The PCB Norsemen: So Much More Than Just Through Vias

john_johnsen.jpgAs most people know, component holes are still highly necessary for components that require them, and clean lead-through-holes (vias) have increased in necessity over the last 30 years. They have dominated the types of holes used in a PCB. The diameter of vias has gone one way, and the complexity around via holes has generally increased.

With a continuous component hole, copper plating is not a problem; however, it requires good process control. The challenges with smaller diameter vias, perhaps depth-controlled, have increased and are, in some cases, challenging for those who produce PCBs and have to assemble and handle solder components.

Via Types
Via holes in the PCB are highly necessary to be able to carry out the number of connections required. In general, the via holes of today can be briefly summarized as follows:

  • Through: Mechanically drilled holes
  • Blind: Mechanical depth-controlled drilled holes
  • Blind: Laser vias
  • Buried: Mechanically drilled vias
  • Buried: Laser vias
  • Back-drilled via holes
  • Half/castellated holes

In addition, laser vias may be stacked or staggered relative to each other, and they may also be stacked or staggered relative to a buried mechanical hole.

Furthermore, laser vias, blind, and mechanically drilled through-holes can be placed in component pads (SMD pads), which requires special treatment.

Filling Vias
Laser vias can be copper-filled or filled with resin. If they just act as fan-out vias, they are simply covered with the solder mask used. When filled with resin, they can also be capped with copper, and then components can be mounted and soldered directly on them. Copper-filled laser vias is the latest method used, but both methods are still very relevant.

PCB manufacturers operate with their own capability in terms of diameter, aspect ratio (AR), and pad diameter requirements on the various hole variants. The problems related to production are mostly the same with all manufacturers, but processes, equipment, technologies, etc., are the reason for PCB manufacturers to have a difference in capacity and capability. This is also reflected in the fact that some PCB manufacturers have specialized in prototypes and small, fast deliveries, while others are specialists in high volumes.

Considerations for Designers
It is essential that designers become familiar with the production processes so they can understand what is possible and not possible to produce. Some who were not aware previously operated with a through-hole diameter of 0.1 mm on 2-mm thick PCB. Fortunately, there are not many left, but some are still out there.

For a PCB to be produced with a good result, it is important to provide the designer with this information on capability and design rules. However, the designer must also be obliged to obtain the necessary information before starting a layout. This is absolutely essential for a good result.
As a designer, you must have access to the current IPC standards that the world's manufacturers adhere to—typically, IPC-6012, IPC-6013, and IPC-A600. However, the designer must also clarify what is available in relation to the type of PCB that is to be realized. I have mentioned in previous columns how important this is, as the cost of redesign due to lack of knowledge about the rules that apply is not something you want to cover.

Laser Vias Used in HDI PCBs
HDI PCBs are an increasingly integral part of the PCB and electronics industry in general. Electronic components are getting smaller and lighter but still require high performance. To meet this, you also need to pack more functionality in a smaller area with HDI PCBs.

HDI PCBs have a higher circuit density per unit than conventional PCBs. They use a combination of buried and blind vias, as well as laser vias. Those that are ≤0.15 mm in diameter are also called microvias (mVias).

Any Layer HDI, ELIC, and ALIVH
High-density PCBs have a combination of different vias, as compared to others that only have laser vias and tend to be called any layer HDI. Other names are every layer interconnect (ELIC) HDI and any layer interstitial via hole (ALIVH).

The maximum number of layers with this technology I have seen is 14 layers. Then, you have a finished PCB with stacked laser vias and a maximum thickness of around 1 mm. This anonymous stackup is one I have worked on, but I do not have permission to show this stackup, so Figure 1 and Table 1 show an equivalent of eight layers and is about 0.6-mm thick.


The most common combination of vias in an HDI PCB is 1–3 sets of laser vias per side, in combination with mechanically drilled buried vias. Through-holes are for components that require this, as well as unplated holes.

Via holes that go from top to bottom have been replaced with the combination of laser and buried holes already defined. This avoids a potential overplating of the outer layers as a result of a longer plating time in order to obtain a solid copper plating in small via holes with a high AR.

Three Variations of Laser Vias With Different Combinations
Figures 2 a, b, and c show some combinations. For all three combinations, laser vias on the top (layers 1–2) and bottom (layers 14–13) are copper filled as they are placed in the SMD component pad; thus, they are soldered. Figure 2a is the least challenging in terms of copper plating and also the most reliable and lowest cost to produce.

Laser vias on layers 2, 3, 12, and 13 are staggered and filled with resin after electroless copper, electrolytic copper plating, and etching. The same goes for the buried hole layers 3–12, often filled with epoxy.

