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

Eurocircuits Printed circuits blog

What keeps us busy at Eurocircuits, projects we are working at, new idea's, background information and a platform where you can participate, give your opinion and guide us to what is important for you as an electronics developer

Eurocircuits data preparation - Single Image (part II) - other layers and outputs
Post by  luc Smets on 01 Mar 2012  | Posted under PCB data Hits: 19029

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.


Posted under PCB data

Leave your comment

Comments (0)