In subsequent units, we will be looking at “how to design a good quality, cost-effective PCB” from the perspectives of assembly and test; in this unit, we are concentrating on the preliminary stage of board fabrication, focusing on what you need to bear in mind when wanting to achieve minimum costs, the best yield, and on-time delivery of the right product.
Which of these aims is most important will depend on your application, but on-time delivery is often a significant factor. In the experience of one major manufacturer, 80–90% of jobs go on hold for one reason or another during the tooling process. Of those, typically 10–30% are held for technical issues, but the balance are delayed simply because information is missing.
Good DfF will provide all the information needed for a smooth-running process that comprises reading in the CAM information and converting it into tooling, providing the detailed Bill of Materials, panellising, tools, routing and specification.
The time this process takes is totally dependent on the job complexity, the quality of the supplied package and the fabricator’s size and attitude to DfF and customer reporting. Volume fabricators with big runs will “tool the package to death”, looking for the all-important small savings; some small fabricators may perform minimum DfF checks and rectify errors and bugs during manufacture (or argue who was wrong after the boards have been delivered); other medium-scale fabricators will fall in-between these extremes. A front-end engineer at a small fabricator may be under pressure to turn round six or seven new designs in a day; in somewhat larger companies that figure may be two or three standard designs or one complex requirement. However, whether the fabricator is small or large, this should be a fast process, taking no more than a day.
Given that the most common delivery requested is for a 5-day turnaround, extending the tooling process beyond the first day because of data shortfalls inevitably causes shipment delay. This is particularly the case with companies working a shift pattern, where direct communication is difficult, and one can easily “lose days”.
If you can learn what the fabricator needs, think of all the issues which may be raised, and provide all the information required in the first instance, you can get the advantage of on-time delivery.
DfF is also about minimising cost. Some fabricators input data to their CAM system before a quotation is finalised, in order to generate an accurate cost estimate, so it can now be very true that “you will pay for what you design”. With improvements in integration of CAD and CAM systems, this is probably the way of the future 1.
1 Pete Starkey reported on a live demonstration in 2001 that “Starting at the buyer’s desk, Frontline’s E-quote package automatically constructed an email and attached the chosen data files defining the job for quotation. The sales office operator received the email and loaded it into E-quote, which automatically segregated the product data files, identified the file types and listed them all in logical sequence ready for submission to the product analysis engine. This processed the job in background and notified the operator when it had completed its analysis, at which time the operator had the opportunity to interact and make choices on, for example, finishes, before launching the costing engine. The rules-based costing engine delivered back to the operator a full cost assessment, together with a pre-formatted quote which was emailed to the buyer. Start-to-finish, the whole E-quote cycle was independently timed at a little over seven minutes!”
Smaller fabricators, where pricing to the nearest penny is not an issue and quality, batch yield and on-time delivery are the critical issues to ensure repeat business, are more likely to quote based on a square footage price with adders for extra operations and quick delivery timescales. But don’t forget that such board manufacturers will have a very shrewd idea of the potential for problems after only a short appraisal of a layout, and will price accordingly.
It is always difficult to give up-to-date accurate information relating specification requirements to cost, but you will certainly pay very substantially if you do not allow plenty of margin. As an example, 0.25 mm diameter holes may be well within the capability of your supplier, but you will get a cheaper result by using 0.6 mm diameter drills, based on the fabricator’s ability to use a higher stack during the drilling process. In the remainder of this unit there will be many more examples of the beneficial effects of good practice.
Poor design also impacts on yield, and this has a direct effect on the price. More seriously, there is a hidden cost of reduced quality. For example, with the necking of tracks, or with too small an annular ring, adding ‘teardrops’ to the annular ring can improve the inherent reliability of the design.
Some fabricators will make adjustments to the layout, but most don’t have time to fiddle around ‘improving’ the design. As well as there being a time constraint, one strongly-held view is that the pre-production engineer should only incorporate scaling factors and etch factors to compensate for dimensional changes in manufacture, and should make no modifications at all inside the board profile. In particular, fabricators with experience of expensive consequential-loss claims may insist that any other modification, however trivial, is signed-off by the design authority before proceeding with manufacture, which will introduce delay. It is your responsibility as designer to get the job right, and to take the trouble to ensure that you clean up your own design, rather than dump it on the manufacturing engineer.
The figure below shows the process route through which we shall be travelling as we consider aspects of how to design for fabrication.
A key to understanding how the fabricator works is the manufacturer’s ‘Capability Statement’, which is usually on their website, and always available on request. Whilst this obviously will have some elements of a selling document, it should also give a clear indication of what a fabricator can make.
Most capability statements have several columns, representing a scale from preferred practice to the limits of what is possible. You are recommended always to “design to the left”, that is, to choose from the column that requires no technical review.
One example of the genre, which has three columns headed ‘standard’, ‘special, and ‘leading edge’ is available at this link.
