PCB Design, Fabrication and Use from the Mil-Aero End-User Perspective
How do leading military and aerospace electronics end-users define their high-reliability printed circuit board requirements? How do they specify their materials? What factors determine their design rules? How do they deal with impedance control? What are their preferred solderable finishes? How do they qualify a new design? And when PCBs are delivered, what are their incoming inspection and quality standards, and how are the boards tested? How are PCBs handled and what precautions are taken to control moisture absorption?
The answers to these and many more questions were provided by a webinar organised by the European chapter of SMTA, moderated by Bob Willis and presented by two industry experts with whom I had the privilege of working for many years on the SMART Group technical committee and latterly as members of the SMTA Europe technical committee: Charles Cawthorne, industrial electronics technologist with MBDA Systems, and Ian Fox, electronics materials and process specialist with Rolls Royce. Their input exemplified the standards and practices adopted by a manufacturer of missile systems and a manufacturer of aero-engine controls and characterised the typical requirements of the hi-rel mil-aero sector.
The first part of the webinar was delivered by Charles Cawthorne, who reviewed the basic fabrication steps for a sequential-build 10-layer PCB as an introduction to a discussion of laminates, prepregs, copper foils and flex-rigid materials, and various aspects of design including via protection and controlled impedance.
The defining specification for base materials for rigid and multilayer printed circuit boards was IPC-4101, with its associated slash sheets defining resin and reinforcement systems, testing parameters and properties. Cawthorne quoted examples of FR-4 materials that demonstrated different glass transition temperatures (Tg), the baseline being IPC-4101/21 with a 110°C minimum Tg. In fact, MBDA specified IPC-4101/126, with a 170°C minimum Tg. But was it sufficient simply to define a Tg? Cawthorne stressed the importance of considering Z-axis coefficient of thermal expansion (CTE), especially above Tg, and explained that MBDA required a Z-axis TCE of less than 60ppm/°C below Tg and less than 300ppm/°C above Tg. Additionally, MBDA required a decomposition temperature (Td) no less than 325°C and a time to delamination at 260°C (T260) of no less than 30 minutes.
For operating temperature above about 130°C, polyimide materials were preferred, example grades being IPC-4101/40, with Tg of 200°C minimum, and IPC-4101/41 with Tg of 250°C minimum, but these materials were significantly more expensive than FR-4.
The defining standard for copper foils was IPC-4562. Cawthorne explained the meaning of the full specification sheet designation, taking as example a typical foil used by MBDA for outer layers: IPC-4562A/3 CuE3HSXS3, where /3 was the IPC-4562 Spec Sheet Number, Cu denoted copper, E indicated electrodeposited, 3 signified high temperature elongation, H indicated half-ounce thickness, S stood for single-sided bond enhancement, XS indicating that this was standard profile, and the final 3 referred to highest quality.
For the additional materials required for flex-rigid multilayer constructions, no flow prepreg was defined by IPC-4101/40, 41 or 42, flex cores by IPC-4204, and coverlays and bond-plies by IPC-4203. MBDA typically used polyimide-based adhesiveless flex cores in accordance with IPC-4204/11.
Cawthorne moved on to a discussion of surface mount design rules, beginning with component footprints for which the defining standard was IPC-7351. This considered three density levels, where Level A represented the largest footprint and Level C the smallest. MBDA used a software-based footprint calculator to optimise design for manufacture, and generally chose to work at Density Level B to give the best compromise between ease of manufacture and minimum footprint area.
The defining standards for PCB layout were the generic IPC-2221 and the sectional standards IPC-2222, IPC-2223 and IPC-2226. There had been lengthy discussion on the relative merits of solder-mask-defined or non-solder-mask-defined BGA pads, and MBDA considered the latter a more reliable option. Concerning offset vias, their preference was to ensure that solder resist was present between BGA pad and via to prevent wicking of solder away from the joint.
The defining standard for PTH footprints was IPC-7251, which covered three density levels, Level A being for the largest hole diameter and Level C the smallest. Historically, MBDA had used Level B or Level C for tin-lead but experience had shown that the PTH diameter needed to be increased for lead-free and Level A had now been adopted for both tin-lead and lead-free soldering. Standard maximum aspect ratio for plated-through holes was 6:1 for rigid boards and 5:1 for flex-rigid. For buried vias, minimum aspect ratios were 7:1 for rigid boards and 6:1 for flex-rigid, with minimum diameter 0.25 mm depending on current handling requirements.
On the question of whether to retain non-functional pads, it was MBDA’s practice to retain them. And thermal relief pads were used on copper planes with the objective of reducing heat-sinking effects.
MBDA had special clearance rules for selective soldering, with local spot masking an alternative if these clearances could not be maintained.
On the subject of microvia design, the defining standard was IPC-2221. MBDA’s maximum aspect ratio was 1:1, with minimum drill diameter 0.13 mm and pad diameter 0.35 mm. Staggered microvias were preferred; stacked microvias were only permitted in special circumstances. Copper filling was mandatory for surface microvias used for via-in-pad designs.
