Skip to content

Exclusive Layout Tips for BGA Chips

With the rising scope of miniature electronic devices with properties such as light weight, small size, many functionalities and reasonable price, the trend of Integrated Circuits (ICs) packaging has been constantly improving. In this context the most powerful IC package in use today by many electronic devices, consumer products, military equipment and medical instruments is known as “Ball Grid Array (BGA)”. The BGA ICs are widely used in computer motherboards, mobiles phones, RAMs, memory modules and other telecommunication and military devices. This IC packages comes in variety of types in which the popular ones are fine pitch BGA or FPBGA. These FPBGAs are from the category of CSP (Chip Scale Package). The CSP package is the one which has the package area less than or equal to 1.2 times of the die and the ball pitch must not be greater than 1mm.

Applications of BGA ICs:

The BGA package ICs are extensively used devices that are preferred by designers in their layouts as they have high pin count and high component density hence it eases the layout routing topology and provides more space on PCB board for more component placement and more space for tracing. Some of the applications of BGA ICs are in Field Programmable Gate Arrays (FPGAs), Microprocessors, Microcontrollers, ADC, DAC, Signal Processing ICs, Image Processing ICs, Video Processing ICs, Memory Modules, SRAMs, laptop RAMs like DDR3, MEMS (Micro-Electro-Mechanical Systems) digital sensors like Gyroscope, accelerometer, temperature sensor and many other.

Properties of BGA Package ICs:

The scope of discussion of BGA IC based PCB layout guide cannot be completed unless we know the properties of BGA ICs. As the number of pin counts in electronic circuits is increasing due to increasing use of I/O ports in circuits like FPGA, so the implementation of BGA ICs is increasing. This is because the BGA ICs have a unique style of pin arrangement. The pin arrangement in BGA ICs are in the form of 2D grid shape. The 2D array of pin arrangement in BGA ICs make them highly suitable in applications like FPGA, DSP and others. The pins are in the form of solder balls that resides inside/underneath the BGA package unlike that of QFP package where the pins are in typical counter clock wise direction, only found on the border sides of package and resides outside the QFP package/body. The diagrammatic comparison of the LFBGA100 (Low Profile Fine Pitch Ball Grid Array) with 100 balls and LQFP100 (Low Profile Quad Flat Pack) package with 100 pins is shown below. You can see the tremendously beautiful package arrangements these two are. Both of them have their own pros and cons. We shall compare these two below.

Comparison of BGA and QFP Packages:

This is the comparison of STM32F103x8 Medium-density performance line ARM®-based 32-bit MCU with 64 or 128 KB Flash, USB, CAN, 7 timers, 2 ADCs, 9 com interfacesBGA and QFP packages.

Comparison of BGA and QFP Packages

LQFP100, 14 x 14 mm 100-pin low-profile quad flat package outline, 0.5mm pitch

LQFP100, 14 x 14 mm 100-pin low-profile quad flat package outline, 0.5mm pitch

LFBGA100 – 100-ball low-profile fine pitch ball grid array, 10 x10 mm, 0.8 mm pitch, package outline

Advantages of BGA Package:

As can be evident from the diagrams above the major advantage of BGA package is its high component pin density. The other advantages are mentioned below

  • The BGA package can range from 250 pins to more than 1000 pins per package. This results in higher pin density and so very small size miniature PCBs are possible to develop by closely placing other electronic components giving them more room on PCB and also giving more space of PCB board for routing
  • Higher performance due to smaller footprints. The BGA package can be up-to 50% smaller than its QFP counterpart and that becomes evident when pin count starts to increase above 250
  • Very suitable for high speed digital circuits, can perform very effectively in microwave frequency circuits
  • Higher electrical performance due to shorter electrical paths/trace between two pins
  • Effective thermal dissipation due to ground (GND) and power (VCC) planes, ground and power thermal rings, that are placed at the center of the package and under the die to efficiently dissipate heat out of the package by means of Thermal Interface Materials (TIMs)
  • BGAs are highly compatible to the automatic placement techniques used by assembly machines due to their self-alignment property
  • Because of the circular aperture of stencil used to place solder balls and larger pitch, the smearing and resolution problem is very less in stencil based printing process.
  • Because the BGA can align itself during solder reflow, the inexpensive surface mount equipment can greatly reduce the assembly cost of BGA thus reducing overall cost of manufacturing the BGA based electronic product.
  • The BGAs are more susceptible to mechanical/mishandling damage as compared to their QFP counterparts
  • The traces connecting the pins/balls of BGA are very short due to very fine pitch so it lowers the inductance of the signal thus improving performance and signal integrity.


  • The biggest disadvantage is the BGAs are difficult to be inspected by naked eye and hence the AOI (Automated Optical Inspection) imagers are not enough to find defects in BGA associated PCBs. Hence expensive X-Ray machines are required to closely look into the possible faults.
  • Rework on BGA ICs associated PCBs is very difficult.
  • BGA are sensitive to humidity and so dehumidification is required prior to their application
  • Another disadvantage of BGA packages is the difficult or incapable cleaningof flux that is left after pcb soldering process. Because of very high pin count, the flux is easily trapped between the pins and could cause electrical failure so cleaning issue in BGAs is also significant

Recommendations on the BGA Package Layout (Guidelines):

The commonly used BGA pitch types are 1.00mm, 0.8mm and 0.5mm. The pitch is the distance between the two consecutive pins in an IC package. There are many suggestions and recommendations that a designer can follow however it is better that the designer uses his/her experience while dealing in BGAs.

