Download to read offline
More Related Content
Similar to BGA Land Pattern Design for Manufacturability
BGA Land Pattern Design for Manufacturability
- 1. 1 of 7 BGALand Pattern Design For Manufacturability Paul W. Ave Introduction This paper outlines and compares the basic characteristics of Ball Grid Array or “BGA” packages, and lists in guideline form how to design for manufacturability a specific BGA land pattern on a given part package. BGA Overview Basically there are two main categories that BGA packages fit into. First the package either has a “Collapsible ball” or it has a “Non-Collapsible ball”. Typically which type of ball chosen for a given package is usually dependent upon the magnitude of difference between the Coefficient of Thermal Expansion, or CTE, of the BGA package’s substrate and the “motherboard’s” substrate. These type of devices are most commonly mounted on tetrafunctional Flame Retardant epoxy based laminates such as FR-4 and are usually designed as such. For relatively small CTE deltas, the component mounting balls are comprised of the eutectic alloy 63%Sn/37%Pb with a melting point of 183 C or a the near eutectic alloy 62%Sn/36%Pb/2%Ag with a melting range of 179-189 C. This is the reason for the label of “Collapsible Ball” because these type of alloys will melt in the range of a typical FR-4 assembly’s Infra-Red or “IR” reflow temperatures. For relatively high CTE deltas the component mounting balls are comprised of the alloy 10%Sn/90%Pb with a melting range of 268-302C. This type of alloy is outside the normal IR reflow temperature ranges and does not melt or is “Non-Collapsible”. Please refer to Table 1 for some example details. Table 1 BGA Package Substrate ~ x,y CTE ppm/C Motherboard Substrate FR4 ~ x,y CTE ppm/C DELTA Ball Type Bismaleimide-Triazine or “BT” plastic 15 17 2 “Collapsible” 63/37 or 62/36/2 Ceramic Material 6 17 11 “Non-Collapsible” 10/90 The thresholds for determining the relative low and high CTE delta levels would be based on what type of service life a particular BGA is expected to have. One particular study tested a CBGA with 10/90 balls and an equivalent CBGA with 62/36/2 balls. The components were tested under similar conditions and the data generated from the experiments predicted 175% more thermal cycles using the 10/90 balls versus using 63/36/2 balls. Please reference Table 2 for details. Table 2 Joint fatigue life predictions for 25 to 55C projected from 0 to 100C ATC data.1 Sphere Metallurgy PWB Finish 100 ppm Failure Cycles 10/90 benzotriazole 7550 62/36/2 benzotriazole 2750 The main reason to use a “Non-Collapsible” ball is to minimize the effects of concentrated strain on the various ball interfaces. This is achieved by maintaining a relatively fixed height equal to the ball diameter or greater and by using an alloy with a relatively high ductility to help relieve the induced strain. The main reason for not using a “Non Collapsible” ball under less strenuous conditions is 1) they are more difficult to rework, both from the part standpoint and the motherboard standpoint. The part must have any missing balls reattached, and the motherboard must have the attachment land area prepped and re-pasted during a rework operation. This is not always practical or feasible on a populated assembly. 2) They are more sensitive to coplanarity issues between the part and the motherboard typically requiring more solder paste volume and/or solder paste inspection prior to a part’s placement on a motherboard. A “Collapsible-Ball” part allows for much more process flexibility in paste application, IR reflow and rework if needed.
