So far in our studies we have examined in detail the materials brought together for an electronic assembly, and the board fabrication and assembly/test processes. However, whilst we looked in Unit 5 at the ways in which design influences manufacture, we have yet to consider the actual requirements for manufacture.
The purpose of this Unit is therefore to look in more detail at how design impacts upon manufacturability, and at the requirements of assemblers and fabricators. We are looking primarily at the issues associated with making a completed board assembly, but inevitably there is some commonality between Design for Assembly issues on the board and the similar requirements for an equipment assembly that will be discussed in Unit 9.
Good design is a combination of computer tools and common sense . . .
Common sense is the most widely distributed commodity in the world, for everyone thinks himself so well-endowed with it that those who are hardest to please in any other respect generally have no desire to possess more of it than they have.
René Descartes (1596–1650)
By the time you have completed this Unit, we hope that you will agree that most of the things that we identify are common sense, but common sense informed by knowledge of the perspectives of fabricator and assembler and of typical fabrication and assembly issues.
When we consider any of the “Design fors”, and especially Design for Fabrication, we will find there is a great deal of detailed information that we need to absorb before we can create designs that are manufacturable. As with other Units, in order to keep this main text at a reasonable length, much of the detail is presented in the form of supplementary material, which we would encourage you to read. Links to this material are found both within the main text and on the module map.
We should like to acknowledge the contributions made to this material by many colleagues in industry. Worthy of a special mention are Neil Purves of Plexus, whose DfA checklist and Good Practice Guide, written for an earlier module, continues to inform our thinking. For fabrication, we acknowledge contributions from both Circatex and Merlin Circuit Technology, who provided insights into the preliminary engineering process carried out by fabricators and the typical problems they experience. We are also grateful to DEK Printing Machines for equivalent insights into the stencil manufacturing process.
The design process ends up by transferring information to fabricator and assembler. In order to do this efficiently, we need to understand the needs of the information user, and the process carried out by the supplier in order to convert the data provided into a form appropriate for fabrication or assembly.
We also need to appreciate that, however good the information supplied by the designer, some interpretation and modification by the supplier will be required in order to ensure that what is asked for will be made. As examples: artwork may need to be adjusted to give the correct final dimensions of a track; board lay-up may need “tweaking” to give the correct impedance or stack thickness after pressing; alternative components may need to be procured in order to hit delivery deadlines.
Throughout this Unit text we will be reminding you of the differences in perspectives of designer and suppliers, and supplements will give more detail (with examples) of the front-end engineering carried out by suppliers.
In the core section of this Unit text, we will be considering four key “Design fors”, but we are starting with a review of the layout design process, which contains a reminder of some of the items that constitute the required data set.
[ back to top ]
We are using the term ‘layout design’ to refer to the stages that convert the completed electronic design into something which can be manufactured, as distinct from the work carried out by the electronic designer, whose task is to create a solution to the marketing requirement by an appropriate choice of interconnected circuit elements and software.
However, the task of converting the resulting design from breadboard (or simulation) into hardware is not just the responsibility of the layout engineer, but will require inputs from many interested parties. Typically at least the first two stages in those listed below (partitioning and technology definition) will be shared between the electronic designer and others, and these are crucially important since they have a significant influence on the final price of the product.
The first requirement is to ‘partition’ the whole circuit, deciding on the split between different board assemblies, and on what elements are going to be embedded in the silicon integrated circuits, and which incorporated on the board itself. This task would normally be done by the electronic design engineer, but with some input from manufacturing partners. Common sense (supported by some theory) suggests that the optimum result, in terms of performance and cost, is achieved by making best use of each of the layers of interconnect. For example, provided that the parts are both available and well away from state-of-the-art, using a higher level of silicon integration costs less than making a more complex printed circuit assembly. [We will return to the concept of partitioning in Unit 9 and again in our Case Studies, because of its influence on the overall cost and performance of a product.]
At the technology definition stage, the designer selects the basic rules that determine the board’s complexity. These include the type of technology to be employed (through-hole, surface-mount or mixed), the board material, the number of layers to be used, minimum track and via sizes, and minimum spacing between objects. The rules may be determined by factors other than electrical function: for example, the design parameters of any device with a keyboard are determined by the size of the human hand. However, most decisions will be centred on cost, production quantity and the expected use of the circuit. This stage has a huge effect on the difficulties of the placement and routing processes that follow.
The circuit interconnection (‘net list’) data now has to be entered into the CAD system. Increasingly this process of ‘schematic capture’ will be carried out using information about the design generated during circuit simulation. However, it is still relatively unusual to have the same level of integration of simulation and design as is used in developing custom integrated circuits. Circuit operation may not be checked before full manufacture, so the net list, which determines the electrical operation of the finished system, must be correct!
At placement, the layout designer selects the physical location of components on the board, which determines the footprints. This ‘layout’ stage uses a ‘library’ which contains dimensional and connection information on each of the components to be used. Each company will have a library of the components used, and there is often a large capital expense to set this up and keep it up-to-date. Like any computer database, superseded information can cause problems.
