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

• Analysis : we have checked your data to make sure that it complies with the service you have chosen.  If we have found any production issues we have provided you with detailed feedback.
• Single Image : we have rechecked all layers and made them ready for production.

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?

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)

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
• 

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.

New as from 21/02/2012:

New in EAGLE Version 6

In the new EAGLE Version 6 format, the EAGLE brd-file is saved in XML format. Also new in EAGLE version 6 is that the used Design Rules Settings (used DRU-file) are embedded and saved in the EAGLE board file (EAGLE brd-file).

In the previously released EAGLE design rules of Eurocircuits (eC-EAGLE-design-rules-24-06-2011.zip) the DRU file description contained quote-characters (“), which are not supported as such in the XML format.

Using these “old” eC-EAGLE-design-rules in EAGLE Version 6 will lead to errors when trying to load a Version 6 EAGLE brd-file which has been saved with the “old” eC-EAGLE-design-rules. The eC-EAGLE-design-rules have been updated to correct this problem:

ec-eagle-design-rules-14-02-2012.zip

When you downloaded the eC-EAGLE design rules earlier and you did not upgrade to version 6 yet, you do not need to install these new DRU files. When you upgraded to version 6 of EAGLE we advise to use these new design rule files.

Design Rules