Prototron Soldermask

Refining Output Data Packages for Fabricators

Bookmark and Share

By Mark Thompson | Published on: March 26, 2018

One of the biggest issues PCB fabricators face is the completeness of the data output package received from customers on a new part. In this column I am going to present what is needed, from a fabricator’s perspective, for a good output package and why.

An Industry-wide Problem

My colleague Dan Beaulieu recently published in his column “The Perfect Customer” that fabrication packages are frequently incomplete, delaying the quote process. This is absolutely a true statement for ALL board fabricators at this time! He pointed out that many larger customers that previously had their own in-house PCB fabrication no longer have that ability, and as such, much of the “tribal” knowledge that was shared between their in-house fabrication and the engineering group in those days has disappeared. So a lot of the board fabrication knowledge has not been passed on to the new generation of engineers and designers. This leads to incomplete or inaccurate output packages that end up having clarification questions prior to quote. Thus, delaying the quote process....

In this column, I will be discussing what files are needed for fabrication and why.

The Basic "Must Haves"

Let’s start with the obvious.

Image Data

The 4 most common and accepted are the following:

  1. ODB ++ (Valor/Frontline’s unique language ) Some of the benefits of outputting ODB++ are:
    1. The IPC net-list is embedded in the data and need not be sent as a separate file.
    2. Fabricators using “Genesis” are looking at a true “apples to apples” comparison; what I see on my screen is the same as what the end user creating the ODB ++ data sees. Odd shaped pads rotated at unusual angles are not always interpreted correctly with some of the older CAM systems, this is not an issue with ODB++ data.
  2. Gerber 274 X ( Gerber data with apertures embedded) this is by far the MOST common output.
  3. Gerber X2 - The newest form of Gerber output- Not all fabricators have the ability to use this type data. Much like the 274 X data has the apertures embedded, the “X2” Gerber’s have additional attributes added.
  4. Gerber 274 D - is one of the older types of Gerber output, this require a separate Aperture file /list or wheel be sent and is a little more cumbersome than “X” type Gerber with the apertures embedded. Providing this type of Gerber data requires that the aperture list be complete or again, you will get a phone call from the fabricator for potential un-assigned D-codes in the wheel/or list

NC Drill Files

This is the file with the Hole sizes, plating status (plated or Not) and the X and Y hole coordinates.

Usable file types for the NC drill file are as follows:

  1. Excellon 1
  2. Excellon 2
  3. An ASCII Text drill file
    1. Please do NOT mix output formats on the NC drill and rout files. Stick with a single convention. Example: 2:4 Trailing zero suppression and Inch units. Do not mix Inch and Metric units on the same file (for instance Inch tool sizes, but metric increments for position or vice versa) Do not mix formats either. (one file output as 2:4 Trailing zero but another in the same output package as 1:5 Leading zero).
    2. If the job has blind vias or epoxy filled vias that are regional (not all one tool size ) please output a separate file denoting just those to be filled. Same goes for any blind or buried vias in the design, output a separate NC drill file for each blind or buried scenario that exists. Example: all tools that will go from layers 1-2 of an 8-layer board can be on the same file but NOT mixed with other blinds or through holes that may be necessary.

Drawings in the form of a DXF, PDF or Gerber

Drawings should include at a minimum:

  1. A Board outline with a dimensioned hole or feature plus overall dimensions.
    1. This is necessary to be able to place the image within the outline file as many times the origins for the output files differ.
  2. Tool chart showing plating status (Plated on non- plated) with tolerances.
  3. Material type.
  4. Solder-mask and ID type and color plus any information about minimum or maximum thickness.
  5. Surface finish type and thickness plus tolerance.
  6. A board stack-up (if either Impedance or dielectrically controlled ) including copper weights for all layers stated as either starting or finished.
  7. Any required testing notes. (standard electrical test, IPC net-list compare, etc.)
  8. Impedance particulars - what width traces are controlled, what layers they reside on plus threshold (50 ohms, 100 ohms, etc.) and tolerance.

Drawing Confusion

Here are some examples of discrepancies or conflicting notes on a drawing that would require clarification:

  • Example 1 : Notes say all inner layers to be half ounce clad but stack up depicting 1-ounce copper internally.
  • Example 2: Notes say all .005 traces on layers 1,3,6 and 8 to be 50 ohms. Gerber image data has no such size being used.
  • Example 3: NC drill file provided does not match the drawing drill table for either hole count, plating status or hole size.

IPC Netlists

Should you have either an AS9102, IPC class 3 6012 multilayer or even just a simple 2-layer board and you want to make sure the files emulate the electrical design parameters...

Please provide an IPC net-list for Net-comparison.

As fabricators we are obligated to run an IPC net-list against your provided Image data for any class 3 6012 or AS9102 parts or any parts that specify a net-list compare to be done on the drawing.

What is an IPC Net List? The IPC net-list is an electrical version of your design parameters to be compared with your exported Image data. It is not a file to be “generated” by a fabricator based on your Image data. If we create a net-list based solely on your Gerber data, at NO point would we ever find a mismatch, which may result in boards successfully being built, tested and shipped that are nonfunctional.

Care should be taken to not assign net-points to things that should not be electrical nets, things such as Non-plated holes or targets.

Before any fabrication edits have been performed, a Net-list compare is done. Any known or otherwise intentional shorts or opens should be noted on a “read –me” file word doc or on the drawing itself. Example: “AGND to DGND short net000 is intentional by design”

Then after any manufacturing edits such as drill compensations or etch compensations are performed the net-list is again ran to ensure the fabricators has not created any electrical anomalies. Some of the most common net list types for fabrication are IPC D356, IPC D356A or a mentor neutral file.

Lastly, any specific panelization requirements such as the addition of text for part marking, fiducials of a specific size or sub panel tooling of a specific size should be negotiated with the fabricator prior to quote. If no sub-panel drawing can be provided, you will want to, at the very least, indicate to a board fabricator areas of either part overhang or feature proximity where you DO NOT wish frame tabs to exist. This will minimize having to go back into CAM to move tabs or add cutouts in the frame.

Conclusion

PCB fabricators are an extension of their customers, and for this relationship to be successful both sides need to work collaboratively, and it all starts with the output package. Following these guidelines is the critical first step to assuring product quality and reliability.

As I've said before, your best bet is to communicate with your fabricator early on.

Contact

Redmond Facility
15225 NE 95th Street
Redmond, WA 98052

Toll: 888.847.7686
Phone: 425.823.7000
Fax: 425.869.2515
email: Info@Prototron.com

Tucson Facility
3760 E. 43rd Place
Tucson, AZ 85713

Toll: 800.279.5572
Phone: 520.745.8515
Fax: 520.747.8334
email: Info@PrototronSW.com

Newsletter Signup

Sign up to stay in touch!

Sign-up