Engineering Spotlight: Net-Lists and Net-List Generation

By Mark Thompson | Published on June 28, 2009 - 10:00 AM PST

Netlist - US Patent 5933356 Reference

What is a net-list used for in a fabrication environment?

A net-list compare is required for IPC Class 3 6012 jobs and any other job that the customer has supplied a net-list on, typically the net lists are IPCD356, IPCD356A or some other ASCII type file such as a mentor neutral file. The purpose of the net-list is to verify the design criteria against the output Gerber files to make sure there are no differences between the desired design and the generated Gerber files. Many times over the years we here at Prototron have been asked to Generate a net-list file from the provided Gerber’s. This is NOT a comparison. If we generate a net-list based upon the provided Gerber’s, at no time will there EVER be a miss-match. The more complex the design is, the more a net-list really should be provided to verify the Gerber output files against the design. Does this mean that if you provide a net-list and it is created at the same time as the Gerber files that you will be guaranteed to not have any inconsistencies? Not at all. The net-list itself can have definition issues that can arise, such as tooling holes also used as grounding screws in the final application can come up in an analysis as “broken” or open nets.

Depending upon how the net-list was generated. The same can be said for edge connection type features where plated half holes or slots make a physical connection in the final application.

A very common INTENTIONAL mismatch is a net-list short from Analog ground to digital Ground, typically described right at the beginning of the net-list, net 0 or net 1. It is ALWAYS helpful when a known anomaly exists on the net-list, that it be communicated via a read-me or some other note so that the job does not go on hold and lose time for no reason. Something as simple as a note saying , “Shorted net at AGND/DGND is intentional.”

Also, Many times erroneous net-list issues occur when there is a difference in the ROTATION of a given feature in either the Gerber files or the net-list itself, An example of this can be surface mount points rotated 45 degrees on the Gerber files and a net-list that is describing them either vertically or horizontally, in some cases creating erroneous “shorts” if there is copper pour close on the Gerber data. The Net-list showing the mounts are horizontally aligned and the Gerber’s showing them at 45 degrees overlapping them and creating the erroneous “shorts”.

What’s the difference between a “1 up compare” and Net-list compare?

A Net-list compare is again the comparison between the provided Gerber data PRIOR to any manufacturing edits and the provided IPC 356 Design net-list. A “1 up compare” is done after manufacturing edits are performed at CAM stage to ensure that no edits performed have the changed the electrical functionality of the boards. This ensures that we the Fabricator have not changed the electrical functionality of the boards by bridging features due to an etch compensation for instance. If I have not mentioned it before, the “Etch compensation” is done in Fabrication at the CAM stage. Generally speaking, for every half ounce of starting copper a half mil of etch compensation is associated. So that after etch your desired line size is maintained.

Getting back to why I brought up the difference between a CAM 1 up compare and a net list compare. Many times there will be a drawing or read me callout for net-list compare and when a net-list file is not provided and the customer is contacted they indicate they merely wanted a 1 up compare to make sure WE have not changed the function of the part by our manufacturing edits. Sometimes our customers will ask for Test based upon the provided net-list list files. Test file generators for modern test machines generally use the customer Gerber files for Test point Generation and NOT the customer supplied IPC net-lists. Having said that, the requirement is still being met as in Both CAM and then again when the TEST files are generated a net-list comparison between the Gerber files and the provided IPC net-list is performed and any mismatches communicated to the customer.

Thank you for your time.
Please feel free to call me with any questions or comments at:

(425) 823-7000 extension 239
or E-Mail me at MarkT@Prototron.com