The net list expresses the connection between each of the physical positions defined during the placement process: ‘routing’ creates the physical net list on the board, by inserting interconnection tracks and vias. Routing is iterative and interactive, taking into account the desired width, segment length and separation of the tracks and the design rules of board manufacturer and assembler. It has been described as ‘algorithmically challenging’! A combination of manual and automatic computer routing is usual, in order to get an optimal result: the computer is an aid to, and not a substitute for, a good designer!
At this stage, the layout designer has a design, but its functionality and performance have not yet been demonstrated. More critically from the manufacturing point of view, only a limited degree of design rule checking will have been carried out.
CAD systems will usually include some circuit simulation, and may also allow the designer to carry out thermal analysis. This is based on worst case figures and enables predictions of ‘hot spots’ to be made. Whilst these are predictions, and will not always be 100% correct, they provide a useful means of highlighting potential problems before production.
Whilst the CAD computer will have been programmed to check data for consistency and conformance to design rules, providing a good monitor of the effectiveness of the design, just relying on this will not necessarily find every non-conformance to good practice. Table 1 is just one of many examples of a list of points which a good board layout designer should have considered.
|1. Is the component layout suitable for the intended assembly method?
2. Are the components regularly distributed, giving a uniform density over the complete board?
3. Can components be inspected efficiently and reworked easily in the event of failure?
4. Has consideration been given to the method of test and to providing sufficient test points?
5. Are any adjustable components easily accessible?
6. Has consideration been given to thermal effects?
|Mechanical and electrical considerations|
|7. Does the layout make good use of the panel area?
8. Has the circuit been divided into functional sub-units?
9. Has the number of different hole diameters been minimised?
10. Has adequate conductor spacing been provided?
11. Can supply line conductors withstand a short-circuit on board?
12. Have analogue and digital parts separate supply lines?
13. Are heavy components adequately fixed?
But even this kind of check does not cover every aspect of Design for Manufacturability. Assemblers in particular will want to add a more formal review of the design from the point of view of assembly and repair. It is possible (and expensive) to have to go round the loop a number of times before a fully working production board and circuit have been developed. Peter Clegg has rightly commented that one factor which increases cost is designers working in isolation!
[ back to top ]
All data packages supplied to board fabricators and assemblers are now in digital form, although there is much reworking and reformatting of older designs. As can be seen from Table 2, a range of useful data can be produced from the schematic captured by the CAD system: manufacture is considered, placement machine drive data is developed, and the data can be used to produce the test vectors for testing the product after assembly.
|PCB photo tooling (‘artwork’)||PCB layout (‘photoplot’)|
|PCB drilling data||PCB profiling information|
|board test data||PCB bill of materials|
|assembly bill of materials||stencil pattern|
|assembly drawings||component placement position/orientation|
|AOI inspection data||circuit schematic and net list for test|
The CAD system produces an enormous amount of data, sub-sets of which need to be provided to the manufacturing team. Before reading further, briefly research this topic area to discover the major standards, and perhaps uncover some of the issues, by combining suitable search terms such as "PCB fabrication" and "data transfer".
When the design has been finalised and the necessary checks have been carried out, it is necessary to produce the board manufacturing tools. ‘Photoplotting’ first appeared during the 1960s, replacing manual methods, often what was referred to as ‘cut and peel’. This used a sandwich of an opaque film on a transparent base: the top film was cut, using a controlled depth cutter, and areas were selectively peeled off the base. The desired pattern could either be left on the base as a positive image, by removing surrounding film, or as a negative image, removing areas corresponding to the desired pattern. Such patterns were normally cut at an enlarged scale of 5:1 or more, depending on size and complexity, and subsequently reduced by a precision photographic process. In contrast, photoplotting is normally carried out at final size, using a material which is dimensionally stable as regards both temperature and humidity.
Early plotters were ‘vector’ plotters that exposed the board image on paper or film using flashes of light to draw the traces individually. The geometry, shape and size of the features were controlled by placing a movable aperture between the light source and the film. The operations required data similar to that needed to operate an NC tool: separate commands to move to a specific XY co-ordinate, select an aperture and open or close the shutter.
This approach still affects the way in which data is transmitted. ‘Gerber format’ instructions for photoplotting originated in the early 1960s, when the Gerber Scientific Instrument Company began building large area drafting machines. For many years Gerber was the de facto standard of the board industry, although the situation is changing. Design information held in a CAD database is extracted by ‘post processing’ by a Gerber driver, to produce plotting information. The Gerber 274D format is a flexible data structure from which the user can tailor plot data to specific needs, within the capabilities of the plotting system.
The laser plotter, introduced in the early 1980s, uses ‘raster plotting’ rather than vector plotting: a laser source scans across the film and is turned on and off as necessary to build up the pattern line by line. Features such as ground planes and other polygon fills can now be imaged without the user having to resort to the complex outline and fill algorithms necessary for vector plotters. This led to the introduction of an ‘extended’ Gerber format (RS274X), which includes aperture code information within the data file, eliminating a frequent source of operator error. In this way Gerber format evolved from a description of machine tool motions to a description of the image itself, with its software supporting libraries of symbols and character sets, component rotation and scaling.
Although used world-wide, Gerber is not the ideal format for electrical test and AOI, as the language does not support net list data. Nor does it support the requirements of the assembler.
