8
\$\begingroup\$

My PCB layout package (Altium) has an option to define the full stack of a via so one may have different sized annular rings on different layers.

I was wondering if it is considered "manufacturable" if a via has annular rings only on layers where it connects to other copper. On layers without connection (passthrough), may have no annular ring, just the plated hole. I understand this this is more of a question for a board house, but i was wondering what the general opinion on this is.

The motivation behind this question is that in very high density designs, it may be critical to have less clearance on an internal GND plane for example. The lack of the annular ring would be of great benefit as it would reduce the area the via needs to pass hough the internal GND plane.

Thanks in advance.

\$\endgroup\$
2
\$\begingroup\$

Removing non functional inner pads should lead to a more reliable plated through hole via. Some people might also say it reduces drill wear for your mfg but the primary reason is long term reliability especially under thermal stress.

\$\endgroup\$
  • 1
    \$\begingroup\$ To add to this, PCB stresses that lead to annular ring cracking can compromise the via "tunnel". Without inner rings the via is less rigidly attatched to the pcb \$\endgroup\$ – crasic Aug 24 '15 at 18:21
6
\$\begingroup\$

1) There is no consensus on whether non-functional pads (NFPs) should be kept or removed.

2) Usually NFPs are removed by board manufacturers either with or without consent of the customer.

3) The primary reason why NFPs are removed is to reduce wear of drill bits.

4) There are claims that NFPs reduce Z-axis thermal expansion. However, my understanding, that these claims lack sufficient amount of research and may not address the modern materials used for board manufacturing.

5) In high speed designs NFPs should be removed as they decrease insertion loss of a via.

6) If NFPs are retained a condition called "telegraphing" may occur

"where there is so much copper at PTHs the material is "resin starved" between pads and you can see the image of this "pancake stack "of copper in the dielectric; the image is "telegraphed" to the surface. When the dielectric is thin and the copper thick, the condition is exacerbated and reliability is significantly reduced."

7) There are reports that NFPs may increase vias' life if aspect ratio is low ("wide" via), but decrease vias' life if aspect ratio is high ("small" via, usually found in multi-layer, relatively thick boards).

Below is the abstract from the excellent research "Non-function pads: should they stay or should they go" performed by DFR Solutions :

There is an ongoing debate regarding the influence of non-functional pads (NFPs) on printed board (PB) reliability, especially as related to barrel fatigue on plated through vias with high aspect ratios. To gather common practices and reliability data, industry experts were surveyed. The overwhelming response indicated that most suppliers do remove unused / non-functional pads. No adverse reliability information was noted with respect to the removal of unused pads; conversely, leaving them can lead to an issue called telegraphing. In all responses, remove or keep NFPs, the primary reason given was to improve the respective fabricators’ processes and yields. Companies that remove the unused pads do so primarily to extend drill bit life and produce better vias in the boards, which they considered the primary reliability issue. For those that keep the unused pads, the primary reason given is that they believe it helps manage Z-axis expansion of the board due to Coefficient of Thermal Expansion (CTE) stresses. However, with the newer materials being utilized for Pb-free assembly, the Z-axis CTE concern seems to have abated. In general, the companies responding did not feel that removing the unused pads would create a reliability issue. All suppliers said that their response was the same regardless of whether polyimide glass or epoxy glass materials were involved.

URL1, URL2

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.