Cawthorne talked in detail about the benefits of via protection, with reference to IPC-4761 regarding the covering or filling of via holes with organic material, and described the characteristics of tenting, partial plugging and complete plugging methods. With all of these, coplanarity remained an issue, and planarisation was necessary as an aid to assembly. MBDA’s approach was to plug and copper-cap all plated-through vias, although it was preferred to use microvias for outer-layer conductors.
On controlled impedance, the defining standard was IPC-2221 Section 6.4, and although IPC-2221 gave equations for impedance calculation, MBDA worked closely with their PCB fabricators who had access to advanced simulation tools, to determine the effects of material properties and pressed dielectric thicknesses and adjust dimensions accordingly.
Ian Fox commented on the close parallel between the requirements of Rolls Royce and MBDA with regard to material specifications and design-rule conventions, and particularly concurred on the benefits of carefully selecting PCB fabricators and building close working relationships with them, as he introduced Part 2 of the webinar programme and reviewed the attributes of a range of surface finishes, going on to discuss testing and qualification of printed circuit boards and incoming inspection procedures.
Electroplated and fused tin-lead was the traditional PCB finish of the military and space communities and remained the preferred finish of the European Space Agency. As Fox said, “Nothing solders like solder!” Hot air solder leveling was still used as a method of selectively applying tin-lead and lead-free solder finishes, but there were issues with non-uniformity of thickness and non-flat surface profiles that made it unsuitable for fine-pitch surface mount assembly.
Electroless nickel immersion gold (ENIG) was probably the most common surface finish in current use. The defining standard was IPC-4552, which specified a nickel thickness of 3-6 microns and a minimum gold thickness of 0.05 micron. No maximum thickness was stated but a typical process maximum was 0.15 micron.
Fox pointed out that the electroless nickel deposit was not pure metal but contained between 8─11% phosphorus as a by-product of sodium hypophosphite used as a reducing agent in the chemical formulation. The copper surface required to be sensitised, typically with palladium, to initiate the nickel-phosphorus deposition. The thin layer of gold prevented oxidation of the nickel surface and rendered it solderable.
Immersion gold was deposited by a galvanic displacement process which effectively involved a controlled corrosion of the nickel surface and tended to be self-limiting in thickness. The immersion gold chemistry was highly acidic and if the process was not properly controlled could cause a hyper-corrosion effect resulting in “black pad” defects.
ENIG offered the advantages of a flat solderable surface to aid fine-pitch surface-mount assembly and could be aluminium wire-bonded. Additionally, electroless nickel had been observed to increase the fatigue life of plated holes.
Electroless nickel electroless palladium immersion gold (ENEPIG), as defined by IPC-4556, offered improvements over ENIG. A layer of approximately 0.5 micron of palladium between the nickel and the gold eliminated black pad effects and rendered the finish wire-bondable with gold or aluminum.
Of the other finishes available, immersion silver—effectively an organo-metallic coating deposited directly on copper—had been associated with creep corrosion and silver migration under certain conditions; immersion tin was good for press-fit but had limited shelf life and was not suitable for multiple reflow operations; neither were the organic solderability protective finishes. So these alternative finishes tended not to be preferred options in hi-rel mil-aero applications.
Moving on from finishes to the final stages of the bare-board fabrication process, Fox described how each PCB was validated before delivery by non-functional electrical test in accordance with IPC-9252, to verify continuity, isolation and track resistance, using a test program generated by the fabricator using a net list derived from the supplied digital manufacturing data.
Rolls Royce specified a minimum test voltage of 40 volts, although 250 volts was preferred, and if testing was carried out below 250V then it was necessary to carry out an additional 250V “proof of design” test. They required a minimum of 10 megaohms isolation between unconnected circuit elements, and a maximum trace resistance of 5 ohms, except in the case of unusually long nets, where trace resistance should not be greater than 0.5 ohms per 25 mm. Adjacency settings for flying probe test equipment were specified as 1 mm on internal features and 2 mm on externals. And if heat sinks were fitted, a minimum insulation resistance of 10 megaohms at 500 volts to unconnected circuitry was required.
How did Rolls Royce qualify a PCB design in terms of structure and fabrication, assembly and reliability, and how and at what stage was the design sealed? These were the areas Fox focused on next.
Baseline structure, material and dielectric separation requirements and layer allocations were detailed in a fundamental design document. Structure and material requirements were discussed with the fabricator as early as possible in the design cycle, and it was acknowledged that the fabricator would likely have a preferred set of materials whose lamination characteristics were well understood and would meet Rolls Royce requirements. Once the PCB build had been agreed, an update design document would be prepared, and this would be a “living” document, constantly updated to reflect changes.