Machinery for numerical controlled drilling of the board is also driven directly from the data produced: this gives information on component holes, via holes and mechanical holes. CNC drills normally use the ‘Excellon 2’ file format, another example of a de facto standard from a leading supplier. Aperture list and drill bit data are contained in a separate ASCII file.
In addition to Gerber and drill files, other information needs to be exchanged with the fabricator, such as the mechanical drawings, and a net list file to represent the physical connectivity. The assembler will need a Bill of Materials (BoM) with a list of components and packages. Most drawing information will typically be transmitted as HPGL (plotter) files or the DXF format native to a number of mechanical drawing packages. For other information, PDF (Adobe Acrobat) files offer a secure way of transferring data which arrives in the form intended, although ASCII is often used for parts lists and placement data.
It would save countless hours and mistakes if CAD data could be transferred directly, rather than using the designer to generate files in the various formats required. For this reason, a number of fabricators have invested in design software, and will accept original source files. However, this still does not provide a totally transparent link, especially at the assembly end.
There have been many stumbling blocks to CAD-CAM integration, such as lack of agreement on naming conventions and tools being supplied without standard interfaces. The IPC 1997 Roadmap identified key needs as being for:
A number of ‘higher level’ solutions have been proposed, but many of these are overly complex and not fully supported by manufacturers. IPC initiatives in this area included the development of a set of specifications, for which the generic standard is IPC-2511A Generic Requirements for Implementation of Product Manufacturing Description Data and Transfer Methodology. The GenCAM format described there is intended to provide CAD-to-CAM, or CAM-to-CAM data transfer rules and parameters related to manufacturing printed boards and printed board assemblies.
GenCAM was probably too late – evidenced by there having been very little sign of activity since 2002! However, in your search you will probably have come across mentions of a data format called ODB++. Introduced by Valor, this is much more than an extension of Gerber, but a fully-fledged format which contains all the information needed to fabricate, assemble and test a design. It is linked with software which allows designs to be assessed for compatibility with the processes being run by the chosen fabricator and assembler, and highlights the inevitable areas where the design is nudging at the boundaries of capability.
[ back to top ]
Apart from the data used to generate artwork and drill files, you will have to provide your fabricator with other information:
On this last point, you will of course have taken advice about the most economic panelisation for your board, taking into account the sizes which your fabricator keeps in stock. You may also want to agree a build-up for the board, and specify controlled-impedance sections, although for this level of detail you are strongly advised to seek help from your fabricator.
How you provide this information, whether as a generic document or embedded in the information for each specific board, is something we will return to in a later section, but at this stage all we want to do is to stress the need to ensure that your design package is as complete as possible, leaving nothing to chance or the whim of the fabricator.
Unfortunately, even complete data sets can sometimes be difficult or expensive to fabricate simply because there is a poor match between the designer’s expectations and design criteria and those of the fabricator. To minimise this mismatch, you need to be aware of the fabricator’s perspective, which we have pulled together in two documents, an Introduction to Design for Fabrication, which explains the rationale for DfF and the role of the “capability statement” and introduces the work carried out by the pre-production engineer in converting the design.
The second document on Design for Fabrication issues is a more extended discussion, incorporating a number of SAQs, and covers ten areas in which the layout designer can influence the outcome.
Suggestion! Before you read these materials in detail, we suggest you start off by creating a list of the Design for Fabrication issues that you would expect to be important to the fabricator. Then, as you read and explore more, review your list, adding appropriate qualifications and information, and probably some extra entries. You will find such a check list useful when you approach the task that is part of Assignment 2.
As well as reading our materials, we recommend supplementing your studies by downloading and examining capability statements from typical fabricators. You will find considerable variation, particularly when it comes to their preferences for minimal cost. And some sites have useful DfF material and check lists.
An example of such a DfF guide that you may want to download is the Merix Design for Manufacturability of Rigid Multi-Layer Boards, which is supplemented by Volume Manufacturing Tolerances. Please visit the Merix web site for further material and any updates.
Also, for a simple reminder of the data requirements, see the Circatex Designer's Check List.
You should also remember that just applying numerical limits pedantically will not guarantee that your board is easy to make at high yield. One needs to apply common sense to the wider situation, and certainly not just rely on a screen carried out by the CAD system. The bullet points below, which are based on some of the more usual constraints and requests for good design practice made in guideline documents, have deliberately been phrased in a generic way, to encourage you to think, rather than blindly apply pre-set limits to every parameter.
And finally: “Have I provided all the information in the right format, so that the CAM team at the fabricator have a chance of doing a fast and accurate job?” Of course, had you devised and transmitted data in ODB++ format, and used the Valor tools, it would have been possible to review the design, not just from a fabrication perspective, but also in terms of the completed assembly.
With the foregoing basic premise of fabricators providing counsel of what is a reasonable design to consider building, it’s useful to go over some of the things that comprise a manufacturable design. Among these are:
Lee Ritchey, Recognizing Intelligent Design, Circuitree, 1 January 2004
[ back to top ]
Assemblers demand a wider variety of information than fabricators. In addition to supplying manufacturing data for the stencils and placement equipment, you may have to provide your assembly house with:
See this link for a general list of files that an assembler might expect.
