BGA chip PCB design

PCB Design of 0.5mm Pitch BGA Chip

With the rapid development of microelectronic technology and technology, high-density ball grid array (BGA) devices have the advantages of small package size, large number of pins per unit area, strong impact resistance of solder balls, good signal integrity and heat dissipation performance, and smaller Therefore, it has been more and more widely used in communication networks, consumer terminals, military electronics, programmable logic devices and other fields. Today, the number of pins of BGA devices visible on the market can reach up to more than 2,000, and the pin pitch can be as small as 0.3mm. The higher pin count and smaller pin pitch make hardware designers face great challenges, and must adopt More advanced PCB technology to meet design requirements, and the most effective way to increase PCB density is to reduce the number of through holes, and accurately set blind holes and buried holes to achieve. This paper takes a project using the EPLD chip of Lattice Company as an example, focusing on the consideration of high-speed signal reflow, stack design, processing technology, etc., and carries out the specific PCB design of the 0.5mm pitch BGA package, which better realizes the single board work performance.

1. 0.5mm pitch BGA

The single board design scheme of a certain project adopts the programmable logic device (EPLD) chip of Lattice Company. The number of pins of this BGA device is 256, the size is 10mm×10mm, and the pad spacing is 0.5mm.

As shown in the figure: the pad diameter is 0.3mm, the center point distance between two adjacent pads is 0.5mm, the edge distance is 0.2mm (7.87mil), and the center point distance between two adjacent diagonal pads is 0.47mm. Obviously, the thinner the copper wire between the pads, the smaller the distance between the copper wire and the pad, the more difficult the processing technology, the higher the cost of the PCB, and the worse the reliability. At present, the mature process level of mainstream printed board manufacturers is that the width of the copper wire is 0.1mm (4mil), and the distance between the copper wire and the pad is 0.1mm (4mil). To draw a copper wire, the distance required is at least 0.3mm (12mil). Obviously, it is not feasible to directly draw a copper wire between two pads. In addition, the minimum metallized through hole size of domestic mainstream printed board manufacturers is 0.2mm in inner diameter and 0.4mm in outer diameter, which is larger than the 0.4mm distance between two adjacent diagonal pads in Figure 1, so the conventional lead from the pad The punching method is also not feasible.

2. BGA chip PCB design scheme

In view of the fact that it is difficult to draw lines directly between the two pads of the 0.5mm BGA chip or the pads are fanned out directly, and because the PCB processing cost has risen sharply after the blind hole technology is adopted, it is decided to use the hole in the board and the special rule area of the BGA. Blind hole technology, that is, directly punch a blind hole on the 0.5mm BGA chip pad to the next second layer, and then continue wiring from the second layer pad.

Using laser drilling technology to make blind holes is mature and reliable, and is widely used in the production of 0.15mm micro-vias. However, the depth of blind holes made by laser drilling is limited, and generally cannot exceed 0.075m. Therefore, in this design, 1~2 layers of blind holes Holes, the thickness of the medium between the top layer and the second layer is less than 0.075m, sequential lamination process method.

The production of blind vias requires high soldering consistency and reliability. In order to prevent poor solderability caused by copper oxidation, the pads of all devices must be treated with protective coating or electroplating. At present, a low-cost application technology to enhance the success rate of welding is the "OSP (Organic Solderability Preseraties, Organic Solderability Preseraties) + Immersion Gold" solution. OSP is to use chemical methods to form an organic film on the clean bare copper surface. The organic film has good oxidation resistance, thermal shock resistance and moisture resistance, and prevents the metal copper surface from being oxidized in a normal environment; but in the subsequent welding high temperature environment , this organic film must be easy to be quickly removed by flux, so that the newly exposed clean metal copper surface will immediately combine with molten solder to form a firm solder joint in a very short time. Immersion gold is to electroplate a layer of nickel gold on the PCB pad. Since nickel gold has a stronger ability to absorb solder than copper, it can significantly enhance solderability.

