Components glued on the bottom side for wave soldering have different land patterns, spacing and orientation rules. The general rule is to start with only chip caps and resistors and other two leaded components. Significant wave shadowing can occur with taller components, such as SM tantalums, particularly when they are placed near smaller, lower chip components or SOT-23s. PCB orientation can often change when the board is panellised.
If density requirements push you to wave solder other component types, then SOT-23s and SOICs can be placed on the bottom side. These components must be oriented correctly for the board to be most economically manufacturable. Land pattern design is critical, including ‘solder-thieving’ pads on the sides of all SOICs.
J-leaded devices such as PLCCs, as well as fine-pitch devices such as QFPs cannot be wave soldered on the bottom side. Some complex designs now have fine-pitch, PLCC and BGA ICs covering both sides of the board, which ensures that such PCBs will either not be wave soldered or require exclusion jigs.
Some components are not able to withstand the solder wave process, but due to space or design restrictions cannot be placed on the side that isn’t wave soldered. In this case the manufacturing engineers would design an exclusion jig that covers the relevant components but allows the other components or pins to be processed. Any jigs produced will obviously add to the process costs and these will have to be amortised to the product. Typical jigs may cost between £20 and £50 each, but, as twenty or more may be used for each batch, the total jig cost is £400–£1,000.
Soldering bottom-side SMT components with a lambda or ‘A’ type soldering wave oftentimes produces unsatisfactory soldering results. These two wave types were designed more specifically to solder traditional THT components. Therefore, in many cases these two wave types do not have the appropriate contact action to break the surface tension of the solder at the component lead/pad interface of bottom-side SMT components. If the surface tension of the solder is not broken, then the solder cannot properly wet the interface, and form a solder joint. This is sometimes called shadowing and is the primary cause of a type of defect commonly referred to as ‘skips’.
A solution is to orientate the pin banks parallel to the flow direction, so that the pins hit the wave sequentially and the plastic body does not affect each pin. When laying out the board, it is recommended to orientate all DIP and axial components along one axis. Figure 1 shows the preferred direction of component orientation when SMT components are to be wave soldered. For reasons of space these may not be possible and this increases the probability of joint defects, for example, short circuits (see Figure 2).
This will also make the board easier to inspect, and will slightly reduce the auto-insertion machine time, saving on production costs. Having even one axial component on a board oriented in a different axis, means that the axial insertion machine must rotate the board or pallet to install that component.
For components with many pins on all four sides, two of the sides will be prone to shorts, no matter which way round the component is rotated. One solution is to position these components at 45° to the flow. In situations where yield issues result from these types of components, but it has not been possible to redesign the product, tooling could be used to set the board at an angle through the wave to be removed after the wave. This obviously adds to the number of process steps.
The problem with the parallel pin banks is “which pin does the last pin snap to?” To prevent excess solder, and therefore shorting, at the last pin, ‘thieving’ or ‘robber’ pads can be added. These are pads, usually two or three times the width of the component pin but the same length, added beyond the end component pins as in Figure 2. In some cases either edge could be the leading edge of the board in wave soldering, so thieving pads would be provided at both ends.
Reflowed SMT components can be placed at any angle on the board. However, it is good design practice to keep to one or two axes, with all polarized components oriented in the same direction. This will simplify inspection and yield a more professional looking board.
Fiducials (or fiducial marks) are artwork features on the outer layers of the board. Fiducials are required if there are any components located on that side of the board. Fiducials are used by assembly equipment for location and registration of the fabrication artwork. Vision systems are required for the precise placement of solder-paste, adhesives, components, and for any other automated assembly processes. Without fiducials, automated assembly cannot easily be carried out.
When reviewing a PCB assembly, some machines in the assembly process require global fiducials for accurate board location for placement of components and optical inspection systems. The first review is to make sure there are enough global fiducials on the board for the process.
Some components also require local fiducials for more accurate placement because of their high number of pins and pin pitch. The fiducials can be beneath the component, or located near the component in two corners. The local fiducial must be within a certain distance from the component in order to be recognised by the optical recognition system.
There may be some instances where the optical recognition system will be confused or unable to find the fiducial:
Through-Hole Technology (THT) encompasses older PCB technology, including axial leaded and radial leaded components, DIPs and any connector or other component with contacts or leads which pass through a plated barrel in the board.
There are two primary types of THT component types, soldered and press-fit. Soldered contacts have a solder joint that fills the barrel and forms a joint on both sides of the board, and are still the most common type. However, press-fit is becoming more popular as High Density Interconnect becomes more prevalent, and small pitch connectors cannot be wave soldered successfully. The press-fit process is an alternative for consideration to hand soldered THT components.