Key to the capability statement is to keep your information up to date, as this can change on a weekly basis. With this kind of document, issue control is important, and there is great danger in keeping pieces of paper which aren’t current – better to refer to the live version each time, than to work with prints which may be substantially out of date.
Note that it is not uncommon for fabricator preferences to change with the introduction of different processes and equipment, and you will get a cheaper result by giving the fabricator flexibility and as much margin as possible.
Before you read further, download capability statements from two/three representative fabricators. What information do they contain in common. Are there any significant differences between them?
Review your answer as you continue to read this unit.
A designer needs to understand the method of manufacture, and unfortunately it is not possible to create a design which is optimal for all fabricators. Some DfF guidance is generic, but there will be other issues which are fabricator-specific, the major item of which is the choice of panel size. As we will see in the next part of this unit, this is a major issue affecting cost, and not all suppliers use/prefer the same size panels.
If you plan to buy from a number of manufacturers, there are two possible scenarios:
Design for Fabrication tools, such as that developed by Valor, overcome the problem of differences between fabricators by holding capability information for each, and assessing a layout for compliance against each fabricator. By making the fabricator responsible for updating the capability information in a standard form which can be interrogated by computer, it is relatively straightforward to assess new designs against the criteria set by a number of fabricators and reach an informed compromise. This is a topic that will be discussed in more depth in the Manufacturability Analysis module (AMI4820).
In addition to the unique data set required to pattern a board, containing information on the copper thickness, the build and mechanical data such as board thickness, the ‘data package’ supplied to the fabricator also has either to reference a generic specification for boards, or else contain a specific specification for that particular board.
Some companies produce generic board specifications which are quite extensive, but it is not necessary to “write a whole book”! All that is needed is an agreement as to what the defaults are going to be if they are not spelt out within the individual board specification. The Circatex Designer’s Check List, which contains a simple listing of the information needed, may be found at this link.
One short-circuit to creating a generic specification is to use an IPC classification. Current practice uses just two of the classes in IPC-A-600: Class 2 for commercial and professional boards; Class 3 for products designed to military requirements.
For the occasions where information is not available, some fabricators may keep an internal ‘help file’, formalising information collected from prior experience, and documenting what is known about general company requirements. For example, a company may have a preference for a particular colour of legend, although this is not explicit on the board drawing. However, whilst history may be some guide, there is inevitable commercial risk in taking judgements about what the customer wants, without getting prior agreement as to those requirements. You will ensure that you get what you want only if you ask for it in the specification, or if the generic specification from your company contains an acceptable default condition for each parameter.
We have already indicated that lack of data is a common cause of delay. As a minimum, the designer has to supply information on:
But how do you get it to the fabricator? Some of the possibilities are email, FTP transfer, disk or direct modem transfer. All are secure, and relatively error-free, and much to be preferred to the original method, which was to send artwork! Still used for some older products, artwork needs to be scanned before use by today’s fabricators, so that appropriate dimensional corrections can be made for the processes being used: this is a source of cost, delay and potential error.
The data format is also important. Apart from ODB++, which is described later, alternative formats for the manufacturing layer are:
Similarly with drilling and with drawings, where your fabricator will be able to accept a variety of formats:
Excellon 2 (with embedded drill sizes)
Excellon 2 plus tool list
Excellon 1 plus tool list
Sieb & Meyer
Given the range of possibilities, and the need to specify the layer sequence and build to reduce the possibility of error, you should include in your data set a ‘manifest’, a document listing and describing the files.
Another data item needed is the ‘net list’. Net lists are used for test purposes but are also useful to the fabricator because they make it possible to check that the artwork actually meets the interconnectivity intentions of the designer. Actually, there is much truth behind the claim that the “Net list is the best form of quality check!” There are currently two industry standard formats for net lists for bare board manufacture:
So what does the fabricator do with the information received? The simple answer is to re-engineer your design! Described as the ‘clean-up’ or ‘reverse engineering’ process, this is largely computerised, but demands skill, and may introduce errors.
The fabricator will use workstations running software referred to by the generic name CAM (computer-aided manufacturing). CAM products you will come across most frequently are GC-CAM (GraphiCode), Ucam (ManiaBarco), and Genesis (Valor), but CAD systems often have CAM bolt-ons. Examples of these are CAM350 from Downstream, a spin-off from Mentor Graphics, and Zuken’s Board Producer.
Before you read further, browse for information on these tools. [To start with, you might try searching with the terms <“PCB fabrication” CAM tools>, and then refine this]
What do these systems do? And how do they benefit the fabricator?
Review your answer as you continue to read this section.
The primary function of CAM software is to allow the fabricator to manipulate data into panels, to create information for AOI/electrical test and for NC drilling and routing, and to generate phototools.
However, CAM tools are being increasingly used to verify that a design:
This second task, referred to as a ‘Design Rule Check’ (DRC), is important in reducing shop floor problems. Typically, automatic procedures will categorise each measurement they make into one of three groups, as shown in Figure 4.