  • Non Solder Mask Defined (NSMD) Landing Pad:

It is recommended that the NSMD style landing pad be used in BGA packages. The NSMD pads are those in which the pad is not covered by solder mask. In the case of SMD (Solder Mask Defined) landing pad the pad is covered with solder mask. The following diagram better illustrates the concept

1- Non Solder Mask Defined (NSMD) Landing Pad
 the typical gradual decrease in pitch from 1.5mm to 0.3mm

The above table shows the typical gradual decrease in pitch from 1.5mm to 0.3mm. The solder ball diameter also decreases. Have a closer look in the difference between the NSMD and SMD pads details, mask openings and copper pad and trace dimensions. You will see that for 0.3mm pitch, in NSMD the copper trace can be as thin as 3mil wide and copper pad dia can be as small as 6mil as compared to 4mil and 9mil SMD counterparts respectively. Hence NSMD is preferred for BGAs over SMD landing pads.

  • Number of Layers:

The number of layers on PCBs that contains the BGA IC is recommended to be determined by a simple formula.

The number of layers on PCBs that contains the BGA IC is recommended to be determined by a simple formula

This is a very simple and handy formula for a PCB designer to determine approximately how many layers will be required for a particular BGA package to route easily. Normally the BGA package’s 60% of the ball pins are used as signals and remaining 40% are used as ground or power. These 40% ball pins are routed to the ground or power plane by means of blind, buried or through-hole vias.

Now suppose the BGA with pin/ball count of 1156 and routes per channel we decided to be 1 (how we decided will discussed below), so the number of layers will be

he BGA with pin/ball count of 1156
Number of Channels
  • Number of Channels:

Now the Channel is defined as the space between the two adjacent balls/pads of BGA that allows the trace to “escape”the body/package of BGA to another point by means of multiple layer connected through “vias” in multilayer PCB. The NSMD type landing pad allows greater space for trace to escape easily between two pads and also gives more room for via placement between two pads either diagonally or inline.

You can see in the figure that the number of landing pads are shown and the arrow sign shows the channels available for traces to escape. So we can determine from this figure that a 5×5 BGA package can have 16 escape channels. This can be written is simple formula as

(Number of Routing Channels=Number of Sides ×(√(BGA ball count)-1) )

In the above case BGA ball count are 25 and number of sides are 4 so

Number of Channels=4 ×(√25-1)

Number of Channels=16

Now in the above example the BGA ball count were 1156. So we calculated the number of channels as

Number of Channels=4 ×(√1156-1)

(Number of Channels=132)

  • Routes Per Channel:

Another important aspect is deciding about how many traces to be routed between two adjacent land pads. This we did in previous step. Usually the standard is 1 trace between two adjacent land pads however in advanced PCB fabrication setups 2 or up-to 3 traces are also routed in between two adjacent land pads. The designer will layout the tracks no problem but it finally depends upon the PCB fabrication shop capability to fabricate such minuscule traces and respective “capture vias”.

The routes per channel is determined by the minimum space required between traces/routes and the trace/route width. The minimum area for signal routing is thesmallest area that the signal must be routed through. This area is calculated by this formula

g=(BGA pitch)-d

Where g is the minimum area and d is the capture via pad diameter

The following table shows the number of routes per channel and their respective formulae

Number of TracesFormula
1g > = [2 x (space width)] + trace width
2g > = [3 x (space width)] + [2 x (trace width)]
3g > = [5 x (space width)] + [3 x (trace width)]

The above table show that by reducing the trace and space size, you can route more traces through g. Increasing the number of traces reduces the required number of PCB layers and decreases the overall cost. The below diagram shows the example of single and double trace escape routing technique

 reducing the trace and space size
  • Placement of Via Capture Pad:

The decision on how to place a capture via pad in between the two surface landing pads is dependent on three aspects.

  • Diameter of Via capture Pad
  • Stringer Length
  • Clearance between via capture pad and surface land pad

The following figure gives a brief illustration of how a capture via pad is placed in between the two landing pads. There are basically two ways of placing via capture pads

  • In line
  • Diagonally
 two ways of placing via capture pads

The basic formula is represented in the form of table below for 1.00mm, 0.8mm and 0.5mm BGA pitch technologies

BGA PitchLayoutFormula
1.00 mmIn Linea +c + d <=0.53mm
1.00 mmDiagonala +c + d <=0.94mm
0.8 mmIn Linea +c + d <=0.46mm
0.8 mmDiagonala +c + d <=0.68mm


There are numerous layout techniques a designer can implement in routing, placement and optimization of PCB layout based on BGA package ICs. However the PCB fabrication shop constraints, overall PCB manufacturing cost and end application requirements are driving factors one the basis of which a designer can use his experience in appropriate and optimum BGA based PCB layout design.