductor is rotated away from the HB1 output inductor as shown in Figure 11. The HB2DC feed inductor is placed as close to the HB1 output pin as possible. The output matching componentsare moved away from the HB1 components and separated from them by a ground area.HB2 matchingcomponents separatedfrom HB1 components bya ground regionconnected to inner layergrounds with viasHB2 inductor isperpendicular to theHB1 inductorThe shunt capacitor isrotated to have theground side connectedto the HB2 emittergroundHB2 input line orientedaway from the HB1 inputline at the packageFigure 10. HB2 InputPCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor11

Components and Placement RecommendationsHB2 emit connecteddirectly to groundHB2 feed inductororiented away fromthe HB1 line to theVcc connectionHB2 outputcomponents movedaway from the HB1output componentsand isolated by theground regionFigure 11. HB2 Output3.6RF Components Keep Out AreaFigure 12 highlights the keep out areas under RF matching components. RF lines and DC lines are not rununder RF components. DC lines that do run under RF traces are on layer 5 and are perpendicular to the RFtrace, when possible. Observance of RF keep out areas on the first internal layer under the RF signal pinsand all matching elements for the three LNAs is essential for realizing the available gain and achievingoptimum noise figure and return losses. Try to shield the RF traces with a ground plane. In this case, layer4 is the ground shield.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.112Freescale Semiconductor

Trace RequirementsKeep outs under RFcomponentsFigure 12. Keep outs for routing under RF components4Trace Requirements4.1 RF SignalsThe RF trace routing is always the top priority and it is necessary to route every RF trace accordingto the impedance matching technique.Impedance controlled traces are implemented by either microstrips or striplines.— The microstrip should be used within a shielded area (with a metal shield cavity) of outer layersfor short interconnection between components.— The stripline can provide good isolation even in an unshielded area (without a metal shieldcavity) because it is completely bounded by an upper and lower layer of the ground plane. It issuitable for RF signals and sensitive lines.Any circuit trace on the PCB has characteristic impedance associated with it. This impedance isdependent on width (W) of the trace, thickness (T) of the trace, dielectric constant (εr) of thematerial used, and height (H) between the trace and reference plane. Many microwave CAD toolsare available and can support the designer to compute trace width.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor13

Trace Requirements Coplanar clearances (G) must be at least the trace width (W) and at least twice the height H1 or H2.This reduces the parasitic capacitance, which potentially alters the trace impedance and increasesthe losses.Width of controlled impedance trace should be wide enough to maintain reasonable insertion lossand manufacturing reliability. Cutting out inner layers ground areas next to the microstrip or thestripline trace layer, increase the effective substrate height; therefore, increasing the width of theRF trace.Microstrip and Stripline Models show the inner ground cut out of the microstrip and the stripline.Cut out ground fill under RF signal pads to reduce stray capacitance losses.Avoid parallel routing and crossing of RF traces and from under signal pads.Keep the routing direct and short. For a long trace, use the stripline.Use the microstrip for RF traces on the components side.Avoid multiple transitions between the layers.Avoid routing RF trace with sharp corners. A smooth radius is recommended.Isolate the Rx and Tx paths by ground.Fill the area around the RF traces with ground and ground vias to connect inner ground layers forisolation.Figure 13. Microstrip and Stripline Model Use controlled impedance RF traces:Rx paths into the LNA:– 50Ω LNA inputs and outputs. Microstrip line (width 0.286 mm) on top layer Stripline onlayer 6 (width 0.105 mm/Ground layers 5 and 8)– Refer to Figure 14 for a routing example of HB1 and HB2 input stripline lines. Note thestripline RF lines are clear of other signal lines and vias. Layer 5 serves as the ground overthe stripline and layer 8 serves as the ground below the stripline. These ground referencelayers should be at equal electromagnetic potential. Tie the two ground references together,in particular along the RF trace, with adequate vias. Note the grounding wall with vias inbetween the RF traces to isolate RF paths. In Figure 15 the microstrip lines on the top layerused to connect the RF matching components are shown. The striplines shown in Figure 14are on layer 6.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.114Freescale Semiconductor

Trace RequirementsGrounding bar between theHB1 and HB2 50 ohm inputlines (Good isolation betweenthese RF traces needs to bemaintained)HB1 Stripline 50 ohm input lineHB2 Stripline 50 ohm input lineMicrostrip line on top layerDigital SPI linesFigure 14. HB1 and HB2 LNA Stripline Input LinesLayer 3 is the ground for themicrostrip with openings at theconnection between the microstripline and the stripline on layer 6Ground via as close as possible tothe RF signal via (at least one isrequired, more are preferred)Microstrip line on the top layerFigure 15. Microstrip Lines Used to Connect the RF Matching Components4.2DC DistributionThere are a number of guidelines pertaining to the DC lines. See Figure 16 for reference. Use several signal vias for layer transitions of the main DC supply and its groundPCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor15