The sequential lamination method has certain process limitations, and it cannot be interconnected arbitrarily, so when designing a high-density PCB, use as few blind holes as possible, and the blind hole interconnection used should not exceed half of the total number of layers, which can reduce lamination. frequency and processing difficulty. In order to reduce the number of blind holes, the outermost pin pads of the 0.5mm BGA chip in the design are first drawn through through holes, and the inner sub-pins are wired through blind holes.

3. Practical application of BGA chip PCB

In fact, the return path of the high-speed signal must be along the path with the least impedance. The return path with the least impedance is generally located on the ground plane closest to the lower part of the signal conductor. The smaller the total loop area, the smaller the external electromagnetic interference and the less susceptible it is to outside interference. Because blind holes need to be made on the pads of 0.5mm BGA chips, local area wiring grooves are formed on the second layer ground plane of the PCB, which will definitely destroy the integrity of the ground plane. For any signal vertically passing through the slots in this area in space, its return path will have to bypass this area, thereby greatly increasing the return area. In order to reduce the impact of slotting in this area, PCB layout and wiring must be fully considered. Try not to place the BGA chip near the center of the board to avoid serious impact on other signal wiring with the slotted ground plane. The single-board PCB design thickness is 1mm, and the number of layers is 6 layers.

The 0.5mm BGA chip is placed on the top layer TOP, the second layer is the ground plane, and the dielectric thickness between the top layer and the ground plane is set at 0.071mm (2.8mil) (less than 75m). Since the design scheme needs to penetrate the blind hole to the second layer, and then continue to open the hole on the second layer to switch to other signal layer wiring, so only a small area in the second layer needs to be slotted. In order to reduce the difficulty of wiring, the width of the copper wire in the 0.5mm BGA area on the second layer is 4mil, and the via type is designed with a via hole with an inner diameter of 0.2mm and an outer diameter of 0.4mm. According to the calculation of the impedance design formula, when the width of the copper wire is 0.1mm (4mil), the thickness of the copper on the plane layer can only be 18m.

Summarize

For 0.5mm BGA chips, after using the single-board local blind hole technology in PCB design, the processing cost will not increase much. From the production situation of 10 R&D prototypes using this EPLD device, there is no single board failure caused by poor lead-free soldering of the chip at a high temperature. The control signals from the pins of the chip have also passed strict timing function tests, and the consistency and stability of the board are also very good, with no warping or pad breakage occurring.

Since the "hole in the board" and blind hole technology will definitely increase the additional PCB production cost and design difficulty, so in the stage of system solution design and chip selection, it is necessary to pay close attention to the package size of the chip. In the schematic diagram and PCB design stage, it is necessary to use the I/O pin functions of the BGA chip reasonably, so that each signal is distributed as evenly as possible in the entire BGA chip area. Chips are laid out according to the principle of proximity to avoid excessively long traces, so as to reduce the difficulty of PCB design. At the same time, in order to ensure the best soldering effect of the 0.5mm BGA chip, soldering must be started within 24 hours after the bare PCB is unsealed, otherwise the bare PCB will be re-packed in a vacuum-sealed package.

The above is the PCB design technology of 0.5mm pitch BGA chip introduced by Shenzhen Zuchuang Microelectronics Co., Ltd. If you have software and hardware function development needs for smart electronic products, you can rest assured to entrust them to us. We have rich experience in customized development of electronic products, and can evaluate the development cycle and IC price as soon as possible, and can also calculate PCBA quotations. We are a number of chip agents at home and abroad: Songhan, Yingguang, Jieli, Ankai, Quanzhi, realtek, with MCU, voice IC, Bluetooth IC and module, wifi module. We have hardware design and software development capabilities. Covering circuit design, PCB design, single-chip microcomputer development, software custom development, APP custom development, WeChat official account development, voice recognition technology, Bluetooth wifi development, etc. It can also undertake the research and development of smart electronic products, the design of household appliances, the development of beauty equipment, the development of Internet of Things applications, the design of smart home solutions, the development of TWS earphones, the development of Bluetooth earphone speakers, the development of children's toys, and the research and development of electronic education products.