A double-sided placement must restrict certain part types to certain sides of the board, since some parts will not be suitable for all types of soldering. Most ICs, SOTs, MELFs and tall parts would disallow wave soldering on that side of the board.
These are wagon wheel-shaped relief pads etched in the copper of a ground plain around a through hole. It connects to the plane through one or more narrow track across an opening in the plane, rather than connecting directly to the plane, so that heat transfer to the plane is minimised during soldering. Figure 5, Figure 6 and Figure 7 show various designs.
Multi-layered PCBs with inner power and ground planes touching plated through-holes that are also used for THT components require thermal reliefs or ties on those inner layer planes. This is because these planes of copper act as heat sinks for the component pins during the solder-wave process, and they consequently do not reach the required temperature for a good solder joint. Thermal reliefs or ties maintain electrical connectivity, but restrict the heat sinking effect.
Figure 8 and Figure 9 show how design errors can reduce the thermal relief spoke width (Figure 8) or even take out a whole spoke.
Similar placement and keep out requirements apply to THT as to SMT:
Most components are available in surface mount format, although some are still only available as THT. As designers and assemblers become more confident in the mechanical strength of SMT components (for example, connectors requiring multiple insertions) this trend will continue.
Connectors are the most widely used THT components and are still very good choices for high reliability, low cost interconnect. In cases where the only THT components used are connectors; press-fit connectors are to be preferred, as the assembly is exposed to one fewer thermal cycles. Press-fit interconnects are highly reliable and solve many of the design and process development issues associated with HDI (High Density Interconnect).
Where wave-soldered connectors are used in mixed technology assembly, special design and clearance considerations must be made in layout and design. Connectors should be oriented in the ‘preferred’ direction for the solder-wave, and thieving or robber pads should be included in the layout if possible.
Using THT components and SMT components on the same assembly is referred to as mixed technology. If design requirements and component selection dictate the use of both technologies, certain design considerations must be kept in mind.
If surface mount components are to be placed on the bottom of the board and wave soldering is needed for through-hole components, then only certain SM components can be wave-soldered.
Where bottom-side components cannot be exposed to the wave solder process (due to lead configuration, lead pitch, temperature sensitivity, package size or excessive component density), there is, fortunately, an option to use exclusion jigs or selective wave solder fixtures to solder THT components onto assemblies.
For the selective wave solder process, the assembly must be designed to accommodate the special solder fixtures needed. Some recommendations for selective wave soldering are:
The ‘Paste-In-Hole Reflow’ (PIHR) process, also called ‘intrusive reflow’, ‘pin-in-paste’, or ‘multi-spot soldering’, is a way of reflow soldering through-hole components that is particularly effective for phone jacks, Pin Grid Arrays and connectors with good lead spacing and sufficient lead clearance on the component underside. Table 1 shows how the PIHR process sequence compares with conventional assembly.
|Table 1: Conventional assembly and PIHR contrasted|
|Conventional assembly process||Pin-In-Hole Reflow|
|Application of solder paste||Application of solder paste|
|Positioning SM components||Positioning SM components|
|Reflow soldering||Positioning odd form components|
|Positioning odd form components||Reflow soldering|
|Hand soldering odd form components|
|Quality inspection||Quality inspection|
Note, however, that the PIHR approach is only effective if:
Using PIHR also has some preconditions:
Figure 10 shows a PIHR application after solder paste deposition: square solder paste pads can be seen on the board where the connector will be inserted prior to reflow.
Electrical designers may insist on tightly grouped parts in sensitive circuits. Overdoing this, however, can result in unbalanced layout that has groups of components at minimum spacing. Parts may be back-to-back on both sides of the board, while other areas are completely devoid of parts and signals. This can make signal routing difficult, and requires the fabricator to add copper to avoid warping and under- or over stretching.
The assembler will have a maximum and minimum board size dictated by the maximum and minimum adjustment ranges of the process and handling equipment. Any board design smaller than the minimum dimensions will have to be placed in a panel or array or have special tooling fixtures developed. Large panels can save material but are difficult to handle because they require de-panellising. This will involve using the fabricator routing the board and the assembler using ‘nibblers’ to de-panellise, V-scoring the panels or snapping the panels manually. Which method is chosen depends on the assembler’s capabilities and any cost implications. De-panellising would normally be done after the last process, before adding any hand-fitted components that overhang the board and interfere in a panel.
