As often as not, not understanding assembly leads to problems in design.

“Mistake” and “error” possess similar meanings in dictionaries. Yet there is a subtle difference between them. A mistake means selecting an incorrect path, when during the time of selection, the correct path is unknown. In contrary, an “error” signifies the selection of an incorrect solution or an incorrect path, when during the time of selection all the data required for a correct decision are supposed to be known. For example: a spelling mistake or a gross error.

Herewith are several common mistakes in PCB design. The consequences of these errors, usually detected during fabrication and assembly, may negatively affect board quality and reliability, and increase production cost and time to market.

1. The components do not suit the production technology. Component selection is an important stage in the PCB design process. Within the selection process, characteristics examined are component functionality and suitability to design requirements, cost and availability. Yet another characteristic worth examining is the component’s suitability to the production technology. Selecting a component that’s a poor match forces use of other, nonstandard means of component soldering. This degrades the component’s soldering quality, increases work cost and prolongs production time.

Following are several examples depicting this issue:

  • A component that does not withstand the soldering temperature. When using the component to be soldered on a surface mount technology production line, verify the part withstands the typical soldering temperature. In SMT production, heat within the reflow oven can reach temperatures in excess of 230°C on average. Some components are defined as SMT, but their maximal soldering temperature, as stated in manufacturer’s data sheets, is 100°C, meaning that type of component must be assembled manually. In cases where large volumes are expected, this may significantly increase the assembly cost because, instead of automated component assembly on the regular production line, parts must be assembled by hand.
  • A component not designated for SMT soldering. Several components are defined as SMT components, but in practice are connected by copper wire using specialized machines called wire bonders. These components cannot be assembled on the conventional SMT production line. By the way, the cost of assembly is considerably higher for this type of component than that of a typical SMT part.
  • Unnecessarily selecting cutting-edge components. Components can usually be ordered in several package sizes. The smaller the package, the more complex the soldering in production, which may lead to non-optimal soldering quality. Sometimes engineers select the smaller option from among several alternatives of package sizes offered by the manufacturer: for example, a QFN with a package pitch of 0.35mm (the distance between the component’s leads), instead of a larger package with a pitch of 0.55mm or even 0.65mm. From an assembly perspective, the larger package is preferable and will lead to better soldering results in production. (The exception is if component density on the PCB is high and, as a result, utilization of smaller packages is unavoidable.)
  • Selecting a component that requires special assembly and installation equipment. There are components whose installation on the PCB requires custom equipment. This increases the PCB assembly cost and can also cause sub-optimal soldering results. Consider, for instance, an SMT connector that protrudes significantly from the edge of the PCB (FIGURE 1). Since the component’s tail is relatively long, its center of gravity is located outside the PCB; therefore, it tends to bend downward after machine placement. This bending on one side of the component, triggers a certain rising on the other side of the component thereby causing insufficient soldering between the lands and the component body. The addition of rims on the edge of the PCB will not help in this case, since the component body is higher than the PCB’s vertical zero axis. To perform optimal soldering of this component, custom equipment is necessary that will support the component body and prevent its downward bending. Use of such equipment adds expense and slows production.

Figure 1. Selecting a component that requires special assembly and installation equipment.

2. Thermal imbalance of the PCB. SMT production assembly involves heating the PCB in a reflow oven. Oven temperatures are high, ranging to about 260°C. This heat spreads over the surface of the PCB. In the event thermal imbalance exists, such that during the soldering, substantial temperature differences are generated between two points on the PCB’s surface (ΔT) (more than 7°C), the PCB will experience thermal shock during heating in the oven. The result of this thermal shock may be PCB warpage, insufficient soldering for certain components, and other defects.

This phenomenon is greatly affected by component location on the PCB. Parts on the PCB are heterogeneous and may include small passives (resistors, capacitors, inductors) whose heat signature is low, together with large actives (BGAs, LGAs) whose heat signature is high. The concentration, on one hand, of components whose heat signature is high in a certain area of the PCB, and on the other hand, the concentration of components whose heat signature is low in another area of the PCB, may cause significant temperature differences between those two areas and instigate thermal shock.

Therefore, during PCB design, it is very important to ensure thermal balance is maintained on the PCB. One recommended method to prevent thermal shock is to uniformly distribute components whose soldering temperature is high across the PCB surface, rather than place them all in a certain single area.

Another way to maintain thermal balance is to ensure the PCB layer stack-up is symmetrical, that is, ensuring the copper and ground layers are evenly divided from the center of the PCB toward the top and bottom layers of the board (FIGURE 2).

