Fresh PCB Concepts: 7 Options for Via Treatment

NCAB-JeffBeauchamp.jpgMany times, I come across a PCB design with via holes that are completely exposed. In some cases, this is acceptable. But there are many other times when I recommend that the hole either be covered and/or tented. But in most cases, I recommend they be plugged.

For example, here are several advantages of via hole plugging:

  • Prevents residues becoming trapped in the holes, preventing corrosion
  • Prevents air leakage during ICT
  • Prevents solder balling
  • Prevents solder paste loss (solder migration)
  • Prevents contamination entrapment under components
  • Prevents migration of adhesives and conformal coatings used during assembly

But before getting into options for via treatment, I want to talk about the term “tenting.” This term is a bit antiquated and refers to dry film solder mask that has fallen to the current liquid photoimagable (LPI) solder mask. In days past, the dry film would cover over the hole without opening and form a “tent.” With LPI mask, the effect is essentially lost, and the liquid will fall into the barrel of the hole. Some of the intended effects remain, but the overall encapsulation is not quite the same.

Now, let’s consider IPC-4761 (design guide for protection of printed board via structures). There are seven different via hole protection types in IPC-4761 (classified as Types I–VII). Some of these types are recommended while others are not, and others are necessary for certain technologies.

Type I: Tented Via Holes

Type I is split into two categories: Type Ia (single-sided) and Type Ib (both sides). Single-sided is not recommended by IPC. In Type I, there is no solder mask opening over the via hole, so it will not be developed away. The aim is to apply solder mask over the via hole, effectively tenting it. However, there is a risk with this option. The tent can break down on one or both sides, leading to entrapment of chemistry or even solder. I personally do not recommend Type I for immersion tin finish due to the risks of solution entrapment and risk of copper corrosion.

Type II: Tented and Covered Via Holes

This type of via plugging is also split into two categories: Type IIa (single-sided) and Type IIb (both sides). Type II is very similar to Type I with a secondary covering of mask applied over the via hole. Again the single-sided version (Type IIa) is not recommended. Even with the secondary coat, similar concerns apply when compared to Type I, and with this type, there is a concern of increased processing/mask height over the via hole, thus causing concerns for stencil applications. Again, I do not recommend this type for immersion tin finish for the same reasons, including risks of solution entrapment and risk of copper corrosion. In addition, I do not recommend this type of plug be used within a footprint of a BGA due to the potential for elevation over the pad surface.

Type III: Plugged Via Holes

Again, this via is split into two categories: Type IIIa (single-sided) and Type IIIb (both sides). Single-sided is also not recommended by IPC. With Type III, a material is applied, allowing for partial penetration into the via. This may be applied from one or both sides; however, as this is not filling the hole, there is no guarantee the hole will be “blocked.” As with the previous types I mentioned, this can lead to exposed copper in the holes, and air entrapment can cause blow out of the partially plugged hole. And I do not recommend it for immersion tin finish due to the risks of solution entrapment and risk of copper corrosion.

Type IV: Plugged and Covered Via Holes

Split into two categories—Type IVa (single-sided) and Type IVb (both sides)—this method is the same as Type III with additional mask applied over the top. Single-sided is, again, not recommended by IPC. The same concerns apply as with the previous types I described, as well as I do not recommend this for immersion tin finish due to the risks of solution entrapment and risk of copper corrosion (Figure 1).

NCAB_Figure_1-0620.jpg
Figure 1: An example showing the potential result of single-sided plug/single-sided tent (Type I–Type IV) with immersion tin surface finish, where the chemistry becomes entrapped and corrodes the copper within the hole. This can be resolved through moving to either type VI via plugging (preventing chemical entrapment) or leaving the hole open (allowing for adequate rinsing/solution flow).

Type V: Filled Via Holes

This is a via hole with material applied into the via, targeting a full penetration of the via hole with full encapsulation. This provides a complete fill of non-conductive (or conductive) material that will eliminate contaminants remaining in the hole.

Type VI: Filled and Covered Via Holes

This is the same as a Type V via hole (full penetration of material into the hole) with an additional covering of solder mask applied over the via hole and pad (Figures 2 and 3). The solder mask may be applied to one or both sides, depending on design needs. When both pads are covered, this offers superior protection of the full hole/pad. Again, with this approach, there is a complete fill within and over the via hole that, therefore, eliminates the concerns previously mentioned (contaminants, chemical residue entrapment, risk of blow out, eliminate paste loss, etc.).

NCAB_Figure_2-0620.jpg
Figure 2: The target is to achieve a complete fill; however, knowing production and process tolerances, we accept a minimum of 70% fill. To achieve the desired results of preventing any residues or chemicals in the hole, we always recommend filling to at least 70%.

NCAB_Figure_3-0620.jpg
Figure 3: With Type VI via hole plugging, we fill the hole from one side to the other, using a stencil and a screen printing process, before we apply solder mask to the surface of the panel.