- 2. 2 of 7 Thechoice of what type of substrate is used on a part is primarily the part manufacturer’s choice based on how much heat the part’s die will need dissipated, and other factors such as the allowable levels of parasitic inductance and capacitance. Typically ceramic or similar type materials have been the choice for devices over 5 watts in power and have been shown to have better inductance characteristics due to shorter internal bond wires. The greatest point of shear strain and the most likely point of first time solder joint failure for a particular part package is again related to the CTE mismatch of the part and the motherboard’s substrate. Basically for ceramic type parts mounted on FR-4, the greater the distance you are from the “Neutral Point” (DNP) which in these cases is from the center of the part package outward, the higher the shear strain on the solder joint. So in other words, the peripheral areas or the outside solder joints should show the first fatigue failures. BT plastic parts will show failures on a relatively small DNP or somewhere on the inside of the ball array nearest the part’s silicon die. Refer to Figure 1. Figure 1 FIRST FAILURES OCCUR AT THE JOINTS FARTHEST FROM THE NEUTRAL POINT FIRST FAILURES OCCUR AT THE JOINTS CLOSEST TO THE NEUTRAL POINT BT PLASTIC CERAMIC NP NP The second main category of description for BGAs has to do with how the balls on the part are oriented. They can be configured either as “Full Grid” or “Perimeter” parts with ball spacings or pitches typically at 1.5 mm, 1.27 mm, and 1.0 mm. The Full Grid parts are usually the higher pitch parts starting at 1.5mm and below. The Perimeter parts usually have the smaller ball pitches at 1.27 and below which allows them to achieve a greater number of balls per square inch, and are easier to route during pc-board layout than a comparable Full Grid Part. The increase in routability is because of the open area available toward the center of the part. Please refer to Figure 2 for examples of some common part ball layout configurations available. Figure 2 N P R G K M L J H F E D C B 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 A .060in(1.5mm) .050in(1.27mm) FULL GRID 225 BGA PERIMETER 256 BGA
- 3. 3 of 7 DFMLayout Concerns for BGAs There are two main areas to consider when laying out and creating a BGA land pattern for a PC board assembly. First, you want to consider how you are going to route or fan out the land pattern for the part. This decision involves a compromise between the desired cost of the board and the limiting physical characteristics of the part. The ideal situation would be to create a layout that involved a PC board with a minimal layer count and included the most cost effective trace widths and via sizes while continuing to provide a highly reliable and easily manufactured assembly. Which, is sometimes easier said than done with the higher ball count lower pitch devices. Listed in Table 3 are some relative cost comparisons between different board lay-up scenarios. Table 3 compares boards that are the same size and have the same number of holes. It is clearly evident, that layer count has the most significant impact overall on the PCB cost followed by trace width and hole size as the next contributing factors. An eight layer PCB for example can cost over twice as much as a comparable four layer PCB. Table 3 Relative PCB Cost Comparisons 4 LAYER 6 LAYER 8 LAYER Minimum Hole/Pad 18/36 18/30 13.5/24 18/36 18/30 13.5/24 18/36 18/30 13.5/24 8/8 100% 102% 106% 158% 160% 163% 204% 206% 210% Minimum 6/6 101% 103% 107% 159% 161% 163% 205% 207% 211% Lines/Spacing 5/5 108% 109% 113% 164% 166% 169% 213% 215% 219% You mainly have three types of balls to route on any BGA part. They are power, ground, and signal or I/O pins. The board complexity will grow as the number of pins or balls increase, and as the pitch between the balls decreases. A cost effective design would focus on routing the signal balls on the outer layers of the PCB and connecting the power and ground connections down to inner layer power and ground planes. The second main area of layout concern is related to manufacturing and rework. The BGA’s position on a given assembly can be crucial in assembly and rework operations. The component must be located in an accessible area, and in a position where manufacturing defects are kept at a minimum. Also, proper part clearances must be maintained to allow for any rework nozzles to come near or in contact with the component for any needed part removal. The Ball Mounting Pad There are basically two categories of pad design for the part balls to mount onto. One being a pad that is called a “Solder-Mask Defined” or SMD pad. The other being called a “Non-Solder-Mask Defined” or NSMD pad. Please refer to Figure 3 for pictorial example. The NSMD pad has a number of advantages over the use of a SMD pad. The two most notably being 1) for an equivalent ball mounting area a NSMD pad will take up less board real-estate than a SMD pad. Figure 3 shows that a SMD pad requires approximately .010”(.254mm) more diameter or 4.24 X 10-4 in2 of copper area. The extra area saved using a NSMD pad can prove to be invaluable for the routing of signal traces. 2) The NSMD defined pad has been shown in several studies using PBGAs and CBGAs to provide a more reliable solder joint connection than an equivalent SMD pad. The reason for this improvement is thought to be the solder stress concentration reduction associated with NSMD pads. The singularity point where the solder attaches to the pad at an approximately right angle on an SMD pad is replaced by an acute stress concentration point for the NSMD pads2 . One particular study done using different vendor PBGAs showed SMD pad solder joint failures at 900 thermal cycles earlier than the equivalent NSMD pads. However, the rate at which the SMD samples failed was less than that of the devices using NSMD pads3 . One advantage that a SMD pad does have over a NSMD pad however is that a SMD pad provides better hold down for a pad and therefore provides less of a risk of the pad lifting during a rework operation. Figure 3 °X DIA.°X+.010"(.254mm)DIA. SMD PAD NSMD PAD
- 4. 4 of 7 Designingthe BGA Footprint For each given category of pad there are essentially three types of configurations. First is a single pad without a trace not necessarily connected to anything that provides a mechanical connection. Second is a single pad with a signal trace connection, and third is a single pad with a via attachment to allow a connection to a remote layer. Please refer to Figure 4 for some pictorial examples of the pads. Figure 4 Different Types of Ball Mounting Pads SINGLE PAD WITHOUT TRACE SINGLE PAD WITH VIA CONNECTION SINGLE PAD WITH TRACE The number of traces that can be routed between two given pads is a function of the part ball pitch and the chosen finished pad and via sizes. Originally when BGAs were first introduced, part vendor’s recommended nominal pad sizes at or near the ball size of the part. Since then additional studies have been conducted to determine the long term reliability of different pad configurations with reduced sizes. Having the flexibility to use smaller pad sizes allows a designer to use the most economical technology to achieve the parts layout. One particular study performed on PBGAs with nominal ball diameters of 0.030”(0.762mm), found that NSMD pad diameters as small as 0.014”(0.356mm) could be used without a degradation in the solder joint reliability. Due to the increased stand-off height achieved with the smaller pads, it is believed the smaller pads may show improved reliability over the larger control pad samples used which were 0.024”(0.610mm) in diameter.4 The main concerns to be aware of are that a finished pad will have a tolerance of approximately 0.0015”(0.0381mm). Which means that if you specify the artwork to have a 0.020”(0.508mm) pad diameter, you could see a range of 0.0185”(0.470mm) - 0.0215(0.546mm) for finished pad sizes on the PCB. Another concern is the reduced amount of adhesion you will have by decreasing the available surface area of the pad, which can lead to an increased number of lifted pads during any needed rework operations. The same study that looked at reduced pad diameters also took this into consideration, and tested the various pad sizes under rework operations. A rework process was developed to accommodate NSMD 0.018”(0.457mm) - 0.024”(0.610mm) pads. Although a low level of pad lift on the 0.014”(.356mm) and 0.016”(0.406mm) pads was observed, the reliability of all other reworked joints (0.014”(.356mm) - 0.024”(0.610mm) surpassed 1000 cycles of solder joint reliability testing.4 The conditions of the solder joint reliability test were -25C/100C with 15 minute dwells at each extreme. Any resistance reading increase of 100% from the initial continuity reading was considered a failure. Once a study completes 1000 thermal shock cycles with no failures, the solder joint reliability is considered acceptable for low power PC applications (ASICs, chipsets, memory).4 The examples that follow in this paper will focus around the application of a 0.020”(0.508mm) pad for use with a part having a nominal ball diameter of .030”(0.762mm) spaced at a pitch of .050”(1.27mm). Also it should be noted that the data referenced in this paper was applied to specific situations. Although theoretically the same designs could be applied to similar conditions, it is recommended that anyone’s particular application be tested or qualified in the intended design and process environment. This always makes good engineering sense. Typically the outside rows and columns of a given part contain the majority of the signal balls. Table 4 contains some examples of different options. Listed in bold type in each of the row scenario columns of the table are the total number of balls for a Perimeter package or it can be used to represent the number of signal balls on a Full Grid package. The RXC dimension specifies the number of balls per row and column for a given part array. Table 4 Examples of Different BGA Configurations Body .050” (1.27 mm) Pitch Size/Side 4 Row 5 Row 6 Row 1.075” (27 mm) 256 20X20 300 20X20 336 20X20 1.220” (31mm) 304 23X23 360 23X23 408 23X23 1.378” (35mm) 352 26X26 420 26X26 480 26X26 1.476” (37.5mm) 384 28X28 460 28X28 528 28X28 1.575” (40mm) 416 30X30 500 30X30 576 30X30 1.673” (42.5mm) 448 32X32 540 32X32 624 32X32 The body sizes listed are square and can reach sizes in excess of 1.673”X1.673”(42.5 mmX42.5mm). A user should use caution when selecting a larger size package to be aware that a given pick and place machine used in the assembly process has certain size and weight limitations which these type packages may approach. Table 5 lists some recommendations for the most economical scenarios of via/annular ring sizes, and lines/spacing widths that can be used with .020”(.508mm) pads on .050”(1.27mm) pitch spacings.
- 5. 5 of 7 Table5 Specification Recommendations for .050”(1.27mm) Spaced .020”(.508mm) Diameter Pads Number of Signal Rows 4 5 6 Via Annular Ring/Drill Diameters (Dr/Dv mils) 36/18 30/18 24/13.5 Lines/Spacings Widths (Wl/Ws mils) 6/6 6/6 5/5 Max Number of Traces Between Top Pads 1 2 2 Max Number of Traces Between Bottom Pads 1 1 2 Figure 5 shows three examples of what the top layers of land pattern footprints would look like for a Full Grid BGAs with four, five, and six signal rows with .050”(1.27mm) pitch spacings. Figure 6 shows what the bottom layers and their various configurations would look like for the same type parts. All of the BGA pads with vias have their holes interstitially positioned and are located between the centers of the surrounding pads. Please refer to Figure 7 for details on the exact dimensions. Figure 7 Exact Dimensions Diagram .025"(.635mm) .025"(.635mm) .050"(1.27mm) .050"(1.27mm) Dr Dv .020(.508mm) Ws Wl .050"(1.27mm) The via annular ring is designed to neck down and meet the mounting pad at the outside of the pad’s solder-mask clearance. The width of the narrowest section of the neck can be in the range of approximately 25%-75% of the mounting pad diameter . This neck down section is the most likely point that a fatigue crack will begin to propagate since it is in essence a solder-mask defined area which will have the same undesirable stress concentrations associated with NSMD pads. However, the widest design will provide some added resistance to pad lifting. Also on the bottom side it is recommended that the via annular ring connection to a trace have a fillet or neck down section. This will reduce the possibility of drill breakout which can cause discontinuity between a via and a trace. Via hole pads that are not used on the bottom layer will be used to connect to internal layer power and ground planes. Figure 5 Top Layer Full Grid BGA Land Pattern for a .050”(1.27mm) Pitch Part 4 Signal Rows 5 Signal Rows 6 Signal Rows Figure 6 Bottom Layer Full Grid BGA Land Pattern for a .050”(1.27mm) Pitch Part 4 Signal Rows 5 Signal Rows 6 Signal Rows Solder-Mask Clearances The recommended nominal solder-mask clearance for a given NSMD pad is .006”(.152mm) greater than the pad or for these examples .026”(.660mm). The recommended solder-mask clearance for the via on both sides of a PCB is equal to the particular via’s annular ring diameter. A wider
- 6. 6 of 7 clearanceequal to that used on the mounting pad could be used, but the risk of exposing the copper on closely spaced traces will be greater. Remember, that every feature has registration and artwork tolerances. Please refer to Figure 8 for more details on mask clearances. Figure 8 Solder Mask Clearances on Various Features MASK CLEARANCE = VIA ANNULAR RING DIA. MASK CLEARANCE = PAD SIZE + .006"(.152mm) Strategic Component Placement Where you place a component can actually affect an assembly’s manufacturability and the number of defects created for that assembly. The larger board assemblies approximately 8”(203.2mm) wide and greater can be more prone to warpage while suspended between two conveyor belts. Assuming a relatively even top side mass distribution, the board will naturally follow the shape of a catenary or parabolic arch as it begins to approach its glass transition temperature. This shape would show a more pronounced warp towards its center. FR-4 begins to soften around 135C which is before the melting point of the 63/37 solderpaste. So, it is a good practice on the wider boards approximately 8”(203.2mm) or greater to position a part toward the outside edges of the PCB. Figure 9 shows an