And don’t forget procurement. Not only is it common sense to advise the supplier about any purchased parts which are unusually high cost or long lead-time, but the designer must always remember that having parts available on the right timescale is a major problem for assembly houses, especially for urgent or prototype applications. Ideally the manufacturing requirements and Bill of Materials should be made available to the procurement team early in the design process.
Providing the assembler with correct and complete manufacturing data, and ensuring that the parts are available for assembly, are necessary parts of Design for Assembly, but only part of the equation. DfA is also about “making it easier”, for which the designer needs to understand the manufacturing process options and supplier preferences. Often these are articulated in company statements of capability in the same way for fabrication, and occasionally assemblers will provide useful DfM information.
DfA is more difficult to manage than DfF because an input is required from more collaborators, and it is difficult to separate this process from the associated fabrication, test and rework/repair issues. As we will suggest in the final section of this unit, good practice is to set up a formal means of review by all parties, and use a series of checklists and score cards to identify problem areas.
As with fabrication, it is not unusual for there to be some iteration of the design, with early prototypes made primarily to check electrical performance and marketing acceptance before engaging in full scale manufacture. Particularly with assembly aspects, it is important to ensure that every ounce of information is extracted from the prototyping exercise and fed back to design, using this as an opportunity to enhance manufacturability, and not just to verify that a small number of units can be successfully “knife-and-forked” through manufacturing.
DfA is about cooperation, and about learning from one’s mistakes, but it is also about using concepts and ideas of good practice that come from others. In the remainder of this section we are providing links on issues to think about. These have been split under four headings:
We have already seen in Unit 5 that components have a significant impact on the process route, and that our process choice will also depend on our assembler’s preferences and capabilities, for both equipment and processes. But the process route is critically important in determining the cost of an assembly, so the layout engineering task may well include negotiating with designer and manufacturer in order to reach an acceptable low-cost compromise.
In this aspect of Design for Assembly it is possible to adapt some generic ideas which derived from studies of mechanical assembly. Read the attached paper on Design for Assembly analysis for a description of methods that will certainly be appropriate in Unit 9, and have some applicability even for board assembly. Notice the structured approach to the task, and the ways in which assembly costs can be estimated and minimised.
Much use is made of rule-based approaches, where general principles and checklists are applied to the analysis. However, some of the generic concepts have to be adapted to the board assembly situation. Read DfA Principles applied to board assembly for an illustration of how Syan and Swift’s strategies have been simplified, almost reducing to a three-fold approach:
This general approach of simplification commends itself as “common sense”, but it is disheartening to observe how few assemblies are as simple as they might be!
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-sided to double-sided surface-mount or surface-mount 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.
One way of improving productivity with little extra complexity is to handle more than a single assembly at a time, creating multiple assemblies on a single panel, in the same way that a fabricator will make more than a single unit from a process blank. A comparable approach, adding additional board area, is also necessary for assemblies that do not have a regular outline. For both, the designer engineer needs to establish at an early stage of design which techniques are to be used for de-panelling and this has an impact on the assembly design. More about the practicalities in our paper Panels and de-panelling.
[ back to top ]
The literature contains many suggestions for good practice, and a search of the TechNet archive will yield information and ideas about many problem components. In the documents linked below, we have tried to summarise some basic principles on key topics, which we encourage you to use as a basis for your own “cook book” of good ideas. The issues that relate to soldering practice and Design for Manufacture (especially relating to wave soldering) are the fullest in terms of technical content. Also, given the historically high level of defects associated with wave soldering, the comments on that topic are worth noting should you be involved with a wave-soldered design.
Although we have provided a great deal of information at the links, during your study of this Unit you have already seen in some detail the various processes by which boards are assembled. So we suggest that you start by reviewing the needs of each of these processes, and draw up lists of the requirements for good Design for Assembly.
Then, based on taking an overview of the whole process, see if you can identify other areas where manufacturing requirements may impact on the design.
Finally, recall that volume manufacturing uses conveyors as links between equipment, and identify any general areas in which conveyors may place constraints on the layout.
Review your lists against the comments that are contained in the rest of this document and in the links below:
It is always dangerous to write the word ‘conclusion’ on any list of issues – there will always be more. Specific points not covered so far include test, inspection and rework. So your lists will grow, particularly when you come across problems that you resolve by discussion with your supplier. Do not be afraid to ask your assembly house for assistance and comment: it is much better to deal with the problem up-front at the design stage, than it is to struggle to make a difficult design.
You will have noticed that a number of the good practice ideas in the previous sub-section relate to the design of component pads. This general issue of “footprints” is a common topic on the TechNet and SMART forums, with designers seeking advice as to the best pad pattern to adopt for any particular component. Whilst the correct answer is that the optimum footprint will depend on the context of the application, on the materials, and on the details of the assembly processes, there is a practical solution in the form of the IPC recommendations that are now embedded in IPC-7315. For each part this makes not just a single recommendation, but three, representing the largest and smallest recommended sizes as well as a typical average footprint.