Type VII: Filled and Capped Via Holes

This is the same as a Type VI via hole with a secondary metalized coating (copper) applied over the top of the via hole on both sides. This is normally used for such applications as via in pad or in BGA applications where high-density features are required. In this case, it is typical that a special resin is used to plug the via to minimize the risk of air bubbles or voids and also prevent expansion due to thermal excursions. Highly specialized equipment is also required to ensure the resin is adequately drawn into the via and eliminate voiding. While many fabricators say they can do this type of via treatment, we have seen that without the specialized equipment to support, quality becomes sacrificed (Figure 4).

NCAB_Figure_4.jpg
Figure 4: A physical board example of a Type VII filled and capped via hole normally used for such applications as via in pad or in BGA applications where high-density features are required.

My Recommendations

I recommend you consult with your PCB supplier with all your PCB designs, particularly when the design is more complex. With many options for treating the vias, it is important to have an open discussion with your fabricator. Clearly explaining why you need a via treatment and what factors are and are not desirable will ensure the best option is used and that it is compatible with other factors in your design.

Jeff Beauchamp is a field application engineer at NCAB Group.

Back

2020

Fresh PCB Concepts: 7 Options for Via Treatment

06-18-2020

In some cases, it's acceptable to have via holes that are completely exposed in a PCB design. But there are many others where the hole should either be covered and/or tented, or in most cases, plugged. Jeffrey Beauchamp shares seven different via hole protection types based on IPC-4761.

View Story

Fresh PCB Concepts: Why Design and Produce PCBs Beyond Industry Specification?

05-07-2020

While questions may be an annoyance, especially when you finally have a board designed and are ready to have it built for a product, Ruben Contreras explains the importance of asking these questions and requiring specifications.

View Story

Fresh PCB Concepts: What You Should Know About Your Board’s Solder Mask

04-09-2020

It’s a weird time we’re all in, and for most designers, work has slowed down or even stopped. While work might have slowed, now is a good time to review some of your past PCB projects to see if you can improve functionality and reduce field failures. Harry Kennedy explains how one of the simplest ways to do that is to start from the top: solder mask.

View Story

Fresh PCB Concepts: The Benefits of Being a PCB Producer Without Owning Any Factories

03-19-2020

With NCAB's infrastructure and factory management team based in China, many customers ask why they don’t own any factories. Jeffrey Beauchamp explains how it's part of the company's long-term strategy and an advantage to our customers that they don’t own any factories. Instead, they “own” what is most important: the relationship with the factory.

View Story

Fresh PCB Concepts: Controlled Impedance—Design to Testing

02-12-2020

Ruben Contreras often gets questions from customers on one of his favorite subjects in PCB design: controlled impedance. Ruben explains how controlled impedance is a science, which is why he likes it; therefore, it must be designed and tested comprehensively.

View Story

Fresh PCB Concepts: Create PCB Fabrication Notes for Success

01-09-2020

When NCAB Group receives Gerber files for an order, there are times Harry Kennedy cringes because there are missing pieces of information necessary to make sure the PCB is made with zero defects. As we come back to work for the New Year, Harry shares some key factors he wishes customers would consider before they send their files.

View Story
Back

2019

Fresh PCB Concepts: Designing a PCB for Telecom Applications

12-12-2019

Jeff Beauchamp and Harry Kennedy discuss PCBs for telecommunication applications, including key factors to consider, such as design and material considerations. They also recommend involving your PCB supplier at the time of design to help ensure manufacturability at the lowest possible cost.

View Story

Fresh PCB Concepts: The Current Material Situation

11-11-2019

We have all heard about the component crisis in the circuit board industry, and maybe you heard about the CCL shortage, but how many are aware of the bare board material shortage? Ruben Contreras explains the current material situation and tips to address this issue.

View Story

Fresh PCB Concepts: Getting It Right From the Start

10-23-2019

When faced with critical time-to-market situations, it is all too easy to say, “It doesn’t matter because this is just the prototype; we can fix this later.” However, if the design is perfected from the beginning, cost savings can be applied, and manufacturability can be ensured. Perhaps most importantly, the design can be adapted with reliability in mind, leaving a seamless transition from prototype to production. How do we get it right from the start?

View Story

Fresh PCB Concepts: Why Material Selection Matters

10-02-2019

When you’re designing a PCB, it’s standard to call out FR-4 material, but you could be holding yourself back or even exposing your board to risk by not knowing more about PCB materials. Let’s take a small look into why. What Is FR-4, exactly? Harry Kennedy of NCAB explains.

View Story

Fresh PCB Concepts: Qualities of Medically Applied PCBs

08-26-2019

In this inaugural column from NCAB Group, Alifiya Arastu discusses details of PCBs used in medical applications, highlighting some of the differences in terms of demands and how the design must be handled.

View Story
Copyright © 2020 I-Connect007. All rights reserved.