Figure 2. PCB layer stack-up design.

3. Incompatibility between fabrication and assembly technologies. The PCB production cycle includes two main stages: fabrication of the PCB and assembly of components on the PCB. Variations in these processes are ripe for incompatibilities. This can occur, for instance, when raw materials for fabrication are optimized for SnPb technology, yet the PCB is assembled using Pb-free technology. SnPb technology assembly is characterized by relatively low temperatures: for instance, raw material possessing a 130Tg. (Tg is glass transition temperature, or the temperature at which the raw material traverses from a solid-rigid state to a flexible-elastic state.) Pb-free assembly is characterized by high soldering temperatures, about 40°C higher than that of SnPb assembly. When a PCB whose raw materials are suited to low assembly temperatures is assembled using higher-temperature Pb-free technology, the PCB will warp during reflow. In this case, it would have been appropriate to define for fabrication raw materials with a higher Tg, such as 170, to ensure the PCB withstands the high temperatures of Pb-free assembly.

4. Component placement at PCB edges. The PCB traverses stations on the assembly line on a conveyor belt. This conveyor belt, which is located along (almost) the entire production line, is composed of two parallel tracks. These tracks comprise a small depression that enables the PCB’s stability on the conveyor belt. The projection of the depression’s area on the PCB is unreachable by the placement machine head. Therefore, no components should be placed in that area. Placing components at the edge of a PCB (< 5mm) may make it difficult or even prevent the machine’s head from placing these components accurately on the PCB. In light of this, it is necessary to verify a “sterile” component-free area is defined at a distance of 5mm from the PCB edge. In exceptional cases, it will be possible to define even smaller distances, but solely upon coordination with the assembler.

In the event the PCB is very dense and the entire board area must be used for components, it is possible to take advantage of the margins used as a support basis for the PCB during production assembly. In this manner, it will be possible to place components even closer to the edge, up to a distance of 1 to 1.5mm. In this case, margins are added to the PCB, wide enough to constitute the PCB’s point of application on the tracks of the assembly machine. These margins are removed after assembly to resume the PCB’s “generic” size (FIGURE 3).

Figure 3. Placing components at the edge of a PCB may make machine placement difficult.

5. Placing fiducials on the PCB’s edge. Fiducials on the PCB are used as datum points that assist the machine head in pinpointing the precise location to place components. Correct locations and definitions of these markers during design have significant implications for assembly quality. Based on these markers, SMT machines carry out their precise actions, such as solder paste application, component placement, AOI, x-ray inspection and more. Since the machine’s visual field at the edge of the PCB is limited, locating fiducials on PCB edges may prevent the placement machine from identifying them. If the machine head cannot locate the fiducial points, component placement may be impossible. Therefore, it is important to meticulously define these important fiducials at a distance larger than 7mm from the edge of the PCB during design.

Additionally, release of solder mask must be allowed to prevent concealment of fiducials and enable rapid, clear and precise identification of the fiducials. In the same context, it is recommended to place three fiducial points asymmetrically on the PCB surface to permit the automated machine to identify the PCB has entered the conveyor belt in the correct direction. Placing four fiducial markers symmetrically on the PCB surface may cause a situation where a reversed insertion is perceived by the machine as a normal correct insertion and will trigger incorrect placement of the components. Likewise, for automatic stencil printers, place fiducial markers on the solder paste and solder mask files.

Moreover, to certify the fiducial is clear and easily identifiable during x-ray inspection, a component-free area (larger than 1mm) must be maintained beside the fiducials along the entire width of the PCB, that is, from the other side of the PCB as well. This is imperative since the x-ray beam penetrates the entire width of the PCB, and therefore images its other side as well. Placing the components next (<1mm) to the fiducials on the other side of the PCB will not permit identification of the fiducials by the x-ray machine, hence making inspection much harder.

This article lists several common mistakes in PCB planning and design. These mistakes stem mostly from a lack of knowledge of the engineer or PCB designer. It is recommended that those involved in planning and design of the PCB be well-versed in production and assembly technologies. It is also advisable for the PCB designer and assembler to consult while the product is in the design stage to ensure the PCB’s suitability and compatibility with these processes. Synergy between planning and design and production will help ensure mistakes do not occur.

Arbel Nissan is chief marketing and business development officer at Nistec Design (nistec.com); This email address is being protected from spambots. You need JavaScript enabled to view it..

Submit to FacebookSubmit to Google PlusSubmit to TwitterSubmit to LinkedInPrint Article