Why you should supply us with Gerber X2 files.

The benefits of the Gerber X2 format

Perfectly understanding customer data and not losing any PCB design information in data transfer, are key issues to seemlessly produce and deliver quick turn around PCB prototypes.

In our BLOG section we already explained the history of the Gerber Format. We have written a white paper on which actions we need to perform once we have received your data to check them and make them production ready. And we have informed you that UCAMCO is no longer supporting the old Gerber RS-274D format.

Gerber X2 is todays” standard. Why should you use it?

X2 adds intelligence to the Gerber format by its use of attributes. When PCB Vislualizer processes your new job, attributes allow the software to put the layers directly in the correct position in the stack-up. Other attributes identify the via pads, the SMD pads and so on. This avoids manual interaction and offers extra info for DRC and DFM checks. UCAMCO”s Gerber X2 intro movie offers a sneak preview in the CAM-engineers environment where he uses a UCAM system reading in X2 and experiencing its benefits.

CAD systems – KiCAD, Pulsonix, Easy-PC, DipTrace and Altium – can all generate Gerber X2 files. UCAMCO cooperated with the CAD and other software vendors to validate their X2 output. We like the efficiency of X2, please use it as It will improve data transfer from you to us in a safe and practical way. 

All about the Gerber format on the UCAMCO website

Standard Gerber declared obsolete

Can standard Gerber still be used to order PCBs?

As you can read from Ucamco”s announcement, Standard Gerber (RS-274D) is declared obsolete as input format for their Computer Aided Manufacturing tools for PCB production.

Eurocircuits has for a long time promoted the use of Extended Gerber (RS-274X) for communicating PCB designs as described in our BLOGs:

It”s safer, faster and fully compatible with our PCB Visualizer tools.  PCB Visualizer cannot process Standard Gerber files as they are incomplete, lacking the built-in shape definition tables etc…

We therefore support Ucamco”s decision to declare the Standard Gerber (RS-274D) format obsolete.

=> Yes, you still can use Standard Gerber (RS-274D) but we STRONGLY recommend you to use Extended Gerber (RS-274X) instead.

If you have any questions on outputting Extended Gerber, please contact us via our Chat service or email us at

euro@eurocircuits.com

This e-mail address is being protected from spambots. You need JavaScript enabled to view it

.  If you need boards made from old files which are only available in Standard Gerber, please contact us on a case by case basis.

We recommend you to also read Ucamco”s announcement in this BLOG.

Open Letter to the Gerber User Community

Please use Extended Gerber for all your operations.
Standard Gerber is technically obsolete.  If you are still using it, you are putting your business and that of your clients and business partners at a useless risk, without benefit.

As the developer and custodian of the Gerber format, Ucamco hereby wishes to communicate the following important information about Standard Gerber.

Standard Gerber is now technologically obsolete.

  • Despite its name, Standard Gerber is not a defined standard for PCB data transfer:  Units and aperture definitions, rather than being governed by a recognisable standard, are in an informal document, the interpretation of which is unavoidably subjective. As a result, Standard Gerber files cannot be machine-read in a standardized, reliable way.
  • Standard Gerber requires aperture painting and copper pours, both of which create manual work in CAM, adding cost, delay and risk to the PCB manufacturing process.
  • Standard Gerber does not support attributes.

Extended Gerber files ARE machine readable, they do not require painting, and they do support attributes. Virtually all software read Extended Gerber and many new implementations no longer support Standard Gerber. There is not a single good reason left to use Standard Gerber. Using of Standard rather than Extended Gerber is a self-inflicted competitive disadvantage.

Extended Gerber fully supersedes Standard Gerber. Extended Gerber is the current Gerber format. Standard Gerber files therefore do not comply with the Gerber specification.

Ucamco”s position regarding the Gerber format is therefore as follows:  Any party that chooses Standard rather than fully standardized Extended Gerber is responsible for any issues that might arise as a result of its use.

Thank you.

Karel Tavernier
Managing Director
Ucamco

Read the full article – with detailed motivation – in pdf format

Gerber past, present and future

More than 95% of all PCB designs produced worldwide are transferred from designer to fabricator as Gerber files. On most CAD systems the Gerber files are output automatically. It is only rarely the designers have to concern themselves about how a Gerber file represents their data. This in itself is a good measure of the power and ubiquity of the format, but occasionally an issue arises where some background knowledge may be helpful – and there are developments being planned for the format which will make it even more useful in future.

Gerber past:

Why “Gerber”?

Joe Gerber (1924 – 1996) was a US inventor who had fled from Austria to the US in 1940. Right from his student days he was interested in accurate data plotting, and during the 1950’s he developed the digital XY co-ordinate table which became the core of his future business, Gerber Scientific. The first product he launched using the new table was one of the world’s first digital drafting machines. Among later products was automatic cloth cutting machinery which is still widely used in the world’s garment industry. In the ‘80s he developed computerised equipment for machining spectacle lenses, again still used today.

In the 1960s Joe Gerber found another use for his XY table. He introduced the world’s first NC photoplotter to generate the phototools used to produce PCBs. It worked by first moving an optical head containing a light source to the correct location over the film on the bed of the plotter. A circular wheel with different sized/shaped holes in it (apertures) was then rotated so that the correct aperture was under the light source. For a pad the light-source was flashed on and off, exposing the pad on the film. For a track the light was left on while the head moved, drawing the track on the film. Hence we still talk about “aperture tables”, and, less often these days, “flashes” and “draws”. The plotters were known as vector plotters as the head followed the actual pattern of the PCB. The actual drive format was based on a pre-existing format, RS-274-D, developed by the US Electronic Industries Association (EIA) to drive any NC machine. The data was loaded into the very first Gerber photoplotters on punched cards.

RS-274-D becomes RS 274X

By the early 1980s PCB Computer-Aided Design (CAD) systems were becoming more common, replacing the old hand-taped 2:1 artworks. CAD systems could output drive data directly to a photoplotter to generate the phototools. At that time most photoplotters were Gerber plotters. Other vendors moved into the photoplotter market, but as Gerber had published a full specification of their format in 1980, Gerber RS-274-D became the de facto standard.

As a vehicle for transferring PCB layer images, the format had one critical limitation: the size, shape and number of the apertures was limited by the physical aperture wheel. This worked (more or less) for designs using conventional through-hole components with round or square pads, but it couldn’t handle the new surface-mount components which used a wide variety of mainly rectangular pad sizes. Using RS-274-D the only solution was to “paint” the pads with tiny draws. Similarly, a simple plane layer could be plotted in reverse, that is, the clearance holes in the plane are plotted black and the board manufacturer reverses the polarity either in his front-end CAM system or physically by contact printing. But this won’t work for mixed plane layers or planes on signal layers. These had to be filled with draws. A large image with SMDs and planes could take up to 24 hours to plot on this type of plotter.

The solution was a new type of photo-plotter and a new format. The raster photo-plotter used a light source, typically a laser, to raster-scan the film in a continuous pattern. The image was built up by a sequence of laser on, laser off commands. Now any shape could be plotted, built up of raster pixels. Today this is the standard industry tool for photo-imaging PCBs, with laser photo-plotters using up to 48 independently-switched simultaneous beams plotting at resolutions down to 50,000 dots per inch or more.

Now it was possible to make the Gerber format more flexible and more suited to the requirements of the PCB designer. RS-274X or Extended Gerber was launched in 1991. This allowed the user to define and image any shape, as a pad, a track or a polygon (plane). The aperture definitions no longer depended on a physical wheel and so they could be derived automatically from the CAD job and included in the file as part of the output.

Gerber today.

RS-274X is the standard PCB layer image data transfer format used today. It is clear, unambiguous, and, if any questions arise, man-readable. Each file is complete and allows you to draw any pad-shape or copper area that you want.

The old Standard Gerber RS-274-D still lingers on, despite its drawbacks. It is very limited; it needs a separate aperture table which often seems to go missing; it produces huge and unwieldy files; the output may require the merging of positive and negative images which at best requires extensive clean-up and at worst generates hard-to-spot errors.

Eurocircuits can still accept the older format if needed, e.g. for old jobs, though it does not work with PCB Visualizer. However, Extended Gerber, RS-274X is our preferred format as it has none of the limitations of RS-274-D and as each file is complete including the embedded aperture definition it works with PCB Visualizer, offering you all the benefits of our advanced data checking technology. All current generation and most older CAD systems generate RS-274X output. If your CAD system is still outputting the old-style Gerber RS-274-D, look into the output settings. Sometimes it is possible to switch from RS-274-D to RS-274X. There may be different terminology used on different systems. If you are in doubt, ask us.

For more advice on input formats, go to our PCB Design Guidelines

Gerber tomorrow.

Extended Gerber, RS-274X, provides an exact and unambiguous image of the layers of a PCB, but there is still some layer information which is necessary for fabrication (especially for automated data preparation) but is not included in the format.

Examples include:

  • What is the function of this layer: top copper, top solder mask, etc.?
  • Does the image show a single PCB or a delivery panel?
  • What is the function of this object: is it a SMD pad or a via pad, fiducial etc.?
  • What is the board profile? Automatic recognition software like PCB Visualizer can recognize rectangular profiles but not complex shapes.
  • What are the drill tolerances on this hole? For example, it may be a press-fit hole.
  • Which are the impedance-controlled tracks?
  • Which vias need to be filled?

The next step is to incorporate this type of information into the data transfer format. Any such further extension of the format has to be compatible with the existing format and with existing CAD systems. Although other formats have been proposed which can include non-image information, Gerber is so widely used and so effective in operation, that, like the QWERTY, QWERTZ and AZERTY keyboards, it cannot be easily replaced.

The Gerber format today is maintained and developed by the Belgian company Ucamco which bought the PCB Division of Gerber Scientific in 1997. Ucamco have recently published the blueprint for the next generation of RS-274X, Gerber RS-274X2. This adds attributes into the format which convey the information listed above.

This new development is further explained in our technical blog on Gerber X2. Eurocircuits are working closely with Ucamco on the new format as part of their drive to provide better tools for the European and global PCB design community. As the new attributes are implemented into CAD systems, we will add new functionality into our data input and validation procedures to handle them. Of course, we will also continue to accept the older Gerber formats.

Extend Extended Gerber – Gerber X2

Gerber”s new attributes set to transform CAD to CAM communication

With the support of Eurocircuits,, LPKF and AT&S, Ucamco drafted a new specification for a ground-breaking second extension to the Gerber format. This offers an unequivocal standard for non-image data that is just as simple, practical and universally accessible as the well-known Gerber image data format it now supports.

Ucamco“s Managing Director Karel Tavernier comments: “CAD/CAM professionals need to transmit data in a robust, reliable and cost-effective way, something the Gerber image format has been doing for years. It”s freely available, simple and to the point. It can be used by everybody, no matter how big or small the CAD or CAM operation is. It”s the most practical image description format out there, and by far the most used by our industry – every single day thousands of perfect PCB layer images are reliably transferred all over the world thanks to Gerber”.

Indeed, with Gerber, CAD/CAM professionals know that the most critical and fragile part of their archives – the image data – is secure and accurate. But there is another part of the PCB design that images cannot convey. This non-image data includes information about layer order and function, the differentiation between objects like SMD and via pads, and a raft of further information that, together with the image data, helps to translate designers” intentions into high performance products.

The problem is that there is currently no Gerber standard for transferring non-image data, leaving designers to decide for themselves how best to communicate with their manufacturing partners. They might add text files or drawings to their Gerber archive, or they might not, putting the onus on CAM engineers to search for the necessary information, or contact the designer if it”s missing. These are error-prone, time-consuming tasks that can end up affecting quality and deadlines, which can translate disastrously into loss of orders, clients and future business, especially in the time-critical context of prototypes and quick-turn boards. Thus whether you are a designer, customer or manufacturer of PCBs, data quality and clarity should be a top priority for you.

This is why Ucamco has developed its Gerber X2 format. X2 offers a series of attributes that provide a standard for describing non-image data – some might rather grandly say that they add intelligence to the image data. Applicable either to a whole file or to individual graphic objects, Gerber”s standard attributes can now be used to define

  • Gerber file function: top copper layer, top solder mask, etc.
  • Part: single PCB, customer panel etc.
  • Object function: SMD pad, via pad etc
  • PCB profile
  • Drill tolerances
  • Locations of impedance-controlled tracks
  • Filled vias
  • An MD5 checksum for added security

The attributes have been purposely crafted, from scratch with the sole aim of supporting the transfer of PCB data from design to manufacturing. They are essential, simple and focused rather than a casual smorgasbord of “nice to haves” with unnecessary complexity, not to mention potential bugs. There is no overhead of manufacturing specific attributes as are found in CAM formats. X2 is simple and clean.

The attributes intentionally do not cover all possible non-image data. Ucamco refrained from adding the netlist to X2 as there is a simple and well-established format adequately describing netlists: IPC-356-A. Materials were not added as they are not linked to images and can be handled by a subset of IPC-2581 as soon as 2581 is opened up to partial implementations. In this way X2 delivers the best of all worlds: accessibility, simplicity, performance, and tried and tested formats that work for everybody. It”s a great combination that gives designers a clear and simple method for ensuring that their manufacturing partners have all the data necessary for efficient, reliable manufacture. And it eliminates the need to adopt complex new formats wholesale, which is a blessing, as Ucamco R&D engineer Thomas Weyn explains: “Imaging software, notoriously hard to implement, takes forever to debug and field test, especially for images as complex as PCBs. Here, errors are fiendishly difficult to detect and almost inevitably lead to scrap, so it is far preferable to keep what we know works (the Gerber image format) and support it, without disrupting it, with what is missing”.

A prime design goal of X2 is ease of adoption and of implementation. To fully exploit the productivity jump that X2 can bring, CAD and CAM software only requires quite minor updates. Given that the imaging model remains unchanged, it only requires adding a few extra lines with the attributes when writing a Gerber file – it could hardly be simpler. The payback for this is a more versatile product and greater competitivity for systems vendors. The attributes” use is not mandatory: they can be used wholesale, partially or not at all, whichever suits the implementation best. Most importantly, systems that have not been updated will still generate the correct image as Gerber X2 is upward compatible with previous versions of the format as the image is not affected by the attributes. Existing workflows are not broken by introducing X2.

Before the final version goes live, Ucamco encourages CAD and CAM professionals to look at it and in particular at the Attributes in Section 5, and participate in its fine-tuning by sending comments to gerber@ucamco.com

In order to make X2 happen, Ucamco need CAD software vendors to buy in to X2. As X2 is easy to implement, it makes a chance. But they need your support. Please write to Ucamco at gerber@ucamco.com and let them know that you support the Gerber X2 format, and that youy would implement it in your workflows when it is available.

The draft Gerber X2 second extension is available at www.ucamco.com/downloads and a brief press release describes the rationale for its development.

Front-end data preparation – new white paper

“What do PCB fabricators do with my data before they make my PCB?”

 

“Why can’t they use my data just as I sent it in?” “Why do I need to know? I’m an electronics engineer and they are the board fabricators?”. Our new white paper, “Front-end data preparation”, answers these questions.

An understanding of the front-end data preparation process is important for two reasons, speed and cost. PCBs for time-critical applications need to be delivered fast and on time. If information is missing from the data set supplied or if it is ambiguous or unclear we lose time while the issues are sorted out. The new white paper explains how we verify that the data is complete and clear, to make sure that we deliver the board that you want. Above all, it contains tips on how to present clear and unambiguous data and avoid some of the common traps which can delay deliveries.

Our pooling services have been developed to deliver prototype and small batch PCBs cost-effectively as well as fast and on time. The specifications of each service are based on a robust level of manufacturability to ensure the quality of the finished product. This is reflected in the cost structure: TECH pool is more expensive than STANDARD pool. The white paper outlines how we check that each design fits the specification of the chosen service. If it doesn’t, we report back the data issues (raise an exception). Are there simple steps which you as a designer or we as fabricators can take to avoid having to use a more expensive option? If so we will propose them. Are there repairs we can make to bring the board back within specification and improve its manufacturability? In many cases we can make these repairs as part of the data preparation process and the white paper has links to more detailed information. Design for manufacturability tips highlight some critical areas. The white paper also links to the free design rule sets which can be uploaded form our website into EAGLE and Altium CAD systems to help ensure that your design meets the specifications of the most cost-effective pooling service.

Although the white paper follows our internal procedures and includes the names of our front-end data preparation stages, our data preparation process follows industry best-practice. So throughout we relate what we do and our design tips to the wider PCB fabrication world. Our goal is to provide a broad set of technical information which will benefit not just our users but also the wider electronics engineering community across Europe.

Download the Eurocircuits-frontend data preparation white paper in PDF format.

To preserve the environment and to make use of the many embedded links to articles on our web site, we recommended that you read this white paper in its digital form.

Eurocircuits production data – what’s in it?

To produce your board we use your design data in Gerber or EAGLE format and first perform the necessary front end actions as described in our white paper: “What do PCB fabricators do with your data before they make your PCBs?“.

When this is done and your board is ready for production, we save your board’s production data in your account. This data we call the job’s “single image” data. “Single image” means the data we load onto our order-pooling production multi-panels, so it may refer to a single circuit image or to a delivery panel if this is what you have ordered. This is the data that is visualized in the PCB image. You can download the full set from within your customer account.

 


The download of the single image production data from the Eurocircuits site has been possible since we launched our e-business platform more than 10 years ago. This open business policy has convinced customers over the years to come to us for their prototypes and small series even if they planned to have their large series produced in the Far East. We offer a fast and convenient way to calculate prices and place orders, a thorough data verification and manufacturability analysis and highly professional production processes. Combine this with the possibility to download the verified data and use it for production wherever else you want, and you have the best possible start for the life cycle of your products.

The single image files are name coded by Eurocircuits. But this is no secret either. Let us explain what the files are and what their names stand for.

file name convention.docx

 

The format of the files is mainly DPF. This is the internal format for UCAM, the front-end data preparation or CAM (Computer Aided Manufacturing) system we use designed and developed by Ucamco. The paste files can also be downloaded as Gerber data. To read DPF files as well as Gerber data and Excellon drill files we recommend GC-Prevue, available as a free download from www.graphicode.com.

We are sometimes asked if it possible to reload the single image data back into a CAD system. This is totally dependent on the CAD system. We have only input and processed manufacturing data. Other PCB manufacturers can use it for production through their own CAM systems. However the manufacturing data doesn’t contain any component information like foot-print coordinates or a functional net-list where nets are linked to component pin numbers and are described as power, ground, data line, etc… A successful reload of DPF or Gerber production data into a CAD system depends entirely on the functionality available in the CAD-system and should be investigated there.

Our team will gladly answer any queries you may have. Contact us on euro@eurocircuits.com.

Eurocircuits Data preparation – Make production panels

By now your job has already been through two of the three front-end data preparation stages :

Stage 3 – Make production panels and production tools

We now have a stack of orders that are ready to go into production.

Our business model is based on “order pooling”. We make our production more efficient by processing several different orders on the same production panel. More efficient production means lower prices for our customers, especially for prototype and small batch orders. Which orders can be pooled together? This depends on a lot of factors, and finding the right balance is our daily challenge.

We need to consider:

  • Delivery term : we separate rush orders from standard delivery orders. If we put both on the same production panel we could find that all panels have rush orders on them. If every job becomes urgent, production efficiency goes down and our delivery performance is affected.
  • Order size : we keep large and small orders apart. The higher the number of panels in a job, the longer it takes to process. Production planning becomes less flexible and again we risk deliveries.
  • Copper distribution : we discussed this already in our earlier blogs about our new plating simulation tool and the Elsyca Intellitool Matrix plating project. We need to be sure that the designs we pool together don’t reduce each other’s plating quality.
  • Classification/complexity of the boards : combining complex jobs with simpler jobs means that the final panel is more complex than it need be and so more expensive to produce. That’s why we have two different pooling services ‘STANDARD pool” for standard boards and “TECH pool” for more complex boards.
  • Technology: some technology options clearly can’t be combined with each other, for example different materials, copper weights and build-ups. In other cases combinations might reduce production efficiency or quality. For example we could in theory combine boards with different legend colors on a single production panel. In practice this would need two printing processes and two curing stages. We would lose time at the print stage and risk the quality if the panel went through too many heating/cooling cycles.

The final decision day by day on which orders are combined on which panel is made by highly skilled and experienced engineers. They have a growing number of software tools to help them to make the best decisions, and we are investing a lot of manpower and resources to develop even more powerful tools for the future.

Once the engineer has chosen the orders for the panel, how do we make it ready for production?


Panel preparation for production

Most of the steps below are fully automated processes

  • Run a Drill Tool Reduction: on pooling panels we remap all drill sizes larger than 1.00 mm to new tool sizes with a step of 0.10 mm rather than 0.05 mm – provided, of course, that we can still maintain the tolerance specifications of the finished hole size. This can reduce the number of different drill sizes needed by up to 60%, which in turn reduces total drilling times and so cuts cost of your PCB.
  • Add any customer-specified markings to the boards on the panel, for example UL markings or customer-specific date-codes.
  • Add different test coupons to the panel for inline quality checking. Together these coupons contain specific features which allow us to check all process steps and make sure that the panel meets all production specifications during and after the production.
  • Add specific galvanic compensation patterns (“robber/thieving bars”) to the open panel areas. This optimizes the final plating results and ensures that after plating the copper thickness in the holes and on the tracks is within the production specifications.
  • Add etch-compensation to meet the panel and production specifications. When we etch down into the copper the nature of the process means that we also etch away a small amount of copper to each side (“under-cut”). Etch compensation makes a small increase in all copper features so that after any under-cutting the feature size is as designed. This is especially important to maintain correct track widths.
  • Calculate the other data we are going to need for panel checking and manufacture, like the total copper surface area or the copper distribution, information which we will need for calculating plating currents.

Panel checking and optimization

  • Perform a galvanic plating simulation to ensure a uniform layer of plated copper over the entire panel within the production specifications. At this stage our engineers may move the circuits around on the panel or change the galvanic compensation patterns to get the best possible plating result.
  • Drill optimization. For each separate drill run on the panel, the complete drill path – the order in which all the holes are drilled – is automatically optimized to get the lowest possible drill time.
  • Routing optimization. For each routing operation on the panel, the complete rout path is optimized. Here we rely on experienced production engineers to get the best possible combination of edge finish, mechanical stability of the panel during routing, and shortest routing time.


Panel plating image samples:

  • Bad copper distribution
  • Good copper distribution

Panel output generation

  • Drill output: we generate drill output files for each drill operation required on the panel (plated, non-plated, blind, buried). These output files will drive our various drilling machines.
  • Rout output: rout output files for all the routing and milling operations needed (board profiling, slots, internal cut-outs). The output files drive the routing machines.
  • Plotter output: plot-files for our laser film plotters for all layers produced by photo-imaging (copper layers and soldermasks).
  • Legend output: for legend (“component ident” or “silk-screen”) printing we use digital ink-jet printers. As well as the legend pattern the output files can contain an instruction that prints a unique barcode on each individual PCB. When tests are completed this will give our customers who want it the ultimate in traceability.
  • Electrical test files for our different electrical test machines. Production panels are electrically tested before the single images are routed out. If needed a single board can also be electrically tested after final board profile routing.
  • AOI (Automated Optical Inspection) output generation. AOI testing is an automated optical comparison between the digital data supplied for the PCB and the actual copper layer we have produced. We AOI test all inner layers to detect shorts, opens and other faults which cannot be rectified once the board is bonded. We also AOI test some outer layers depending on the technology level of the panel.
  • Other information needed for manufacture such as:
    • the surface area and density calculations for copper layers, soldermask layers, plating layers, etc
    • panel images
    • drilling, routing and scoring drawings etc…

To production

The complete production panel job and all generated output data are packed together in a structured zip container and uploaded to the system.

The production panel is now ready for manufacture. Our production planners decide which production unit is going to actually make the panel (Eurocircuits Kft in Hungary or Eurocircuits Aachen in Germany). The decision is based on the technology required, the size of the job, the delivery term and available capacity.

Eurocircuits data preparation – Single Image (part II) – other layers and outputs

Have you ever wondered what we are doing to your data when the order status is Single Image? Here is the answer based on the instructions we give to our data preparation engineers. Many of the steps described below are automated for speed and accuracy but we have ignored this to make a clearer presentation. More information on our requirements can be found on the home page under “Technology Guidelines”.

Stage 2 – Single Image data preparation (Single Image and Single Image Cross Check)

We covered before :

  • Eurocircuits data preparation – Analysis : the initial stage, checking if the data are complete and no obvious problems are there to fulfill the order.
  • Eurocircuits data preparation – Single Image (part I) – drill data and copper layers. : Verify and clean up the drill data and the outer and inner-layers.

This current article, Eurocircuits data preparation – Single Image (part II) – other layers and outputs, is our third article in a series about frontend engineering and is about the preparation of Soldermask, Silk screen (legend), coding on PCB”s, making customer panels, machine outputs: “drill layer, rout layer, V-cut layer”, SMD paste layers and optional other layers.

Solder-mask preparation

  • Replace any painted pads and areas with proper flash pads and polygons as for copper layers
  • Check for missing soldermask pads on component holes or fiducials
  • Check and add soldermask clearance pads on all non-plated holes
  • Check and correct the cover between the edge of the soldermask and the adjacent copper tracks or planes (= Mask Overlap Clearance or MOC) depending on the specification of the pattern class
  • Check and correct the clearance between the copper pad and the edge of the soldermask (=Mask Annular Ring or MAR) depending on the specification of the pattern class
  • Check and correct the minimum width of the solder-mask bridge between adjacent soldermask pads (=Mask Segment or MSM) depending on the specification of the pattern class
  • Save job


Silk-screen (Legend) preparation

  • Check and clip clearance to the board outline
  • Check and correct minimum text width to 0.17 mm
  • Clip the silk-screen data to ensure that there is no ink on component pads
    • As standard clip back 0.10 mm from the soldermask
    • If there is no soldermask clip against the copper pads, plus drill holes, plus rout layer
    • If there is no copper clip again the drill holes, plus rout layer
  • Save job

PCB coding

  • Add the Eurocircuits order number on the top or bottom silk-screen layer as specified
  • Add UL marking indication and any customer-special marking indication as ordered
  • Add Barcode coding (for traceability) as per specification
  • Save job

Drill drawing preparation

  • Assign standard hole-size symbols to the drill holes and provide the key
  • Check that all required dimensions and tolerances are indicated
    • For slots, indicate width, length, plated or non-plated
  • Add any additional information required:
    • Special routing or depth routing
    • Press fit holes
    • Other useful information
  • Save job

Rout layer preparation

  • Copy outline to rout layer
  • Check for any customer special instructions for board profile and prepare accordingly
    • Special rout shapes and tolerances
    • Non standard tooling (radius, …)
    • Specific requirements for a customer panel
    • Separate outer (profile) routing from inner routing (cut-outs and slots) and apply proper tool sizes and numbering
  • Convert drill holes larger than 10 mm into inner routing
  • Check and set rout directions
  • Apply tool compensation
  • Add break tabs according to specifications
  • Check and set correct tool sequences for pre-drills, routing stage drills, inner/outer routings
  • Save job

V-cut ( scoring) layer preparation

  • Create V-cut layer with 0.90 mm V-cut draws as per specifications
  • Save job

Paste layer preparation

  • If solder paste data is supplied by the customer use it without modifications
    • convert any painted pads to flash pads.
  • If no solder paste is supplied prepare the paste layer from the board data. Select all non-drilled, flashed pads that are free of soldermask and copy to a paste layer.
  • Save job

Special layers preparation

These layers will be prepared only when ordered.

  • Gold Finger Layer Preparation
    • Create the gold finger connections according the specifications
    • Add specific routing for the gold edge-connectors
    • Check the connections widths and positions and the bus bar width and position against the modified mechanical layers

  • Peel-off Layer Preparation
    • Create the peel-off layer as specified by the customer
    • Check that it is conform to our production requirements and resolve any errors.
  • Via-Fill Layer Preparation
    • Create the via-fill layer as specified by the customer
    • Check that via-fill is only applied on 1 side of the PCB. This cannot be the side with any BGA on it
    • Check that the via-fill layer is conform to our production requirements and resolve any errors
  • Carbon Layer Preparation
    • Create the carbon layer as specified by the customer
    • Check that it is conform to our production requirements and resolve any errors

Make a customer panel

The Single Image (the “deliverable”) may be a customer-specified panel or array. There are three options here:

  • Panelisation done by Eurocircuits according to the Eurocircuits standard panel rules
    • Create a Eurocircuits standard panel using automated panelisation routines in accordance with the order details:
      • Step X and Y
      • Panel border width
      • Distance between the individual circuits
    • Check for panel stability
      • Check routing or V-cut positions
      • Check break-tab positions and add more if needed for panel stability
  • Panelisation done by Eurocircuits to the customer’s specification
    • Prepare the panel to the customer’s panel drawing
    • Check for panel stability
      • Check routing or V-cut positions
      • Check break-tab positions and add more if needed for panel stability
  • Panelisation done by the Customer
    • the customer supplies fully panelised Gerber data
      • Check for panel stability
      • Check routing or V-cut positions
      • Check break-tab positions and add more if needed for panel stability
  • Save job

Final Check

  • Build a new netlist from the current data and check it against the reference netlist saved immediatly after the customer data was loaded.
  • If there are any differences between the two netlists, find the reason for it and correct when necessary.
  • Check each copper layer against its original data
  • Some differences are caused by our actions to make the board easier to produce, ignore them and find out where all other difference originate from and repair if needed.
  • If there are no more errors:
    • zip the job data
    • upload it to the system to allow for the next stage in the preparation process to begin

A second engineer now runs a series of checks to confirm that the production data matches:

  • the customer’s order and his other instructions
  • the specifications of the chosen Eurocircuits service

If there are any errors, these must be corrected. When the data is confirmed as correct, it is passed on to the next stage where it will be placed on a production pooling panel. We will bring this story shortly.

Eurocircuits data preparation – Single Image (part I) – drill data and copper image

Have you ever wondered what we are doing to your data when the order status is Single Image? Here is the answer based on the instructions we give to our data preparation engineers. Many of the steps described below are automated for speed and accuracy but we have ignored this to make a clearer presentation. More information on our requirements can be found on the home page under “Technology Guidelines”.

Stage 2 – Single Image data preparation (Single Image and Single Image Cross Check)

The name “Single Image” may be slightly confusing as it includes both single circuits and customer panels or assembly arrays. We use it to mean what we will deliver to the customer (individual circuit or panelised array) in contrast to our pooled production panels.

Build the job

  • load the job data received from Stage 1 (Analysis of PCB CAD data)
  • remove everything outside the board outline.
  • build a job netlist from the drill and Gerber data. We will use this later to check that we have not made any mistakes during the data preparation. If you have supplied an IPC netlist from your CAD system we will check the job netlist against this at this stage and raise an exception if we find discrepancies.
  • save a copy of the layers as received as a reference for later checks.
  • load the correct build-up for the job using the material thickness/copper thickness etc specified in the order
  • save the job.

Prepare the drill layer(s)

  • calculate the Nominal Hole Size. Where our standard tolerances (+/- 0.1 mm) apply, the nominal hole size is the finished hole size specified in the data (e.g. 0.80 mm). Where the designer has specified his own tolerance (e.g. +0.1/-0.00) we will aim to produce a hole in the middle of this tolerance band (so the Nominal Hole Size will be 0.85 mm).
  • increase the Nominal Hole Size to the Production Hole Size to accommodate the plating on the hole walls, the mechanical tolerances of the drilling machines etc. This is to ensure that every finished hole size is within tolerance. The rules are:
    • plated holes with finished diameter of 0.45 mm or less (taken to be via holes): increase by 0.1 mm.
    • plated holes with finished diameter of 0.50 mm or more (taken to be component holes): increase by 0.15 mm.
    • non-plated holes: increase by 0.05 mm. This is due to the bounce-back of the laminate: the drilled hole is always slightly smaller than the drill diameter.
  • Sort and regroup all drills and slots in the correct functional drill layer.
    • Put all drill and slots – PTH and NPTH – to the first drill run
    • Move any NPTH drill, slot or inner cut-out that is or can be seen as part of the board profile to the profiling run.
    • Move all NPTH drills larger then 6.00mm to the profiling run.
    • Move all NPTH drills and slots that are in a copper area (pad or plane) to the second drill run or the profiling run as per production requirements.

There are 3 possible steps in the production flow where we can drill holes:

  • First Drill Run or plated drill layer:
      • This is one of the first steps in production. All holes drilled here will become plated (PTH)
      • unless the hole is being covered with dry film, this process is commonly known as “tenting”
  • or “tented NPTH hole”. Tented NPTH holes MUST have a copper clearance of 0.30mm and can
  • have a maximum size of 6.00mm.
  • Second Drill Run or non-plated drill layer:
    • Is performed after the electroless plating process (or blackhole process). All holes here are non-plated (NPTH)
  • Profiling run or rout layer:
    • Is the last step where the profiling of the board is done. These holes are also non-plated (NPTH)

Outer Layer preparation

  • Clean the data
    • Replace any painted pads and areas with proper flash pads and polygons. Painted features filled with small draws were common in old-fashioned standard Gerber data but are not needed with Extended Gerber where you can define any pad shape or filled area you require.


Check for missing copper pads on plated-through holes (PTH).

  • Check non-plated holes (NPTH)
    • Any NPTH hole which has a copper pad that is smaller than the hole, remove the copper pad
    • For the NPTH in the first drill run (Tented NPTH): Check the drill to copper clearance, it should be minimal 0.30mm.
      • Repair if needed by creating 0.30mm clearance to copper (=same repair methods/restrictions as Minimum copper to edge clearance in DRC – see article about Data Analysis)
      • If impossible to repair then move the NPTH to the second drill run or the profiling run as per production requirements.
  • Check and repair the copper free area of 0.25mm for all elements from the rout layer (=same repair methods/restrictions as Minimum copper to edge clearance in DRC)
  • Run automated design-rule checks (DRCs) to find violations against the minimum required design specifications of the chosen service. At this stage, any violation found should normally be repairable by us.

To ensure a robust end product with optimum plating, no drill breakout and, where relevant, good solderability, we look for a minimum annular ring of copper around the hole. This ring is measured from the production hole (the TOOLSIZE) which is oversized from the finished size (the ENDSIZE) to allow for the plating in the holes. For inner layers the annular ring required is larger than for outer layers to compensate for any movement in the material during bonding. For the values required see “PCB Classification” under “Technology guidelines” on our home page.
  • Check and repair minor copper defects which may cause problems in production: peelables (see PCB Design Guidelines p. 11), pinholes and copper slivers:
    • The dimensional values of the copper defects to be detected depend upon the pattern class – Peelables and Pinholes are filled, Slivers are removed.
  • Save the job.

Inner layer preparation

  • Clean the data as for outer layers.
  • Remove all non-functional pads
  • Check for missing copper pads on connected plated-through holes
  • Check and repair the copper free area of 0.25mm for all elements from the rout layer (=same repair methods/restrictions as Minimum copper to edge clearance in DRC).
  • Check and repair all thermal pads as needed
  • Check for proper thermal to plane connections, rotate the thermal if needed – Min thermal “air-gap” should be 0.20mm.
  • Run automated design-rule checks (DRCs) to find violations against the minimum required design specifications of the chosen service. At this stage, any violation found should normally be repairable by us.
  • Save the job.

This is the end of the drill data and copper image preparation. The next article will cover Soldermask preparation, Silk screen (legend), coding on PCB”s, making customer panels, machine outputs: “drill layer, rout layer, V-cut layer”, SMD paste layers and optional other layers.

Eurocircuits data preparation – Analysis

Have you ever wondered what we are doing to your data when the order status is Analysis or Single image? Here is the answer based on the instructions we give to our data preparation engineers. Many of the steps described below are automated for speed and accuracy but we have ignored this to make a clearer presentation. More information on our requirements can be found on the home page under “Technology Guidelines”.

Stage 1 – Analysis of PCB CAD data (Analysis and Analysis Cross Check)

Analyse the data files

  • Sort the data into Gerber files, Excellon drill files and any additional files (doc, txt, pdf, …) If the data comes in CAD format (EAGLE) convert into Gerber files, drill files etc.
  • Check the additional files: is there any job information there that is not in the Gerber/Excellon files or in the order (e.g. copper weights, soldermask colours, panel setup, tolerances, layer build-up etc)?

Convert the data into the format used by our data preparation software (DPF)

  • Upload and convert the Gerber and drill data. Is there critical information in aperture-lists, tool-lists or other files?
  • Check for undefined apertures or drill-tools (hole sizes) or 0-size apertures or drills

0-size aperture in the left image, should have been aperture 0.8 as in the right image.

Build the basic job


  • Give each file its proper description. These designators are used for subsequent automatic processing. The file may be:
    • a Copper layer: outer or inner
    • a Drill file: plated (PTH), -non-plated (NPTH), buried, blind
    • an Extra file: (solder)mask, silk(screen), rout, score, outline, paste, peeloff (mask), carbon,…
  • Stack the layers correctly in the job build
  • Align all layers exactly to each other.
  • Check that all layers “read” correctly. As we always view the data through the board from the top, the top layer should read correctly and bottom layers should be mirrored.
  • Reverse any “negative” plane layers where the Gerber image shows the pads etc that will be clear (not copper) in the finished board.
  • Create the outline layer. This layer represents the actual board size and shape.
  • Delete the board outlines from the other layers (but it’s a good idea to include them in the Gerber data so that we can make sure that all the layers are correctly aligned)
  • Save job

Mixed readable and mirrored text (left) – Top right corner cut out ? (right)

Check the data against the order and the specifications of the chosen service.

  • Check the job data against the order details:
    • number of layers, board size, single board or customer panel
    • soldermask and silk options
    • specific requirements such as edge plating, gold edge-connectors, carbon, peel-off mask, viafill etc.
    • specific requirements such as special build-ups, special materials, thickness of board and copper, specific tolerances, blind/buried vias.
  • Check the copper data against the drill files: are there any missing copper pads?
  • Check the drill data against the copper data: are there any missing drill holes?
  • Check the soldermask data against the copper pads: are there any missing soldermask pads (windows)?

Check the data against the minimum values of the chosen service

  • Check for minimum finished drill size: for example, a finished hole size less than 0.25 mm is not allowed in STANDARD pool.
  • Check for slot and cut-outs less than 0.50 mm in width – not allowed in any service.
  • Check for drill-drill distance <0.15 mm – not allowed in any service.
  • Run automated design-rule checks (DRCs) to find violations against the minimum required design specifications of the chosen service.
  • Any violation that is found will be evaluated:
    • Is it repairable by us without compromising the board functionality
    • Is the number of repairs or the complexity of the repairs needed in line with a normal data preparation process. Too much or too complex repairs are most often better solved on the customer side in the CAD system.
  • Following DRC checks are performed:
    • Minimum track width. Violations against minimum track-width will not be repaired by us
    • ]
    • Minimum isolation distance. Violations against isolation between tracks or between track and pad will not be repaired by us
    • Violations against isolation between track or pad and a copper plane can be repaired by locally withdrawing the copper plane area.
    • Repair is only possible if we do not create open nets in the copper plane.
    • Minimum ring of copper round drill holes on outer layers (Outer Annular Ring – OAR). OAR violations on via holes can be repaired by reducing the via drill size (the limit is the minimum via size for the pattern class) possibly in combination with enlarging the copper pad. All holes with finished diameter of 0.45 mm or less are considered being a via hole. OAR violations on component holes are repaired by enlarging the copper pad. The repairs can only be done provided they do not violate an isolation rule which cannot be repaired.
    • Minimum ring of copper round drill holes on inner layers (Inner Annular Ring – IAR) The same repair rules apply as for OAR violations.
    • Minimum edge of drill to copper clearance on inners for drills without copper pad (IPI). Minimum IPI value is set to minimum IAR + 0.075mm for the given pattern class:
    • Violations of IPI clearance on a copper plane are repaired by withdrawing the copper plane with the needed IPI clearance value. Repair is only possible if we do not create open nets in the copper plane. Violations of IPI clearance involving tracks can be repaired by moving the specific track away from the drill provided this is possible and that it does not create any insulation rule violation which is non repairable. Violations of IPI clearance involving pads are not repairable.
    • Minimum copper to edge clearance depending whether the board outline is to be routed or scored (V-cut) .
    • Violations against the edge clearance on a copper plane are repaired by withdrawing the copper plane with the needed edge clearance value, being 0.25mm for routed board outlines and 0.45mm for scored board outlines. Repair is only possible if we do not create open nets in the copper plane. Violations on the edge clearance involving tracks can be repaired by moving the specific track inwards the board provided this is possible and that it does not create any insulation rule violation which is non repairable. Violations on the edge clearance involving pads or drill holes are not repairable.

Move to next stage or raise an exception and halt the job

• If an exception (report of documentation problems) is required make an exception document:
  • summarize all the exceptions points
    • Data missing or unclear
    • Data incorrectly formatted or corrupted in transmission, not defined apertures or 0-size apertures
    • Readability not clear, Job build not clear,outline missing or not clear
    • The provided data do not correspond with the selections made in the order
    • DRC errors that cannot be repaired by us ( see above).
  • propose solutions where possible

• If no exception is required:
  • upload the job onto the system for next stage, single image preparation.
Our data preparation process consists of 3 steps :
  • The first step is the data analysis, what this document is about. Data analysis is performed on all inquiries placed with design files and on all orders. The purpose is to detect if the documentation provided is complete and useful to quote for or accept an order.
  • The second step is the single image preparation. In this stage we are preparing the layout so that it gets fit for production . More info about this stage follows here
  • The third step is the panelizing of different jobs on a production panel – we come back in detail to this later also.

The pictures shown in the articles about data preparation are based on real pcb orders, but have been modified to show specific problems and solutions.