A Helpline customer recently requested Design for Manufacturability review of a design for a Printed Circuit Board assembly planned for harsh environment, high temperature use. The response of the EMPF included the requested DFM and prototype assembly fabrication, but also re-balling of a BGA (Ball Grid Array) at the EMPF factory.

The EMPF Helpline and demonstration factory have combined resources to provide solutions for insertion of electronics assemblies into high reliability applications. Recently a Helpline customer requested the development and documentation of a robust manufacturing process for a high-reliability PCB (Printed Circuit Board) assembly. In addition to process development using the demonstration factory equipment, and subsequent documentation, a DFM (Design For Manufacturability) review of the assembly was conducted at the EMPF, noting any issues of concern affecting the producibility of the assembly.

A test vehicle representative of the prototype product was provided by the customer. The PWB was high-temperature Rogers substrate material with 12 layers that included blind and buried vias. The goal of the project was to solder both ceramic and metallized ball grid array packages simultaneously to this substrate at high yield and good reliability of the final assembly.

The project addressed 10 different processes used to manufacture and test the circuit assemblies. The three following processes are addressed in this article:

PWB (Printed Wiring Board) Fabrication
PWA (Printed Wiring Assembly) Manufacturing
BGA (Ball Grid Array) Re-balling Processes

High Reliability, Low Cost PWB Fabrication
ACI reviewed the design provided by the customer for applicability in high reliability applications. The ACI engineering and design staff compared the bare PWB design to IPC guidelines for printed wiring board design. Many of these design rules can be found in the IPC 2220 series of documents. Several suggestions were provided for improving manufacturability and reliability.

ACI insisted that the PWB line spacing should not reduce the manufacturability of the PWB substrate. As a rule for most economical PWB fabrication at the average fabrication facility, 0.005" traces with 0.005" spacing are the desired minimum, usually available for no premium over wider line boards in bare board price. PWB lines and spaces down to 0.0015" are available usually at a premium price. The line spacing to adjacent copper features should not be less than 0.005" in order to guarantee suitable insulation resistance between conductors and other features. Long parallel traces are difficult to produce and subject to crosstalk, and should be avoided for enhanced producibility of the base substrate board.

ACI also made suggestions about the copper used for internal and external traces. Copper weight and density should be balanced on all layers (assuming ½ ounce copper cladding of the starting laminate) to avoid excessive warp and twist of the finished multilayer board after lamination. Heavier copper, usually used for higher current carrying capacity, reduces etch accuracy, because copper etching is isotropic, thus narrowing the imaged lines as it etches through the thickness of the foil cladding. Also, copper planes should not be exposed on PWB edges when routed from the substrate.

For high reliability surface mount electronic assemblies, land patterns must conform to IPC-SM-782 design rules for IPC class 3 solder fillets. BGA land patterns should be equal in size.

For the wave soldered PTH components, general requirements for Plated Through Holes (PTH) and annular rings must conform to IPC-2221 and IPC-2222 for class 3 assemblies.

PCB Assembly Manufacturability
To properly assess the manufacturability of the test board design, ACI performed a small R&D build of the prototype design. The build was designed to gather as much information regarding the manufacturability as possible. A small set of test boards were printed, placed, reflowed, inspected, and reworked using automated equipment. Notes were obtained about every aspect of the assembly process. A number of recommendations were produced as a result.

Since test is an important part of manufacturing, the customer was advised to consider in-circuit test - design in nodes and test points for access where possible. Silk screen part outlines, polarity, pin 1 indicators and reference designators where possible to improve test, inspection and repair of the assembly.

To properly design for reflow - be sure that heavy components are on the primary side of the board so they will not drop off when the secondary side is wave or reflow soldered. Remove vias from under BGA components that are to be underfilled so that the underfill material will not run down the vias. Location and size of tooling holes should be appropriate for the equipment requirements.

Fiducial marks should be placed so they are not obscured by equipment rails (a minimum of 0.100" from edges is adequate in most cases). Add local fiducial marks to BGA components to improve placement accuracy.

Soldermask defined lands for BGA components that are to be underfilled are recommended, to keep the underfill from encapsulating the pad edges. Allowance of a 0.100" keep-out distance around BGA's for rework and underfilling is an additional aid to manufacturability.
All components should be placed away from board edges a minimum of 0.050" for handling requirements. Land patterns must be isolated from adjacent features and lines by solder mask over bare copper - exposed copper should be no closer than 0.050" to the features to be soldered to prevent inadvertent shorting.

If possible, all active components should be placed on the same side of the assembly - avoid placing BGA components directly behind each other on opposite sides of the assembly

BGA Component Re-Balling Process Development
This process was developed by the EMPF using the customer supplied ceramic components. Fixturing occurs by applying a 4 mil deposit of solder paste to the ceramic component prior to application of the high temperature balls. Once the high temperature balls are affixed to the component via solder paste, the component is then subjected to the reflow process, melting the solder paste and forming a permanent attachment of the balls to the component.

Process Steps for Re-Balling BGA Components
The BGA components for the assembly were supplied having incorrect solder alloy ball contacts. It was therefore necessary to re-ball these BGA components with the proper alloy solder balls before assembly onto the PWB substrate.

First, water soluble solder paste was applied to the component substrate using the designated "paste on part" fixture (See Figure 3-1).

With the component still on the fixture, the fixture and component were installed onto the Metcal 550 rework station. Then, using the vacuum pickup nozzle of the rework station, the pasted component was slowly separated from the fixture. The solder preform with the correct alloy was inserted into the reballing frame and the frame was accurately positioned on the rework station platform under the pasted component.

The component and solder preform were then reflowed together using the specified reflow profile. Upon completion of the reflow process, the paper backing was removed from the reflowed component and visually inspected for missing balls. Finally, the component was cleaned using DI water. The EMPF recommended that components be baked at 125º C for 24 hours prior to use.

Using the customer supplied PWB substrates and components, the EMPF was able to establish and implement these assembly processes for BGA reballing, PWB design, and PWB assembly in the EMPF demonstration factory. A thorough DFM (Design for Manufacurability) review was performed on the assembly, the printed wiring board, and the BGA component designs. Principles of pad design and component placement for high reliability in harsh environments were applied during the DFM review. This resulted in the recommendations to the customer on optimal manufacturing of the assembly using high temperature materials in its intended introduction into a high-stress, high reliability application.

By following these basic DFM principles and instituting the reballing procedure developed at the EMPF, the customer was able to achieve a higher yield and a higher volume manufacturing of this PCB assembly.

For more information, or to learn more about applying DFM principles to your product line, please contact the EMPF helpline at (610) 362-1320, or email us at helpline@empf.org