As part of the qualification procedure, Rolls Royce would initially visually assess external features and quality in accordance with the basic requirements of IPC-A-600, then microsection, primarily to assess the build, core thicknesses, dielectric separations and copper weights of internal layers, drill quality and copper thickness of plated-through vias, but also include an assessment of key features such as blind and buried vias. And finally, to cross-check to ensure that their measurements agreed with the lab report supplied by the fabricator.
The integrity and structural robustness of the fabrication would subsequently be assessed by solder float testing in accordance with IPC-TM-650, 2.6.8E, Condition A, ensuring that the test piece contained key structural features, through-holes, blind and buried vias, followed by further microsection examination. Where appropriate, multiple solder float tests would be carried out to observe at what point the structure began to break down.
A number of complete PCBs would then be subject to assembly simulation and reliability testing by multiple reflow operations using a representative oven profile, followed by extended thermal cycling, visually assessed for evidence of bow and twist, and again microsectioned to examine key features. A typical accelerated thermal cycling regime used at Rolls Royce was three cycles per hour between -55°C and +125°C. Successful completion of this testing would assure that the design was robust.
In parallel with bare-board reliability testing a fully assembled board would be produced by the standard production route with an appropriate solder reflow, followed by functional testing and Rolls Royce’s standard screening procedure. Successful electrical validation after reflow followed by completion of the screening tests, would validate the printed circuit design and build and allow the design to be sealed, and the design document updated to include all materials, measurements and test results. Should an alternative fabricator be required at some point in the future, this approach would enable the design to be moved with a high degree of confidence that its performance would be unaffected.
Having described the details of the qualification procedure, Fox discussed Rolls Royce’s incoming inspection and quality standards for production PCBs. Samples from a delivered batch were visually inspected at 4X magnification and examined for significant defects such as scratches that could result in open circuit tracks, etch defects that could result in opens or shorts, flaking or crazed solder mask and stained or discoloured solder pads that could affect solderability.
If microsections were supplied with the delivered batch of PCBs, they would be examined, and measurements and comments compared with the submitted laboratory report, paying attention to drilled hole quality and plated copper thickness. Also, innerlayer copper foil thicknesses and electroless nickel thickness where checked if the finish was ENIG or ENEPIG.
Rolls Royce used IPC reference standards as follows: IPC-6011 Generic Performance Specification for Printed Boards; IPC-6012 Qualification and Performance Specification for Rigid Printed Boards; IPC-6013 Qualification and Performance Specification for Flexible Printed Boards; IPC-6016 Qualification and Performance Specification for High-Density Interconnect (HDI) Layers or Boards; and IPC-A-600 Acceptability of Printed Boards. Boards were classified according to end use: Class 1 – general electronic components; Class 2 – dedicated service electronics products; Class 3 – high reliability electronic products; and Class 3/A – supplementary requirements to Class 3 for space and military avionics electronic products. Inspection and quality requirements for each class of PCB were detailed in the individual IPC specifications.
Fox went on to discuss Rolls Royce’s handling and storage procedures for PCBs upon receipt. All boards delivered were required to be securely packaged to prevent mechanical damage in transit, with packaging suitable for use in an ESD protected area. Dissipative packaging was acceptable, but full moisture-barrier ESD bags were preferred, and if multiple PCBs were contained within a single bag they required to be individually wrapped in sulphur-free paper. Once removed from their packaging all PCBs required to be handled wearing either ESD-safe gloves or finger cots, unless they had been transferred into assembly pallets. Any boards incorrectly handled were required be washed, dried and re-baked prior to use.
PCBs delivered in dissipative packaging were immediately transferred to low-humidity storage cabinets and stored until required, although boards delivered in full moisture bags could be stored in normal-humidity environments for up to 14 days prior to being used. If the 14-day period was exceeded, the boards were required to be baked prior to use, at 120°C for a minimum of four and a maximum of eight hours.
Fox commented that PCBs fabricated in FR-4 material and soldered using a tin-lead profile were extremely robust and that delamination during soldering was rare for assemblies stored in normal-humidity conditions for up to seven days, although this might not be true for lead-free soldering. Polyimide-based rigid, flexible and flex-rigid PCBs were not as robust, and assemblies stored under normal humidity conditions for more than 24 hours required to be re-baked prior to soldering.
In general terms, the procedures described for Rolls Royce were directly comparable with those described for MBDA, and the presenters were unanimous in re-emphasising the importance of working closely with their chosen PCB fabricators at all levels and all stages of design, qualification and production of their circuit boards.
From a personal point of view, it was a great privilege to listen to two leading expert PCB technologists from the military and aerospace industry sectors sharing their experiences and describing the procedures and precautions taken by their respective companies to ensure the quality and reliability of PCBs supplied to them by their approved suppliers. Many thanks are due to Charles Cawthorne and Ian Fox for generously providing the knowledge, to Bob Willis for his professional and seamless management of the webinar, and to the European chapter of SMTA for delivering another interesting and informative learning experience.