Arguments For and Against Non-Functional Pads

Inside the PCB in the above image, there is a group of pads attached to the signal vias, known as non-functional pads (NFPs). NFPs provide some advantages in specific cases, while in other instances there are good arguments to remove them. The inclusion or exclusion of NFPs is a long-standing debate, and some designers like to make blanket statements regarding the removal of these pads.

So to help clear things up, we're going to outline some of the best reasons to keep and remove NFPs. What we’ll find by the end of this article is that the removal of NFPs should be targeted to certain cases. In some instances, the presence or absence of NFPs should be simulated in order to verify the design will function as intended.

Why to Keep Non-Functional Pads

Greater Adhesion on Through-Hole Pads

Through-hole components require that solder infiltrate the entirety of the through-hole pad, and this causes the internal copper to heat up. Keeping the non-functional pads on these through-holes will help prevent pull-away from the PCB material on the internal layers. To ensure additional reliability, soldering can be temperature-regulated with thermal relief connections back to any internally connected plane layers.

This through-hole connector takes advantage of internal NFPs to anchor copper to the PCB.

Reduced Thermal Cycle Failure in High Layer Counts

There is some evidence that keeping NFPs, at least on some of the internal layers, will reduce failure from thermal cycling. Due to CTE mismatch between copper and PCB materials, the copper features will become stressed if the PCB heats up. The presence of NFPs holds the via wall in place and helps distribute stress along a via barrel. When the space between NFPs becomes too large, there is greater potential for stress concentration and eventually fatigue failure.

Why to Remove Non-Functional Pads

Tool Wear During Drilling

One area that PCB manufacturers might complain about is tool wear from drilling NFPs. When a PCB is fabricated, any NFPs in the internal layers will be undrilled until the layer stackup has been pressed. Once drilling begins, it will have to drill through each NFP in order to form through-holes. A drill will need to pass through each NFP, which speeds up tool wear. In prototyping, this does not matter due to the low volume of drilling. In high volume, tool wear adds up, so removal of NFPs offers an opportunity for cost reduction.

Clearances Cut Up Plane Layers

Whenever a via passes through a plane layer, there must be some allowance for clearance between the via and the copper plane. The same applies to copper pour. When these are not densely placed, the clearance does not remove a large amount of copper from the plane. However, if you look under a BGA, the clearance to an NFP creates a large anti-pad, and this might not leave very much copper in the plane.

When vias get too close, the clearance rule around NFPs can cut out portions of the plane.

In the internal layers below a BGA passing into a plane layer, it may be best to remove the NFPs, at least in the plane layer. This helps keep uniform ground and sufficiently large power rails in the power layer to the greatest extent possible.

Additional Space for Routing

Another reason to remove NFPs is to allow more space for routing. NFPs take up space between vias, and if these are densely spaced it could be difficult to get many signals between vias. Selective removal of NFPs on certain vias can allow more space for trace routing. This might even be recommended on BGAs so that you can complete fanout routing into the internal layers.

Clearance rules can limit where you can route when non-functional pads are present.

Signal Integrity

One of the most common reasons people think they need to remove NFPs is for signal integrity. This only starts to matter in the GHz range, and the effects will not be noticeable on most digital signals or RF signals. The removal of NFPs for signal integrity reasons should always be simulated using a 3D electromagnetic field solver. You may find that the NFP actually helps in the inductive range of via impedance, especially when the anti-pad ends up being a bit large.

Summary

Obviously, there are many situations where removal of NFPs provides mixed benefits. From the above points, it should be clear that the best approach for dealing with NFPs is to remove them selectively. Rather than examining each via individually, there are a few areas where you can look to remove NFPs:

• On high speed or high frequency traces that require vias

• Below a BGA as part of fanout routing

• On high layer count boards being produced at volume as a cost reduction opportunity

If you want to eliminate NFPs on select through-holes, make sure you have CAD tools that make it easy. Multi-disciplined design teams rely on the best set of PCB design features in Allegro PCB Designer from Cadence. Only Cadence offers a comprehensive set of circuit, IC, and PCB design tools for any application and any level of complexity.

Subscribe to our newsletter for the latest updates. If you’re looking to learn more about how Cadence has the solution for you, talk to our team of experts.