In Figure 2b, all laser vias are filled with copper and stacked on top of each other. There is a cost for copper filling of the inner laser vias, and the reliability of stacked vias is lower than in Figure 2a where they are staggered. The big change in Figure 2c, compared to 2b, is that laser vias are stacked on the buried hole (layers 4–11). The buried hole is now also clad with copper to secure the connection to the laser via, which is placed directly on top.

Of the three examples, Figure 2c has the highest cost and is also less reliable than Figures 2a and 2b. The lower reliability in Figures 2b and 2c is based on a potential expansion of the material in stackup that may affect the connection between the vias that are directly connected to each other. In certain cases, electrical properties must be prioritized, and lack of space can also be the reason why an extended stacked vias solution is chosen.


In certain situations, there may be up to three copper platings on some layers. This is related to conditions such as copper filling of laser vias, overplating of mechanically drilled vias, and the plating of through-holes. This can create challenges for the subsequent etching of narrow conductors, which is a concern with HDI PCBs today.

 IPC Standards

The amount of copper plated in the various holes is, in most cases, specified in IPC standards that PCB manufacturers and end customers adhere to. You get a full overview—including the complete standards, tables, and illustrations—on IPC’s website, but here are some values from IPC-6012E.


How to Avoid Layout Rejections
Every week, we receive many layouts that are rejected long before they end up in PCB production. The main reason is that they contain design issues that have not been clarified with the PCB manufacturer before the design begins, or the design is not in accordance with IPC requirements.

Typical conditions are:

  1. There is too great a distance between the layers where laser vias are used.
  2. The copper is too thick in relation to the conductor widths to be etched and the distance between them.
  3. The designer has not calculated that inner layers can also be plated when laser vias and buried holes are used.
  4. The AR is incorrect, which especially applies to smaller drilled holes. The recommended
    maximum AR is 8:1 on buried and through-drilled holes. Laser vias have a recommended maximum AR of 0.8:1.
  5. There is a misunderstanding of the use of laser vias, often defined as through-holes with a 0.1-mm diameter.

Resolving the Layout and Making It Producible
In these cases, we open a dialogue with the designer and give them an introduction and recommendation on how their design can be made producible. Vias plays an important role in a PCB as signal speeds increase. A PCB designer must be able to handle this. In general, we can say that vias constitute a discontinuity in the transition from a conductor and will affect the signal in designs with high-signal speeds.

Capacitance can increase rise time, which reduces speed. Therefore, designers must ensure a good impedance transition. The larger the pad diameter, the lower the impedance due to the increased capacitance. By removing non-functional via pads on the inner layer, the capacitance can be reduced.

A dangling via stub acts as an open resonator. When using laser vias, we have no stub. On traditional drilled vias, a stub can be removed with back-drilling.

Drilled Via Hole Reliability
The reliability of drilled via holes is affected by several parameters:

  1. A reduction in the length of the hole will make the hole more reliable, which can be done by reducing the total PCB thickness or reducing the length of a buried hole.
  2. An increase in the diameter of the hole can also provide increased reliability, but this is typically a non-option due to lack of space. For example, 0.2–0.25 mm can provide increased reliability.
  3. The choice of material—especially the coefficient of thermal expansion (CTEz) and elastic modulus or stiffness (Ez)—also contributes to increased reliability, but Ez is not mentioned on all datasheets.

In materials, there is a different mix of glass and resin. Previously, it has been the practice that the properties for laminate and prepreg stated in the datasheet are for the type with the thickest glass, type 7628, but this is now beginning to be nuanced a little more. This is good because, typically, the most advanced PCBs use prepreg with the lowest glass content—glass styles 106 and 1080.

The CTEz expressed in ppm is approximately 25% higher for a 106 (thinnest) prepreg than for a 7628 (thickest). For Ez, which is measured in megapascal (MPa), then the typical value for 106 prepreg is around 4300; for 7628 prepreg, it is approximately 5,800. Resin content in a 106 prepreg can be well over 70%, while in 7628, it is down in the range of 42%.

For an EMS or others who will assemble components and solder them, it is important that they also understand a stackup and know what challenges they may have to solve. I am thinking in particular that a number of copper-filled buried vias directly into BGA footprint is something that they should know about, and it will help them determine a good soldering profile.

Early Involvement, Lower Cost
I have been in the industry of printed circuits for ages and deal with layouts and PCB design every day. Vias play an important part of the PCB, so it's important to know what they are, how they work, and how to solve any challenges involving them. My job is to advise on design, solve EQs, and ensure all parameters are covered early in the design process. The earlier we talk and discuss, the fewer the mistakes and the lower the cost for avoiding expensive redesign.