Grounding Connect signals and ground directly by the vias on pads.Put ground vias along microstrips, striplines and non-RF sensitive lines for better isolation.Add ground vias on the outer ground filled area to connect to the inner ground layers for improvinggrounding isolation.Avoid perforating the Vcc line trace with noisy vias.Add multiple ground vias under the LNA for proper grounding to inner ground layers.Add multiple vias to connect the inner layer DC supply line to surface supply pins to minimizevoltage drop.Do not route Vcc under 52 MHz crystal even if the routing is under several layers of ground.Vcc signal is routed down onlayer 5Figure 16. DC Line Showing Routing5GroundingFor grounding, follow these guidelines: Make the internal ground area as solid as possible. Do not break the ground into pieces. Provide good solid ground by using multiple vias. Fill as much ground as possible in the area between the walls of shield cavities and outline of theRF section. Connect each ground pin or via to the ground plane individually. A daisy chain connection to theground pins shares the ground path, which increases the return current loop. Use ground via stitching to transition from top layers to inner ground layers.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.116Freescale Semiconductor

References 6The PCB pattern under the LNA must bridge the ground pins (pins 2, 5 and 16) and the ground pad.Add ground vias to inner ground layers for each ground pin.ReferencesFor more information refer to the following documents. Freescale documents are located at: MC13853 Data Sheet - Tri-Band Low Noise Amplifiers with Bypass Switches (document number:MC13853)7Revision HistoryTable 2 summarizes revisions to this document since the release of the previous version (Rev. 1.0).Table 2. Revision HistoryLocationRevisionFigure 3Revised drawing.Section 3.3, “LB Component PlacementsRemoved sentence “The shunt capacitor should have a short, lowinductance path from the ground side to the LB emitter pin.“ from the firstparagraph. Replaced final paragraph in section.Figure 6Removed text for LB Shunt Capacitor note.Figure 7Revised text for LB Emitter note.PCB Layout Design Guidelines for Radio Board Using the MC13853 LNAApplication Note, Rev. 1.1Freescale Semiconductor17

How to Reach Us:Home Page:www.freescale.comWeb Support: or Locations Not Listed:Freescale SemiconductorTechnical Information Center, EL5162100 East Elliot RoadTempe, Arizona 852841-800-521-6274 or, Middle East, and Africa:Freescale Halbleiter Deutschland GmbHTechnical Information CenterSchatzbogen 781829 Muenchen, Germany 44 1296 380 456 (English) 46 8 52200080 (English) 49 89 92103 559 (German) 33 1 69 35 48 48 (French) Semiconductor Japan Ltd.HeadquartersARCO Tower 15F1-8-1, Shimo-Meguro, Meguro-ku,Tokyo 153-0064, Japan0120 191014 or 81 3 5437 ale Semiconductor China LtdExchange Building 23FNo. 118 Jianguo RoadChaoyang DistrictBeijing 100022China 86 10 5879 [email protected] Literature Requests Only:Freescale Semiconductor Literature Distribution CenterP.O. Box 5405Denver, Colorado 802171-800-441-2447 or 1-303-675-2140Fax: group.comDocument Number: AN3585Rev. 1.107/2008Information in this document is provided solely to enable system and software implementers to useFreescale Semiconductor products. There are no express or implied copyright licenses grantedhereunder to design or fabricate any integrated circuits or integrated circuits based on the informationin this document.Freescale Semiconductor reserves the right to make changes without further notice to any productsherein. Freescale Semiconductor makes no warranty, representation or guarantee regarding thesuitability of its products for any particular purpose, nor does Freescale Semiconductor assume anyliability arising out of the application or use of any product or circuit, and specifically disclaims anyand all liability, including without limitation consequential or incidental damages. “Typical” parametersthat may be provided in Freescale Semiconductor data sheets and/or specifications can and do varyin 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.Freescale Semiconductor does not convey any license under its patent rights nor the rights of others.Freescale Semiconductor products are not designed, intended, or authorized for use as componentsin systems intended for surgical implant into the body, or other applications intended to support orsustain life, or for any other application in which the failure of the Freescale Semiconductor productcould create a situation where personal injury or death may occur. Should Buyer purchase or useFreescale Semiconductor products for any such unintended or unauthorized application, Buyer shallindemnify and hold Freescale Semiconductor and its officers, employees, subsidiaries, affiliates, anddistributors harmless against all claims, costs, damages, and expenses, and reasonable attorneyfees arising out of, directly or indirectly, any claim of personal injury or death associated with suchunintended or unauthorized use, even if such claim alleges that Freescale Semiconductor wasnegligent regarding the design or manufacture of the part.Freescale and the Freescale logo are trademarks of Freescale Semiconductor, Inc. All otherproduct or service names are the property of their respective owners. Freescale Semiconductor, Inc. 2007, 2008. All rights reserved.

successful radio PCB design using the MC13853 LNA. The MC13853 has three bands, a low band and two high bands, in a QFN16 package. The most critical aspects of radio frequency (RF) circuitry are addressed and it is highly recommended to follo