Typically, each pad will be large enough to accommodate the entire termination of the component lead that will be in contact with the board and allow for the tolerance of component placement, dimensional tolerances of the component and pattern accuracy of the substrate. Purves suggests some general rules:
The IPC-7351 Land Pattern Viewer is a shareware program that allows users to view component and land pattern dimensional data in tabular form as well as graphical images that illustrate how a component is attached to the land pattern on the board. The free software can be downloaded at http://landpatterns.ipc.org/default.asp, and the updated .plb files for any of the 3 IPC-7351 land pattern libraries (Least, Nominal, Most) are at www.pcblibraries.com/resources/PFiles.asp.
Be aware however that the Microsoft .NET Framework is required to use this software. This is a free download from Microsoft.com – search for ".net framework redistributable" – but you may experience problems with this aspect, and this is not something that AMI support as it is not specifically required by this module.
The initial concept of a footprint was of a pad that surrounded the component termination, allowing the creation of a smooth solder fillet of generous proportions. However, as components have shrunk, so has the available real estate for the device pad. This is particularly noticeable when components such as 0201 capacitors are used, there being little point in paying extra for a small part and foregoing much of the advantage by designing with over-large pads. In consequence, there is a trend towards using pads of similar size to the component terminations. This forces a rethink, not only on the practicalities of solder joint inspection, but also on how to apply enough solder paste to make a satisfactory joint. So the traditional approach of insetting the stencil aperture, so as to make a seal between stencil and pad in order to avoid paste bleed under the stencil, goes out of the window – the designer and assembler have to work together to get a sufficient joint, and the solution may involve printing paste into the solder mask well around the pad, and not just on top of the pad itself.
In reviewing pad designs, you will also find many deviations from the traditional annular pads for through-hole components, and rectangular pads for surface mount parts. These may be aimed at improving yield and joint quality, at tackling specific problems such as solder beading or tombstoning, or at making it easier to inspect a joint. Whenever you come across design variants, such as the “home plate” design used for small chip devices, or the tear shape used for BGAs, seek to understand the rationale for the design, and how it works.
Whilst we considered the materials used for solder mask in Unit 1, and our discussion on soldering has indicated the important of this material, solder mask is often regarded as a necessary evil, and the promoter of problems such as solder balling. In order to view solder resist as an important element in the design, it is necessary to think of the board as being in three dimensions, rather than flat, and try and visualise the interaction between mask and stencil, the flow of solder paste, and the way in which solder wets preferentially. More about such issues in our paper Solder mask design basics.
Although not every board will contain legend or "nomenclature", having additional information printed on the board itself can be advantageous during both assembly and subsequent test diagnosis and repair. Neil Purves’ recommendations as to the information contained in this layer, and its format, can be found at Legend recommendations.
In general, an effective design is one that allows as much space as possible between the components to be assembled, as this simplifies every process. But in practice, it is frequently necessary to space components as closely as possible. How close should this be? The answer of course is that the distance to the adjacent components depends on the processes through which the product is to pass. More information in our paper Component spacing.
An assembly issue that is easy to overlook is that of handling, both during the processes themselves and between processes. So we have to provide clearance around the periphery of the board, consider height clearances above and below the board, especially on second-side assembly, and also consider how to provide board support. This last has always been important at printing (to get an adequate stencil-board seal) and at placement (to reduce vibration moving components), but is becoming increasingly important during soldering processes, especially at the higher process temperatures now used for lead-free solder formulations.
Support may require permanent tooling (as with printer nests), temporary tooling (such as support pins for printing and placement), space around the panel periphery and appropriate tooling holes for using wave soldering pallets, or component-free areas underneath the board for support wires for reflow or wave soldering. More insights into the issues at this link.
The sketch below shows a side view and plan view of a sample board assembly. Examine this from a DfA perspective and recommend appropriate design changes, explaining the reasons for any changes to the product’s designers.
More information on the DfA of mechanical assemblies can be found at “Design Engineer on a disk”
(index at http://claymore.engineer.gvsu.edu/eod/design/design-1.html;
Design for Assembly starts at http://claymore.engineer.gvsu.edu/eod/design/design-54.html)
Information on tools for mechanical DfA can be found at:
On-line DfA checklists and guidelines can be found at the web sites of some assemblers. Try a Google search for "PCB design guidelines" or visit the Durant Eaton site http://www.xs4all.nl/~tersted/PDF_files/CutlerHammer/design.pdf.
Generic design links at:
Information on tools for electronic DfA can be found at http://www.valor.com.
[ back to top ]
As we have already indicated in Design for Assembly, there are a number of specific data requirements for the test stage, most of which will have been supplied to the assembler in the manufacturing package. A typical set of requirements might be for:
Most of the issues should have been thought about and if necessary discussed with the assembly team in advance. But there is the same question as with fabrication: “Have I provided all the information in the right format, so that the assembly team have a chance of doing a fast and accurate job?”
Whilst providing all the information is as critical for DfT as anywhere else, completeness is not an end in itself, and the designer needs to take account not only the effectiveness and coverage of the tests, but also the practicalities of implementing the test routines. Comparatively small differences in design may make the product much easier to test, particularly from the point of view of making probe contact.
Before you consult our comments, reflect on your knowledge of the testing process, and identify a list of DfT best practice consideration. As in earlier sections, the checklists (or mind maps, or similar) you create will be a useful resource for your professional life, and not just for Assignment 2.