Here are the top five things to remember about vias:

  1. Be sure to stay updated with the latest IPC standards relevant for your design and need.
  2. Make sure you have the AR in place.
  3. Make sure the pad diameter is sufficient. Remember that the unprocessed hole is drilled around 0.1 mm larger than the nominal diameter. For laser vias, the unprocessed hole is
  4. Use stacked laser vias only if needed. Otherwise, they should be staggered.
  5. Only use stacked laser vias on top of buried holes when needed.

The last advice from me might sound simple but it’s crucial: It is important that you discuss design requirements with your PCB supplier and make sure that you understand each other and agree on the way forward.

This column originally appeared in the November 2020 issue of PCB007 Magazine.



The PCB Norsemen: So Much More Than Just Through Vias


As most people know, component holes are still highly necessary for components that require them, and clean lead-through-holes (vias) have increased in necessity over the last 30 years. John Steinar Johnsen explains how the challenges with smaller diameter vias, perhaps depth-controlled, have increased and are, in some cases, challenging for those who produce PCBs and have to assemble and handle solder components.

View Story

The PCB Norsemen: A Path to Successful PCB Fabrication


In the PCB fabrication process, there can be multiple actors involved. How can you ensure that all these actors are cooperating to maximize the positive effects and minimize the negative effects of the pillars of PCB fabrication? It might sound like an insurmountable task, but Didrik Bech shares a path that can increase your chances of success.

View Story

The PCB Norsemen: Leadership Styles for Success


Leadership is the foundation of a successful business. Elmatica CEO Didrik Bech looks deeper into the various styles of leadership and shares his experiences and opinions.

View Story

PCB Norsemen: The Importance of Quality Management


Most companies have a quality management system, but the important factor is not if you have one; it's about how that system is implemented in your company's values, strategies, and goals. Didrik Bech explains how you can use your QMS as a competitive advantage and shares five top reasons for having one.

View Story

The PCB Norsemen: It’s All About Being Prepared


COVID-19, known globally by now, and buzzwords like social distancing, isolation, home office, antibac, and lockdowns, are humming in every ear. Raymond Goh explores how this will impact the electronics industry and how to respond. Humans tend to stick to habits. Will the same happen to PCB production?

View Story

The PCB Norsemen: Can Better Guidelines on Cosmetic Failures ‘Save’ Functioning PCBs?


Every year, fully functional PCBs are scrapped due to cosmetic “failures” that are not approved. Is this right, or do we need to make an even more precise set of rules on how to handle this? Jan Pedersen shares his thoughts on the issue.

View Story

The PCB Norsemen: What Are the True Benefits of Going Digital?


2019 might have been the year when the trend word digitalization really kicked off and transitioned from being a buzzword to aligning with keywords and concepts as AI and IoT. Didrick Bech explores the future of digitization, which is already here.

View Story

The PCB Norsemen: Automotive Standard Elevates the Excellence of Electronics


IPC-6012DA (currently in WAM1) was the first automotive standard for printed boards; it also needs to expand to cover all types of rigid printed boards. To meet the PCB needs in the automotive industry of today and tomorrow, we have started to collect information and identify the types of printed boards not covered by the existing standard. One finding in the research is printed boards used for LED headlights and taillights, which have two requirements not covered; these are described as metal-core printed boards and high-power printed boards.

View Story

The PCB Norsemen: New Trends in the PCB Industry at productronica 2019


Working with PCB technology and standardization as I do, it is always interesting to see the new trends and where the PCB industry is moving. Changes tend to happen at a slow pace; still, I visited productronica this year for dedicated meetings and expected to learn about new processes and production equipment. What hit me was the different manufacturing focus between Asia and Europe. 5G applications and smartphones—both making an impact in the news as a high focus in Asia, where most of the production is placed—were hardly mentioned at productronica 2019. However, I picked up on other new trends in the PCB industry.

View Story


The Laminate Market: What Will the Future Bring?


PCBs have been manufactured more or less the same way since we entered the industry in 1972, but the circumstances surrounding the boards have changed. The PCB Norsemen have addressed the copper situation several times in our columns as well as the component crisis affecting the PCB industry. Now, we’re experiencing external factors—such as Brexit and the trade restrictions between China and the U.S.—that are affecting the industry and causing delays due to raw material demand and prioritization by huge market players.

