Global Sources
EE Times-Asia
Stay in touch with EE Times Asia
?
EE Times-Asia > Manufacturing/Packaging
?
?
Manufacturing/Packaging??

Optimising BGA signal routing in PCB designs

Posted: 02 Feb 2015 ?? ?Print Version ?Bookmark and Share

Keywords:Ball grid array? BGA? printed circuit board? signal routing? vias?

In some designs where electro-magnetic interference (EMI) is a concern, the external layer or top layers aren't used to route even the outer periphery. In that case the top layer is used for a ground plane. EMI includes the susceptibility of a product to fields from the outside world that couple in and radiate emissions from a product, which causes it to fail compliance tests. A product is considered EMC compliant if it satisfies three criteria:
???It doesn't interfere with other systems
???It's not susceptible to emission from other systems
???It doesn't cause interference with itself.

To prevent the product from transmitting and receiving undesired signals, it's recommended that the product be shielded. Shielding generally refers to a metallic enclosure that completely encloses an electronic product or portion of product. However, in most cases having the outer layers filled with ground plane serves the shielding purpose as it absorbs energy and minimises interference.

Via in pad for ultra-fine pitch
When using the via-in-pad technique for BGA signal escape and routing, vias are placed directly on the BGA pads and filled with conductive material, usually silver, that provides a flat surface.

The micro BGA via in pad fan-out example used here is based on 0.4 mm ball or lead pitch and the PCB is 18 layers, including eight signal routing layers. A greater number of layers is usually required for BGA routing. But in this example, the number of layers isn't an issue since fewer number of BGA balls are involved. Still, the key issue is the micro BGA's narrow pitch of 0.4mm with routing not permitted on the top layer, except for fan-outs. The goal is to fan out the micro BGA without adversely affecting PCB fabrication.

Figure 5 shows the footprint from the BGA device's manufacturer. As can be seen, the recommended pad size is 0.3 mm (12 mils), and pin pitch is 0.4 mm (16 mils). It's not possible to have the traditional dog bone fan-out pattern due to the extremely small space between the pads. Even a small size via cannot be used for a dog bone fan-out strategy; here a small size via means 6 mil drill and 10 mil annular pad. Another important mechanical limitation is board thickness, which is 93mils.

Figure 5: Footprint from the BGA device's manufacturer.

In this case, the easiest solution is using micro-via-in-pad. However, micro-via size cannot be more than 3 mils. But the 93 mils board thickness is a limiting factor. Another option is blind and buried via technology. These options will limit manufacturing choices and increase costs.

To have the option of going to different fabrication houses, drill size in a 93 mils thick board cannot go smaller than 6 mils, and trace width cannot be smaller than 4 mils. Otherwise, only a high end, exclusive board manufacturer can handle this project, at a premium. Figure 6 shows the BGA footprint associated with this example.

Figure 6: This fan-out method avoids using a high-end technique and doesn't jeopardise signal integrity. BGA pins are divided into two sections as far as internal and external pins.

The fan-out method shown in figure 6 avoids using a high-end technique and doesn't jeopardise signal integrity. BGA pins are divided into two sections as far as internal and external pins. Via-in-pad is used for the internal section, while external pins are fan-out at a 0.5mm grid. Figure 7a shows the top layer and figure 7b shows top and internal routing layers.

Figure 7a and 7b: Via-in-pad is used for the internal section, while external pins are fanned out at a 0.5mm grid. Fig. 7a shows the top layer; Fig. 7b shows top and internal routing layers.


?First Page?Previous Page 1???2???3???4?Next Page?Last Page



Article Comments - Optimising BGA signal routing in PCB...
Comments:??
*? You can enter [0] more charecters.
*Verify code:
?
?
Webinars

Seminars

Visit Asia Webinars to learn about the latest in technology and get practical design tips.

?
?
Back to Top