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.