View Story

The PCB Norsemen: Avoid Failures in PCB Production With Compliance Control


Failures and reliability in the printed circuit industry are usually considered in the context of quality claims and non-conformity. This is a logical approach; however, there is a new context where these aspects are under close scrutiny, namely compliance—especially in the defense industry. Failing to understand import and export compliance for every country you deliver to and from will, at some point, result in challenges in your supply chain with potentially severe ramifications.

View Story

The PCB Norsemen: From Wooden Huts to Homemade Go-karts—It All Starts With Design!


Whether building the coolest go-kart or the most sophisticated electronic hardware, the story is the same: It starts with design. And for designers and manufacturers, early involvement and commitment between all the involved parties in a product development process diminish the risk for mistakes and misunderstandings.

View Story

What Is Reliability Without Traceability?


High reliability and compliance are hot topics at conferences all over the world. If you are a supplier to industries like defense, automotive, medical, and aerospace/space, high-reliability and regulatory compliance are strict demands for electronic device manufacturers. This column discusses how high-reliability demands enforce the need for traceability, and at what level the traceability should be.

View Story

The PCB Norsemen: Merging the Best of Both Worlds—Young Superheroes and Knowledgeable Wizards!


Companies that dare be true to themselves, trust their employees, and provide direction, freedom, and responsibility to their most important asset—namely, their employees—are more likely to succeed. However, we can all rattle behind these positive words and agree with these statements. The real question is, “How do you actually create and sustain an environment that motivates and attracts people—especially millennials—in the wave of Industry 4.0?"

View Story

The PCB Norsemen: My Flexible Story—Flex Circuit Development Through the Decades


Senior Technical Advisor Jan Pedersen is celebrating 26 years at Elmatica. In this column, he shares his thoughts from his long experience in this exciting industry, and talks about those things that have changed a lot in the past few decades, and the others that haven't.

View Story

A PCB Broker’s Guide Through the Galaxy of Automation


A smart factory is defined by its ability to harness manufacturing data flowing throughout the enterprise and then convert that data into intelligent information that can be used to create improvements in productivity, efficiency, savings, yields, automation, enabled traceability, compliance, and reduced risk of errors and rework. All of these items are crucial factors when manufacturing printed circuits.

View Story

The PCB Norsemen: Technology’s Future Comes Together—A Great Slogan for Us All!


“Technology’s Future Comes Together” was the theme of this year's IPC APEX EXPO, which is quite suitable during these changing times. I guess we all need to come together, especially the automotive industry.

View Story

The PCB Norsemen: PCB Standards for Medical Device Applications—A Hard Nut to Crack!


With digitalization, AI, and IoT, the traceability and transparency to how a PCB is produced will be even more important. We must rule out the PCBs that follow the standards to the ones that do not. The day will come when you or someone you know might need a medical device, and you want to make sure it does its job correctly.

View Story


Digital Specs for Automated Manufacturing: Find the Missing Link!


Automation and connected smart factories are the new manufacturing trend. Industry 4.0 and the Internet of things (IoT) continue to enter PCB manufacturing. However, if we continue down the same path with specifications and requirements written on electronic papers and unintelligent production files, human interpretation is still crucial to avoid mistakes. CircuitData could solve this problem because having one language for automated smart factories is the future!

View Story

PCB Norsemen: The Solution to the UL Challenge—Industrial Awareness


Writes Jan Pedersen: The solder-limit subject has been a "hot potato" for a quite some time, with many discussions around the new requirement from Underwriters Laboratories (UL) that UL’s Emma Hudson brought to attention in early 2018.

View Story

The PCB Norsemen: Lean Challenges—Standard vs. Non-Standard Products


Writes Didrick Bech: People tend to treat standard and non-standard products in the same way; however, they represent two parallel product segments and consequently different challenges for your Lean manufacturing process, especially in relation to production and logistical operations. When you fail to differentiate the processing of standard and non-standard products, not only is the Lean manufacturing process disrupted, but you also introduce a variety of production, financial and logistical challenges.

View Story

The Velocity of Technology— What Does It Really Mean?


PCB Norseman, Jan Pedersen: Driving a car is probably one of the areas where the user comes in direct touch with the technology development. And we understand the speed when we see how fast we get new versions of smartphones and other gadgets. But in what direction are we going?

View Story


Industry 4.0, AI and CircuitData


PCB Norseman, Andreas Lydersen: As automation works its way onto the shop floors, it still struggles to replace humans in the supporting roles, such as designers, purchasers, brokers, and back-office staff. Where automation on the shop floor replaces humans in doing repetitive manual tasks, the supporting roles (at least some of them) require intelligence to understand and utilise information.

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