A simple DfT checklist could be something like the following:
A rather fuller list is contained at A brief list of test requirements.
Before reading our short paper Practical aspects of Design for Test, use your knowledge of the test process, as described in Unit 7, to reflect on the practicalities of providing test points, trying to identify the key physical aspects of the board layout, and the influence of the test method on the design.
When assemblers plan the assembly process, they have to include test, so a test fixture must be ordered and test software produced by the fixture manufacturer. If we take an ICT machine as an example, what will be the process after the assembler has supplied the data for the fixture manufacturer? Compare your answer with this one.
[ back to top ]
Repair and rework are two aspects of the same challenge: rework is rectification work carried out during manufacture in order to meet performance and quality criteria; repair is a set of similar processes, but carried out on a product which has been released into the field and subsequently failed.
At board level, repair and rework involve the same considerations, but repair has the additional complication that one has first to access the board to be repaired. As a designer involved in the whole of a product, you will be able to influence mechanical access consideration, but perhaps not take the final decisions. However, as the board designer, you can at least ensure that the board you design takes into account the requirements of repair and rework at the component level.
There is a practical difference between repair and rework: often those carrying out field repair have an insufficient toolkit. This is not something that we can do other than disparage, and assume for the purposes of this section that repair and rework of boards is carried out under proper factory conditions, with full antistatic precautions, trained operators and the right equipment.
The overriding requirement is that any components to be replaced should be accessible. This means that it should be possible to apply the correct implement, whether soldering iron or hot air tool, without the tool coming into physical contact with other components, and preferably with the heat focused so that damage is not done to adjacent components and their joints.
More information on access issues in the short paper on Rework considerations.
The second area to be aware of is that of thermal demand. So far in our discussion of soldering we have skated round this topic, although it is implicit in two observations we have made in other parts of this module:
The challenge of providing enough heat is made more difficult during repair and rework because our intention is only to reflow those joints which are associated with fault component, or are faulty in themselves. This means that the surrounding area acts as a heat sink. Whilst we can attempt to overcome this by applying very high temperatures, to do so risks damaging the board.
This is particularly the case for boards with relatively small pads. The combination of adhesion always being worse around the periphery (and small pads are ‘all edge’!) and reducing at high temperature, means that these pads are particularly prone to lifting, if the solder is not fully molten and any stress is applied to the component attached to the pad.
It is good practice to try and distribute the components which are thermally large for repair/rework as well as for reflow. If the parts are large, then consideration should be given to specifying the use of background heating during rework, in order to enhance the process and reduce the risk of damage.
The section on The tool-box in Repair and rework contains a list of equipment recommended for a typical mixed technology application, for use by a trained multi-skilled operator. The cost in equipment and training is, however, considerable and not always affordable, and it is common to divide up the task in terms of the skills and equipment needed.
In practice, rework should be planned by the assembler in concert with inspection and test. The decisions on which the plan is founded concern the topics below:
These decisions have to be made in the light of information on the design, the customer quality requirements, the components used, the expected defect level, and (from the test and inspection flow-chart decisions) the stage of the process sequence where the defects are brought to light. There are many potential contributors to the team that carries out such planning.
As part of the preparation for a product review, prepare a list (with explanations) of the issues that you need to take into account when specifying the methods, equipment and processes needed to repair the product down to the component level on the internal boards.
[ back to top ]
We have stressed throughout the preceding sections that the data set provided by the designer needs to be complete and accurate, and lack of completeness is a common complaint from those carrying out pre-manufacturing engineering functions, whether for board fabrication, stencil manufacturer or board assembly. Don’t forget that a missing piece of information is similar in impact to a missing component – not only will the missing element prevent completion of the task, but its absence may cause work to be halted at an earlier stage. Particularly where the validity of the whole set of information depends on the missing data, as frequently the case with board fabrication, it may be unsafe even to initiate the manufacturing process.
“Some of our customers send us no information at all and we have to guess; others send us more information than we require, with a sample they have made up themselves, and then we can see at first hand what it looks like. If it’s a brand new design, we will have CAD information, typically Gerber files of the circuit board, but we won’t know what the actual devices look like until they come in. Then we have to think about what device goes where, and which way round it should go, if this is not clear from the board. Sometimes we can spend a day phoning the customer, sorting out the finer details of orientation.
“Supplying a piece of paper with the right information is not a great deal, but customers require educating. Some of them are purely design houses, and they don’t want to understand production. They would rather take all the trouble we give phoning them up about silly questions.”
Paul Rich, Ultra Electronics, July 2005
Whilst the overall data set needs to be complete, it may not necessarily be in everyone’s interest to supply the whole of the data set to every user. The approach should be to consider what is needed by any “internal customer” and provide that, in order to simplify their task.
For any document, the writer should focus on who will be using the document and what actions or decisions the users will be making based on the document.
Cutler-Hammer PCB Design Guidelines
As well as being complete, the data set needs to be accurate. We have already commented about the advantages of using data formats that combine data from required in different stages of fabrication and assembly and thus allow proper cross-checking.