As well as identifying specific areas in which rules are infringed, CAM software will generate reports, such as Figure 5, that indicate the overall quality of the design, and the number of places in which rules have been transgressed.
It is important for the designer to remember that CAM software can only check a design and add features for fabrication; it cannot correct, amend or adapt an incorrect design. For this to happen, the design needs to be returned to the design workstation.
The process steps, described briefly below, are:
The first of these stages involves setting up the ‘layer matrix’ (Figure 6), and then compiling the drill list (Figure 7) and setting the drill attributes (Figure 8). The attributes information determines the use being made of the hole, its size and whether or not it is internally plated. This last aspect is important as it affects the connectivity of the board, and hence the validity of the later net list check.
Finally, the board profile information is added (Figure 9), as part of the complete mechanical description of the board.
A potential problem with all mechanical data and related artwork results from the differences between imperial units (commonly used in the USA) and the metric system preferred through Europe. For example, it is well-known that connectors may have spacings based on 2.5 mm or 2.54 mm (= 0.1 inch), and multi-way connectors will quickly show the effects of a mismatch. However, other effects are more subtle, as can be seen from Figure 10, where rounding errors can give rise to a 3.175 µm shift from nominal before fabrication has started.
A number of the CAM operations relate to the interaction between the way in which CAM routines such as Design Rule Checking operate and the way in which CAD programmes generate fills. If an area is built up of a number of lines, net list verification, test data generation and DRC functions will look at each line, and perform their actions on each: the greater the complexity, the greater the time taken, and the greater the possibility of error. In the example shown in Figure 11, four drawn pads account for 5511 bytes of information, whereas, converted to flashed apertures, this is reduced to 32 bytes.
The problem can be surmounted by substituting a simple image for the original line composite. Figure 12 shows the auto-substitution sequence for some SMD pads.
1: Normal PCB view
2: These pads are made up of 0.2mm lines
3: SMD pads now = rect80x40xr4
4: View after substitution
The situation becomes worse where, as in the example shown in Figure 13, the designer inputs a value for the clearance between adjacent copper areas and then ‘floods’ an area (such as a ground plane) with fine lines in order to create a high-definition image: this will drastically slow down the net-list and other checking functions. The ‘contourised’ version is treated by these as being just a single node, despite its complexity.
Drawn ground plane made up of 126,256 0.1 mm lines
Ground plane ‘contourised’ as one surface aperture reduces file size by 90%
One of the problems faced by the CAM software user is that the system treats every copper feature as lines or tracks, unless they have been assigned ‘attributes’ declaring a different function. Two examples of this are shown in Figure 14:
As far as possible, the attribute detection functions are carried out automatically. Another useful attribute that can be set automatically is the designation of a pad as being intended for a SM component (Figure 15).
Gerber 274X pad
After conversion of highlighted pad
Drill holes and SMD attributes are mutually exclusive, and it is usually not desirable to design drilled holes into SMD pads (Figure 16). As a result, auto-detection will usually not recognise SMD pads with drilled holes, and these have to be manually edited.
A bad idea in theory
A bad idea in practice!
Setting object attributes is also used as a way of preventing copper thieving (‘robbing’) areas from taking part in test output generation and design rule checking, creating false results (Figure 17).
The net list is a useful quality check: for engineering, because it ensures that the layout process has not changed the electrical connectivity of the board; for manufacturing, because it ensures that the manufactured product matches the designed output.
As soon as the drill attributes (for example, PTH, non-PTH) have been defined, a ‘reference’ net list can be computed from the CAD or Gerber information, and compared with that in the original net list supplied by the customer.
As with dimensions, this net list comparison with the standard can create a ‘traffic light’:
Graphical comparison functions can also be brought into play to check that intended changes have been mirrored in both net list and design. This can apply both to cases where the connectivity has changed, or where other features are involved, as in Figure 19.
Zoom view shows fiducial removed
In AMI4820 Manufacturability Analysis, you will be introduced to Valor software, but we thought it worth pointing out in this context that the data transfer medium used by Valor has considerable attraction. All the information we have listed so far (layer data; drilling data; net list; drawing) can be cost-effectively contained within a single integrated data set referred to as ODB++. Sent in a compressed format (.TGZ), this can be read directly into the fabricator’s front-end software tools (such as Genesis, Barco, Lavenir, GC-Cam) without any need to identify each individual layer.
The data set is coherent and automatically identifies the layer to which the information refers. It saves time (Merlin claim “We can input ODB++ data 78% faster than Gerber data”) and reduces errors: Merlin measured 226 jobs, and found 41 errors in those supplied with Gerber data (Figure 20) as against zero errors with ODB++ transfers.
There are discernable trends (Figure 21) towards using ODB++ as a transfer medium that reduces both costs and errors, and allows the designer and fabricator to exchange ‘intelligent’ data, or at least data which contains all its intended information without degradation or the need for reverse engineering.
Take as example a circuit that you have designed or know well, and describe:
How might this process have been improved?