exaggerated example of the potential problem. The problem would be more severe for the larger size BGAs, and for those parts that are made of more rigid materials with Non-Collapsible balls. The components should be positioned on the outside to fit within your normal DFM guidelines of machine and conveyor clearances. Figure 9 Board Warpage Comparison The PCB Outside Edges vs. The PCB Center An Exaggerated View Another advantage to positioning the component towards the outside of the PCB is that it will allow for easier accessibility should any troubleshooting or rework be required. Rework Clearances The part’s footprint should also be laid out taking into consideration the clearances necessary to allow for any needed rework machine to come in close contact with the intended part. The first consideration would be for the top side of the PCB. A good default value would be a .100”(2.54mm) component keepout zone around the maximum outside dimension of the part. One aide that a designer can use would be to incorporate an outline box equal to the maximum outside dimension of a part plus the nozzle clearance onto the silkscreen layer of the part’s footprint. It would also be a good practice to add the row and column alphanumeric numeric ball identifiers to help anyone in troubleshooting, and for identifying correct part polarity on the PCB. Figure 10 shows a pictorial example of this. Please note that the circular pads shown in Figure 10 are there merely for reference, and normally would not be part of the final silkscreen image. Figure 10 BGA Silkscreen Layer with Some Recommended Part Clearances N P R G K M L J H F E D C B 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 A X X SILKSCREEN OUTLINE X=MAX. PART WIDTH + NOZZLE CLEARANCE 0.100"(2.54mm) 0.100"(2.54mm) 0.625"(15.875mm) MAX ALLOWABLE PART HEIGHT UNDER PART The bottom side of the PCB assembly will also have maximum component height restrictions when bottom side heat diffusers are used to heat a part from the underside of an assembly. Though not always necessary on PBGAs it is almost imperative to use a bottom side diffuser with CBGAs. Summary BGAs have been adopted as a viable replacement to high I/O fine pitch QFPs. The components themselves however, can sometimes prove to be a challenge as far as being a cost effective alternative. To overcome this, designers must understand the basic characteristics of an intended part, and be aware that through proper considerations they can develop a cost effective yet highly reliable assembly. The basis for this is rooted in proper footprint design for manufacturability. Acknowledgments Special acknowledgments go to Jason Brown of Peak Plastics , Andrew Mawer of Motorola, Cindy Ramirez, and Pat Hession of Compaq Computer for data, information , and support provided for this paper. References 1. D.R. Banks, T.E. Burnette, R.D. Gerke, E. Mammo, and S. Mattay. “Reliability Comparison of Two Metallurgies for Ceramic Ball Grid Array” , Proceedings of the 1994, International Conference on Multichip Modules, Denver, CO pp. 529-534. 2. A. Mawer, D. Cho, and R. Darveaux. “The Effect of PBGA Solder Pad Geometry On Solder Joint
- 7. 7 of 7 Reliability”,Proceedings of the 1996, Surface Mount International, San Jose, CA, p.135. 3. C. Ramirez, and S. Fauser. “Fatigue Life Comparison of The Perimeter and Full Plastic Ball Grid Array”, Proceedings of the 1994, Surface Mount International, San Jose, CA, p. 259. 4. J.D. Brown, and B. Bromley. “PBGA Solder Joint Reliability/Manufacturability as a Function of PCB Pad Size”, Proceedings of the 1996, Surface Mount International, San Jose, CA, pp. 162-165.