Related to this is the troublesome matter of the issue control of design data. All manufacturers seek to avoid a situation where different sets of manufacturing data co-exist in a single manufacturing area or, worse, within the documentation for a single batch. It is not unknown for issue-related problems to be experienced as a mismatch between stencil and board, or between stencil, board and Bill of Materials. Such situations may be caught during manufacture, but may also require expensive rectification. Achieving a coherent data set is the primary responsibility of the layout designer to manage, with systems colleagues in procurement and manufacturing.
Whilst data integrity in its widest sense is a common issue, achieving a manufacturable design involves a complex interaction of materials, components, processes and process sequences, with an option selected in one of these areas having an impact elsewhere.
From the designer’s perspective, a key requirement is having an understanding of the supplier’s process. This refers not only to the processes involved in the manufacture itself, but also to the procedures that are carried out by the supplier in converting data into a useable format, making allowance for predictable changes that will take place during processing.
In order to understand the process more fully, we followed the process through both with the fabricator and a stencil maker. Because of the video-intensive nature of this material, it is too big to host on this site, and will be made available on DVD.
On many occasions the engineer performing this pre-processing work needs to import information that is not necessarily on the drawing, so is delayed by the need to refer back to the designer. But in other cases the information is not readily available, with the result that an informed guess must be made.
Ideally, standard elements should be defined within a specification agreed between the companies, to avoid error. But what should be assumed, and what should be on the specification? There is an interesting discussion on this on TechNet in November 2005, which we have excerpted at this link, from which it is clear that views range very widely.
[ back to top ]
Most of the design recommendations, manufacturing process controls and quality procedures are well documented. As usual, early leads were given by the military establishment, but increasingly specifications world-wide are based around those compiled by the IPC. The most relevant standards are listed in Table 3:
|Generic Standard on Printed Board Design||IPC-2221|
|Design Guidelines for Reliable Surface Mount Technology Printed Board Assemblies||IPC-D-279|
|Generic Requirements for Surface Mount Design and Land Pattern Standard||IPC-7351|
|[supersedes Surface Mount Design and Land Pattern Standard||IPC-SM-782]|
|Process Control Guidelines for Photo-tool Generation and Use||IPC-A-311|
|Documentation Requirements for Printed Boards, Assemblies and Support Drawings||IPC-D-325|
|Information Requirements for Manufacturing Printed Board Assemblies||IPC-D-326|
|Specification for Base Materials for Rigid and Multilayer Boards||IPC-4101A|
|Guidelines and Requirements for Electrical Testing of Unpopulated Printed Boards||IPC-9252|
|Acceptability of Printed Boards||IPC-A-600|
|Acceptability of Electronic Assemblies||IPC-A-610|
|Acceptability of Electronic Wire Harnesses and Cables||IPC/WHMA-A-620|
|Generic Performance Specification for Printed Boards||IPC-6011|
|Qualification and Performance Specification for Rigid Printed Boards||IPC-6012|
|Qualification and Performance Specification for Flexible Printed Boards||IPC-6013|
|Quality Assessment of Printed Boards Used for Mounting and Interconnecting Electronic Components||IPC-TR-551|
|Requirements for Soldered Electrical and Electronic Assemblies||J-STD-001|
|Solderability Tests for Printed Boards||J-STD-003|
|Moisture/Reflow Sensitivity Classification of Plastic Surface Mount Devices||J-STD-020|
|Packaging and Handling of Moisture Sensitive Non-Hermetic Solid State Surface Mount Devices||J-STD-033|
Standards are continually being revised, and many older standards are being replaced: students are advised to consult the IPC Web site (http://www.ipc.org) for the latest status. Particularly important recent change has been to the land pattern standard which has moved from IPC-SM-782 to IPC-7351, in the process becoming more generic and supported by better software. Visit http://www.pcblibraries.com/ for “19 reasons why you should switch from the SM-782 to IPC-7351”.
[ back to top ]
Despite valiant attempts to save trees and do everything electronically, there is still a considerable amount of documentation associated with the manufacturing process in addition to the original information supplied by the designer. Some of this information flow is helpful, providing control and performance-enhancing feedback; other records form part of the legislative armoury. Looking in turn at some of the key areas:
Product identity : The product made generally needs to bear some identification, though this could be on the enclosure rather than the board. More typically, however, even if the enclosure is labeled, each board will bear a part identity, either etched in the copper or printed as part of the nomenclature. This identity may be accompanied by issue revision information, and declarations of conformance, for example showing compliance with UL flame retardancy standards.
Batch identity : So far, such identification is common to the whole production and built into the original artwork. However, it is usual for users to require batch identification, or in the case of high-reliability products, an individual unit identification. Batch coding might take the form of a date code and/or a factory code and can be applied by a variety of means, as for components. Where there is a requirement to identify each panel or each circuit, then some form of bar-coding using a label is the most usual solution. Care has to be taken to ensure that the bar code label will survive the processing steps after its application, including rework and any cleaning. Not only is it important that the label should remain legible, and the part identifiable through to the end of life, to aid servicing and eventual disassembly, but it is also important that the adhesive used should be compatible with the assembly and not cause any damage.