Assemblers will usually have two or three preferred panel sizes that reduce changeover downtime caused by adjusting rails, repositioning barcode readers etc. The assembler will advise on this.
A breakaway rail or frame (Figure 12) will need to be added to a single PCB or panel if it is not possible to provide a sufficient clearance of components or copper traces for the process rails and board clamps. This increases PCB cost. During PCB assembly the PCB is handled by two opposite straight edges on the PCB. The areas indicated in Figure 11 show the keep-out area on the sides of the card that are carried by the conveyor and clamped during placement.
The routing operation removes the single PCB image from the production panel. Routing is also used to create cut-outs and slots in the PCB interior. The key design consideration is providing sufficient clearance between the edge of the rout and board traces and holes.
Scoring cuts a small vee notch into the bottom and top surfaces of the board. This allows the board to be ‘snapped’ apart from other boards after assembly. This is an alternative to using breakaway rails. It provides the minimum board-to-board spacing of all these options. The assembler can provide component and trace to score edge distances that are required for their processes.
Tooling holes are used to constrain and locate PCBs during bare board testing (board fabrication) and In-Circuit Test (board assembly). Tooling holes may also be used for functional test and for various assembly stages. It is more efficient to combine these functions with any holes required for mounting the board in the enclosure assembly, because this cuts down the drill process during fabrication.
Tooling and mounting holes are points of stress, and should have extra clearance for components. It is recommended to leave these holes unplated, because the hole plating process during fabrication is hard to control. If plating is necessary, the hole tolerance will need to be increased to allow for this.
Polarized components such as electrolytic capacitors and transistors should always be oriented in the same direction. The polarity should be clearly marked in silkscreen for all components for easy inspection.
Any components placed must be considered for their height. This obviously depends on the assembly process used and the side of the assembly on which the component is placed. This issue is difficult for some designers to take into account because of the 2D nature of ECAD systems.
For components fitted by hand there will be no restrictions, but the pick and place machines will have a maximum height of component picked by the machine head. Components to be wave soldered will be restricted by the height of the component as tall components may foul on the wave solder machine.
Figure 13 and Figure 14 show some common problems seen by assemblers. As mentioned earlier aligning similar components will aid inspection. Even better are clear indications of Reference Designators for components in the right place and readable and clear polarity markings for polarised components. Generally, for ICs, Pin 1 indication is used with a number or Pin 1 ‘dot’. Silkscreen outlines of components are also useful for visual inspection. LEDs and two-pin diodes should be clearly marked with the diode symbol to indicate the cathode and anode. Polarised capacitors and oscillators should have their polarity clearly marked.
Modern, fine pitch circuits require an efficient gasket seal between the stencil and PCB so the correct amount of solder paste is deposited on the smaller pad areas. The slight raise on any silkscreen near the pads will lift the silkscreen stencil, promoting smear and consequently bridged joints.
It is common sense to keep any mounting holes or other non-electrical holes free of solder during the wave-soldering process. If possible, this is achieved by specifying unplated through-holes. If holes are plated internally, they must be masked on each board before wave soldering, which creates an additional manufacturing step. However, through-holes used for mounting, and which will already have hardware in them during wave soldering, can be plated.
Figure 15 shows a PCB assembly plan view and side view. Study this for DfA and provide recommendations for redesign to the product’s designers providing reasons for any changes. The PCB assembly in Figure 15 shows the components to be assembled both topside and bottom-side.
The emphasis of DfA for mechanical and electronic engineers varies widely. As we have seen the aim of mechanical DfA is to reduce the number of components first and then analyse each for easy assemblability. Removing one or two components from an assembly with 15 or 20 components can make a big cost saving. On the other hand, for a PCB with hundreds, if not thousands of components, it will not. What makes a greater impact is the alteration of the component types and locations to eliminate processes from the overall assembly. Each new process added – single to double sided SMT or SMT to mixed technology – adds labour and process time to the assembly. This also adds to product cost. Mechanical and electronic DfA rejoin when making recommendations for changes to the process or design for greatest assembly efficiency.
Each Design for ‘X’ method imposes its own constraints on the design of a PCB. These constraints will have to be considered as part of a larger set of constraints if the designer is to be aware of the full impact of the design decisions made and therefore arrive at any compromise between conflicting guidelines. Only when the designer has a full awareness of these guidelines are the most efficiently fabricated, assembled and tested PCBs designed.
More information on the DfA of mechanical assemblies can be found at the following sites:
Information on specific tools for mechanical DfA can be found at the following sites:
Online DfA checklists can be found at the following sites of various assemblers:
Information on specific tools for electronic DfA can be found at the following sites: