Note: we run the same data analysis before we make a quotation as well as when we receive an order.
Automatic data input and analysis
We use an automated software program to input your Gerber layout files and Excellon drill files as well as EAGLE BRD files.
The program converts these into our internal front-end engineering format, checks that all layers are present and performs a preliminary analysis to establish the production parameters of the job.
At this stage, our new PCB Visualizer software will allow you to see all layers of your board on screen.
There are other data transfer formats in use (for example, Mentor Graphics/Valor’s ODB++). We prefer Gerber as it is simple, unambiguous, and man-readable.
Read our “Ten rules to provide perfect data for PCB production“. This is a brief overview of how to provide good and clear data. Combine this with logically chosen file names for your Gerber data and you will prevent unnecessary misunderstandings.
Use Extended Gerber (RS274X) with embedded aperture sizes and Excellon drill files with embedded drill diameters wherever possible.
They are faster to process and there is less risk of error. A second useful format is EAGLE 6.x native format.
This is an XML based format that we can transform to our internal CAM-format without having to use the intermediate format Gerber and hence this limits the risk of mistakes.
Why do we change format?
- There is a lot of production information needed for data analysis, tool generation and manufacture which is not included in Gerber or Excellon (for example layer types for automated processing or net-lists for data verification).
- Gerber and Excellon data is supplied in many different versions. Data processing needs a standardised format.
So the more powerful data preparation packages (“CAM systems”) use their own internal data formats. We use Ucamco’s UCAM software with internal format DPF (Dynamic Process Format).
Our engineers complete the analysis, confirm the build for a multilayer, verify the data and raise any questions with the user.
Include clear information in your data package to avoid losing time while we contact you for clarification.
See our White Paper “PCB Design Guidelines” for more information on how to present data most clearly.
All information concerning your design including the build-up should be clear from your digital data to allow automatic data processing. In the event that this is not enough to clarify your design, include a README file in the data package.
This is a clear and simple way to provide information in the order, especially for the board lay-up if the file-naming is ambiguous.
Our engineers check:
- Does the job data match the order details (e.g. has the customer ordered a single circuit but supplied several circuits as a panel, or ordered one top silkscreen but supplied data for top and bottom?).
- Are the layers consistent with each other (e.g. are there drill holes missing from through-hole component pads or vias)
- Is the copper distribution within our manufacturing parameters, especially if the data is a customer-designed panel (more information on this topic).
- Does the design data meet the specifications of the chosen service? A full list of checks is set out in our blog.
Eurocircuits have different specifications for the different pooling and non-pooling services. Other fabricators have similar specifications for different costing bands. Our STANDARD pool and TECH pool specifications correspond pretty well with most fabricators’ standard and tight or high-density capability/costing bands.
Build our DRC minimum values into your CAD system to ensure the most cost-efficient and best-priced design. For EAGLE users we provide sets of DRU files including these values. For Altium users also.
!!! Different minimum track and especially isolation values are required for different copper thicknesses (see PCB Design Guidelines – Classification page). Ensuring a clean etch and good insulation between tracks and pads requires a minimum isolation distance.
This distance depends on the copper thickness. Etching down, even with modern etching systems, also produces some sideways etching into the wall of the track or copper feature.
We compensate for the loss of width by modifying the production films, but there remains an effective minimum gap dependent on the foil thickness. On outer layers when we plate through the holes we also plate 25 – 30 microns of copper onto the tracks and pads, so 18 micron start copper foil will end up +/- 45 microns and 35 micron start copper foil will end up 60 – 65 microns.
This means that in many cases you can use a thinner foil and still achieve the thickness of copper you need, e.g. for current-carrying capacity.
!!! To ensure a robust end product with optimum plating, no drill breakout and, where relevant, good solderability, board manufacturers look for a minimum annular ring of copper around the hole.
To achieve optimum quality we measure this ring 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 Design Guidelines p. 7.
What happens when we find an error in the data (points 1 – 3 above)?
- If the data error means that we cannot complete the analysis, we stop the process immediately and report the data issue to the customer (raise an exception). Typical examples are: no drill data, no board outline, panel instead of single circuit.
- Otherwise we complete the analysis and raise an exception at the end (or for an inquiry, put it in the manufacturability report).
What happens if we find a violation of the service parameters (point 4 above)?
We evaluate the violation to see:
- Can we repair it without affecting the board functionality?
- Would the repairs be better done by the customer on his CAD system? I.e. are there too many repairs needed or are they too complex to carry out as part of normal data preparation.
There is a full list of the checks we run and what we regard as repairable on our blog.
These are Eurocircuits’ repair procedures which we like to make clear to our users. Other fabricators may use different procedures which they may or may not make explicit. If you are concerned that your design may be changed in ways you do not want you should ask what their policies are.
For pooling service orders we make the permitted repairs without further comments. For the rest we halt the job and provide the customer with a detailed report of the issues with screen dumps and advice on possible repairs (raise an exception).
For inquiries and On demand orders we produce a detailed manufacturability report describing the issues and proposing solutions. If the only violations are repairable under our procedures we list what we have done for our customer’s approval.