Batch traveller : For the purposes of yield control, corrective feedback and component traceability, it is common also to have some type of “batch traveller”, which records the materials used and the operations performed during assembly. Formerly such travellers were paper records, but these are being superseded by computer-stored data. It is not uncommon for the information recorded during manufacture to be quite extensive and linked both to receipts of components and tests on the completed product. In some factories, on-line information is available on the makeup, history and status of individual units, both in-progress and in the field.
Conformance paperwork : Also generated electronically, but likely to be produced as printed paperwork, is some type of “conformance declaration”, indicating to the end-customer that the product has met the specification, both in terms of performance and the test supplied. Such “certificates of conformity” are always part of the formal quality system and the contract between supplier and customer.
Such certificates of conformity relate to the agreed contract, rather than to generic standards. However, a second type of conformance declaration lies in conformance marking, such as the CE mark applied to many items intended for general sale. The indication here is very specific, meaning that the product complies with all applicable Community regulations, predominantly those associated with consumer safety such as the Low Voltage Directive, but including requirements under the EMC Directive.
Yet a third type of conformance declaration concerns compliance to the RoHS Directive, but this is implied rather than explicit – merely putting a product on sale after 1 July 2006 is equivalent to making a statement that the product complies with the Directive, so, for example, only contains permitted lead. The supplier can be challenged to provide evidence, within 28 days of being asked, that the product is compliant, but there is no requirement for any marking. However, many manufacturers have decided to apply an overt “lead-free” declaration by sticker or otherwise, if only to assist their service department in using appropriate materials if the product is returned for repair.
Whatever information is collected is of no assistance to the manufacturer if it remains as raw data: some analysis is needed in order to give appropriate feedback, so that any necessary corrective action can be taken. In an ideal world, feedback will also influence the monitoring process, so that only useful information is collected, avoiding unnecessary cost. This is equivalent to the idea of tailoring the inspection process to the anticipated fault spectrum that we encountered in Unit 7.
[ back to top ]
We have already shared some ideas for good practice, particularly as regards fabrication and assembly, but the idea of Design for Manufacture in its broadest sense reflects the whole organisation and culture of a company and is not just a prescriptive list of instructions.
Probably the most important factor is to embed the Design for Manufacture concept into the company’s operating systems. A key is to use a team approach, seeking to integrate the perspectives of a wide range of “problem owners”. Who might these be? And how would the team function? Think about these issues, before consulting our own suggestions.
In order to be effective, the team will not only need to communicate and share experiences, but will need to adopt an appropriate modus operandi and use effective tools. In many cases, the tool may start as a simple checklist, such as the one at this link. However, as the team becomes more expert, and the applications more complicated, some more sophisticated method may be needed. Particularly where there are different ways of approaching the problem, some analytical aid to decision-making might be helpful. An example of such a metric is the “score card” seen in this Agilent example.
The logical extension to such an approach is the type of formal analysis that we saw under DfA, probably using a custom software tool. The more complex the product, the more benefit that can potentially be gained from a formal review and analysis of the options. However, using software for this may be “over the top” for many companies, and a rules-based approach, supported by engineering commonsense, may be the most cost-effective solution.
We have three other suggestions for good practice, which may be summarised as:
The first of these bears re-emphasis, although we have already suggested that it is helpful to start a dialogue between the electronic designer and manufacturing colleagues as early as possible in the design life. As you will know from other studies, a very high proportion of the overall product cost (whether tooling, unit cost, or design cost) is irrevocably committed within a short time of the project start.
The philosophy of keeping it simple is not unique to electronics manufacture, and has to be interpreted not just in terms of avoiding complexity, but also by seeking to keep as far as possible away from the “cutting edge” of technology. Scarlett recommends striving for simplicity: “The first point to consider in the design of any multilayer board is whether the board should be a multilayer at all, or whether it should be designed as a double-sided board, possibly of greater surface area. Since the manufacture of multilayer boards always involves all the steps necessary to make double-sided boards, plus a number of other costly operations, a double-sided board will invariably be cheaper than a comparable multilayer.”
Whilst still true, this comment was made nearly 20 years ago, and his advice must be interpreted in the light of a need for higher interconnect densities. In practice, this means selecting solutions which involve the lowest possible technology which will accomplish the task, for example, being aware that there is a trade-off between the track-gap dimensions and layer count.
Above all else, avoid over-specifying your requirements: Figure 1 shows a generalised yield:difficulty graph, which points up the need, as far as possible, to keep designs well within the boundaries of standard practice.
Table 4, a yield chart for quoted for board outer1 layers some years ago, is a specific example of how yield losses escalate rapidly at or near the limits of capability – fine tracks (but, more importantly, fine gaps) cause significant yield losses:
|track (mm)||gap (mm)||yield|
Given rapid progress in technology and expertise, today’s fabricator would probably predict higher yields, but the fact remains that pushing every aspect of the design to the limit will be costly. Just because something can be done doesn’t mean that you would be justified in designing in that way.
Finally, as we have already commented in relation to prototyping, every opportunity afforded by a product iteration should be taken to improve the design from the manufacturability standpoint. However, bear in mind that all changes cost money, and further “gilding the lily”2 may cease to be cost-effective once a workmanlike design has been achieved.
[ back to top ]