AN10778

AN10778 PCB layout guidelines for NXP MCUs in BGA packages Rev. 2 — 15 April 2011 Application note Document information Info Content Keywords LPC175x, LPC176x, LPC177x, LPC178x, LPC181x, LPC182x, LPC183x, LPC185x, LPC431x, LPC432x, LPC433x, LPC435x, LPC2220, LPC2292, LPC2364, LPC2368, LPC2458, LPC2468, LPC2470, LPC2478, LPC2880, LPC2888, LPC3130, LPC3131, LPC3141, LPC3143, LPC3152, LPC3154, LPC3180/01, LPC3220, LPC3230, LPC3240, LPC3250, LH79524, LH7A400, LH7A404, TFBGA100, TFBGA144, TFBGA208, TFBGA180, TFBGA296, LFBGA208, BGA256, LBGA256, LFBGA256, LFBGA324, LFBGA320, Layout Guidelines, BGA, PCB, Fanout This application note is focused on Printed Circuit Board (PCB) layout issues when using (L)(LF)(TF)BGA packages from the NXP LPC Microcontroller family. Abstract NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Revision history Rev Date 2 1 20110415 20090122 Description Added information for LPC1700/1800/4300 LBGA256 package. Initial release. Contact information For more information, please visit: http://www.nxp.com For sales office addresses, please send an email to: salesaddresses@nxp.com AN10778 All information provided in this document is subject to legal disclaimers. © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 2 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages 1. Introduction The plastic Ball Grid Array (BGA), including Low-profile Ball Grid Array (LBGA), Lowprofile Fine pitch BGA (LFBGA) and Thin-profile Fine pitch BGA (TFBGA) packages have become, for many applications, the first choice for designers requiring medium to high pin-count IC packaging. For this reason many of the LPC Family of Microcontrollers are available in the LBGA, LFBGA or TFBGA package. When comparing it to other common alternative packages, such as the Quad Flat Pack (QFP), the (L)(LF)(TF)BGA device has many advantages, such as: • The (L)(LF)(TF)BGA has no easy-to-bend leads that can cause deviation from coplanarity. • The (L)(LF)(TF)BGA is typically 20 % to 25 % smaller than an equivalently functional QFP. • Resolution and smearing problems with respect to the stencil-print process are less because the pitch is larger, and the apertures are circular. • The self-alignment property of the component results in a large process window for automatic placement. • The (L)(LF)(TF)BGA is compatible with today’s assembly techniques, which means that no adjustments are necessary to standard machines or materials. 1.1 Scope The scope of this application note is focused on Printed Circuit Board (PCB) layout issues when using (L)(LF)(TF)BGA packages from the NXP LPC Microcontroller family. Including: • Recommended footprint patterns for the TFBGA180, TFBGA208, TFBGA296, LBGA256 and LFBGA320 pin packages. • Recommended trace, space and via size for fan-out routing of the TFBGA180, TFBGA208, TFBGA296, LBGA256 and LFBGA320 pin packages It is recommended that other assembly topics such as the solder paste chemistry, reflow solder profile and solder paste stencil etching, which are affected by all components on the board level assembly and not limited to the Microcontroller BGA alone, be a collaborative effort between the system designer and the assembly contractor. 2. BGA package description A cross section of the typical (L)(LF)(TF)BGA is shown in Fig 1. AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 3 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Fig 1. (L)(LF)(TF)BGA cross section This application note applies to BGA packages listed in Table 1. Table 1. BGA packages NXP outline code SOT1018-1[4] SOT740-2[6] SOT926-1[2] SOT569-2[2] SOT570-2[2] SOT950-1[2] SOT1019-1[5] SOT1020-1[5] SOT1048-1[1] SOT1021-1[5] SOT930-1[2] SOT640-1[3] SOT824-1[2] Outline dimensions 17 x 17 x 1.35 mm 17 x 17 x 1.55 mm 9 x 9 x 0.7 mm 12 x 12 x 0.7 mm 12 x 12 x 0.8 mm 15 x 15 x 0.7 mm 14 x 14 x 1.27 mm 14 x 14 x 1.25 mm 15 x 15 x 0.7 mm 17 x 17 x 1.25 mm 12 x 12 x 0.7 mm 10 x 10 x 0.8 mm 13 x 13 x 0.9 mm Ball pitch 1.0 mm 1.0 mm 0.8 mm 0.8 mm 0.8 mm 0.8 mm 0.8 mm 0.8 mm 0.8 mm 0.8 mm 0.65 mm 0.5 mm 0.5 mm Ball diam 0.50 mm 0.50 mm 0.45 mm 0.45 mm 0.45 mm 0.45 mm 0.45 mm 0.45 mm 0.45 mm 0.45 mm 0.40 mm 0.30 mm 0.30 mm Ball configuration 16 x 16; full matrix 16 x 16; full matrix 10 x 10; full matrix 13 x 13; partial matrix 14 x 14; partial matrix 17 x 17; partial matrix 16 x 16; partial matrix 16 x 16; full matrix 18 x 18; partial matrix 20 x 20; partial matrix 17 x 17; partial matrix 18 x 18; partial matrix 24 x 24; partial matrix Package name BGA256 LBGA256 TFBGA100 TFBGA144 TFBGA180 TFBGA208 LFBGA208 LFBGA256 TFBGA296 LFBGA324 TFBGA208 TFBGA180 LFBGA320 [1] [2] [3] [4] [5] [6] Reference JEDEC MO-216 Reference JEDEC MO-275 Reference JEDEC MO-195 Reference JEDEC MS-034 Reference JEDEC MO-205 Reference JEDEC MO-192 AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 4 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages 3. BGA footprints When building a BGA footprint the number one consideration is ensuring the ball pattern and outline matches the device package. This includes correct orientation of ball A1, matching all ball column x row locations, and the ball-to-ball pitch. Solder joint reliability is also of primary concern. For cost sensitive applications, minimizing the number of PCB layers required to route the BGA is a consideration. The BGA land pattern footprint plays a key role in solder joint reliability, and the number of PCB layers required to route the balls. 3.1 Land pad design The PCB BGA land pads have to be designed to ensure solder joint reliability and provide optimum manufacturability. The two basic types of BGA land pad design are: • The Solder Mask Defined (SMD) land pad • The Non-Solder Mask Defined (NSMD) land pad; recommended type for PCB 3.1.1 Solder Mask Defined (SMD) land pad The SMD type of BGA land pad design is characterized by the copper pad being larger than the solder mask opening above this pad. Thus the solder joint area of the land pad is defined by the opening in the solder mask. 3.1.2 Non-Solder Mask Defined (NSMD) land pad The NSMD type of BGA land pad design is characterized by the copper pad being smaller than the solder mask opening. Thus the solder joint area of the land pad is defined by the size of the land pad. The solder mask clearance around the land pad must be large enough to ensure that no solder mask overlaps the land pad. Typical solder mask to land pad clearance is in the range 0.06 mm to 0.075 mm, depending on the PCB manufacturer’s solder mask alignment tolerance. Fig 2. Solder mask vs. non-solder mask defined land pad AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 5 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages 3.2 Recommended BGA footprint The NSMD type land pad is recommended for the PCB BGA footprint. In addition to the top surface of the land pad, the reflowed solder paste will wet to the side wall making a mechanically stronger solder joint than the SMD type pad. The smaller NSMD land pad also leaves more space for routing traces between the land pads. It has been shown that matching the solder joint area of the PCB land pad to that on the BGA package substrate equalizes the ball solder joint stress between the BGA package and PCB land pad thereby reducing the chance of a solder joint stress crack. All of the BGA packages referenced in this application note use SMD type pads. The NSMD type pads on the PCB should be approximately 10 % to 15 % smaller than the SMD pads on the BGA to achieve equalized stress. This difference between the BGA package SMD pad and recommended PCB NSMD pad for each BGA package is reflected in Table 2. A generic BGA footprint is shown in Fig 3, and the specific dimensions for each BGA package are listed in Table 2. Fig 3. Generic BGA footprint AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 6 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Table 2. Recommended BGA footprints Ball Pitch Ball diameter BGA substrate Land diameter 0.45 0.4 0.4 0.4 0.4 0.4 0.4 0.4 0.4 0.4 0.26 n/a 0.25 PCB land pad Solder mask diameter 0.45[4] 0.35[4] 0.35[4] 0.35[4] 0.35[4] 0.30[4] 0.30[4] 0.35[4] [6] 0.30[4] [7] 0.30[4] 0.25[5] 0.25[5] 0.25[5] diameter 0.6 0.5 0.5 0.5 0.5 0.42 0.42 0. 5 0. 42 0.42 0.37 0.36 0.36 17.6 9.6 12.6 12.6 15.6 14.6 14.6 15.6 15.6 17.6 12.4 10.4 13.4 Outline X & Y Package Name (L)BGA256 TFBGA100 TFBGA144 TFBGA180 TFBGA208 (SOT950-1) LFBGA208 LFBGA256 TFBGA296 TFBGA296 LFBGA324 TFBGA208 (SOT930-1) TFBGA180 (SOT640-1) LFBGA320 1.0 0.8 0.8 0.8 0.8 0.8 0.8 0.8 0.8 0.8 0.65 0.5 0.5 0.50 0.45 0.45 0.45 0.45 0.45 0.45 0.45 0.45 0.45 0.4 0.3 0.3 Notes: [1] [2] [3] [4] [5] [6] [7] All dimensions are in millimeters All BGA substrate land pads are SMD type All PCB land pads are NSMD type The recommended solder paste diameter is the same as the PCB land pad The recommended solder paste diameter is 0.02 mm larger than the PCB land pad Used for routing 1 trace between land pads Used for routing 2 traces between land pads AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 7 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages 4. Recommended fan-out trace / space guidelines The small pitch between BGA balls and their matrix arrangement makes it impractical to route all of the BGA balls away from the BGA on a single layer. Fan-out vias (also called escape vias) are required to route the balls to other layers on the PCB. There are several via technologies used on PCB’s. They are: Through-via, Blind via, Buried via, Micro via and In-pad via. Through-vias, where the drilled via hole goes through all layers on the PCB, cost considerably less than Blind, Buried, Micro and In-pad vias. Through-vias are generally larger than the other types of vias as well. All recommended fan-out examples in this application note use the through-via exclusively. 4.1 Recommended 1.0 mm and 0.8 mm pitch BGA via fan-out pattern For 1 mm and 0.8 mm pitch BGA’s, the recommended via fan-out pattern centers each via within the space between four adjacent BGA land pads as shown in Fig 4. Generally, a single trace is routed between adjacent BGA land pads, allowing the two outer rows of balls to be routed without a fan-out via. For BGAs with larger than 0.8 mm ball pitch one or two traces may be routed between adjacent BGA land pads, allowing the three outer most rows of balls to be routed without a fan out via. By reducing the BGA land pad, trace width and trace-to-pad space design rules for the 0.8 mm ball pitch TFBGA296, two traces may be routed between the BGA land pads. See Table 3 for the layout tool design rules for 1.0 mm and 0.8 mm pitch BGA via fan-out. Fig 4. 1.0 and 0.8mm pitch BGA Via fan-out pattern AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 8 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Table 3. BGA Pitch 1.0 mm and 0.8 mm pitch BGA layout design rules BGA land Via pad Pad Land pad Between vias to via Trace / # of traces space space 0.2 0.24 0.148 0.173 0.15 0.1 0.105 0.105 1 2 1 1 Between Land pads Trace / space 0.18 0.11 0.15 0.1 # of traces Drill size Inner plane / finished layer antihole size pad 0.3 / 0.18 0.25 / 0.1 0.25 / 0.1 0.25 / 0.1 0.800 0.695 0.695 0.695 1.0 1.0 0.8 0.8 0.45 0.45 0.35 0.30 0.55 0.485 0.485 0.485 1 2 1 2 4.2 Recommended 0.65 mm pitch BGA via fan-out pattern For 0.65 mm pitch BGA’s, the recommended via fan-out pattern centers each via within the space between four adjacent BGA land pads. Instead of placing the vias 0.65 mm apart they are placed 1.3 mm from each other, skipping every other location, and staggering them between adjacent rows, as the partial fan-out example is shown in Fig 5. With this pattern the TFGBA208 package can use 0.125 mm (0.005”) trace and space design rules. With a single trace routed between adjacent BGA land pads, the two outer rows of balls can be routed without a fan-out via. See Table 4 for the layout tool design rules for 0.65 mm pitch BGA via fan-out. (1) Note: no connect pins on the LPC3152/54 Fig 5. Recommended 0.65 mm pitch BGA via fan-out pattern AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 9 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Table 4. BGA Pitch 0.65 mm pitch BGA layout design rules BGA land pad Pad Via Land pad to Between via space vias Trace / space 0.122 0.125 Trace / space 0.125 Between Land pads # of traces 1 Drill size Inner / finished plane layer hole size anti-pad 0.2 / 0.05 0.6 0.65 0.25 0.425 4.3 Recommended 0.5 mm pitch BGA via fan-out pattern The pattern of centering the through-via within the four adjacent BGA land pads can not be used with 0.5 mm pitch BGA’s. This is due to the smallest through-via pad being too large to fit in the space available between the land pads. With a single trace routed between adjacent BGA land pads, the two outer rows of balls can be routed without a fan-out via. The two inner rows of balls must be routed to vias in the center area of the BGA and escape routed on other layers. An example fan-out of the LFBGA320 package is shown in Fig 6. See Table 5 for the layout tool design rules for 0.5 mm pitch BGA via fan-out. Fig 6. Example fan-out of LFBGA320 AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 10 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages Table 5. BGA Pitch 0.5 mm pitch BGA layout design rules BGA land pad Pad Via Land pad to Between via space vias Trace / space 0.1 0.1 Trace / space 0.08 Between Land pads # of traces 1 Drill size Inner / finished plane layer hole size anti-pad 0.2 / 0.05 0.6 0.5 0.25 0.4 5. Board cost considerations PCB cost is affected by many factors, generally increasing in cost as: 1. Overall PCB area increases 2. As the number of layers increases 3. Using in-pad via, blind via, buried via, micro via 4. As the diameter of the through-via decreases 5. As the trace width decreases below 0.125 mm (5 mils) 6. As the space between metal features decreases below 0.125 mm (5 mils) Therefore, selecting via size, trace width and spacing for fan-out routing of the BGA requires a balance between feature size, number of PCB layers and overall board area to get the most economical layout. 5.1 Area rules On many boards the design rules for via size, trace width and space for fan-out routing of the BGA may require smaller feature sizes than any other area on the board. If your layout tool is capable of defining multiple rule areas, it may be cost effective to limit the area around the BGA to the smaller feature sizes and use larger vias and larger trace widths and spacing for the balance of the board. In other words if all but the BGA fan-out can use 5 or 6 mil trace and space rules, then limiting 3 or 4 mil trace and space rules to the BGA fan-out area may have only a small cost premium. 5.2 How many PCB layers to fan-out the BGA Generally one trace is routed between adjacent BGA land pads, enabling the two outer rows of BGA balls to be routed on the same layer as the BGA is mounted on. The next two rows in can be routed on the next signal layer, provided the vias are spaced far enough apart to allow one trace between them, as is the case for the 1.0 mm, 0.8 mm and 0.65 mm recommended fan-out via patterns in Fig 4 and Fig 5. Each additional BGA row will take one additional PCB layer to fan-out. For example, the TFBGA296 has balls seven rows deep and will take 5 PCB layers to fan-out, including power and ground. Because PCB’s are constructed in even number layers, a PCB using the TFBGA296 package would require a minimum of six layers, including one split power plane and one ground plane. AN10778 © NXP B.V. 2011. All rights reserved. Application note Rev. 2 — 15 April 2011 11 of 14 NXP Semiconductors AN10778 PCB layout guidelines for NXP MCUs in BGA packages 6. BGA power and ground NXP LPC Microcontroller family devices have many power and ground pins. This is due to having multiple power domains, and the potential for large simultaneous switching currents when all 16-bit or 32-bit external data bus outputs change from all low to all high, or all high to all low, at the same time. It is recommended that the MCU VDD(core) and VDD(IO) power nets and VSSx be distributed on a plane layer of the PCB instead of routed by the thin traces, like those used for carrying other signals. BGA power and ground balls are typically routed to a near by fan-out via the same as any signal. It is recommended that the short trace between the BGA ball and fan-out via be no wider than 0.15 mm (6 mils). Although it is common to use a wider trace (0.5 mm) to route power and ground from other IC packages (SOIC, QFP, TSOP, etc.), using larger than 0.15 mm may begin to act like a heat sink that could adversely affect the solder joint. If a BGA power or ground pin must be routed more than 1 mm to get to a fan-out via, the trace should be routed the first 1mm with a