mobile | classic
Dataweek Electronics & Communications Technology Magazine

Follow us on:
Follow us on Facebook Share via Twitter Share via LinkedIn


Electronics Buyers' Guide

Electronics Manufacturing & Production Handbook 2019


Current carrying capacity of a through-hole via
EMP 2018 Electronics Manufacturing & Production Handbook, Manufacturing / Production Technology, Hardware & Services

Editor’s note

This article contains several references to the books ‘Right The First Time, A Practical Handbook on High Speed PCB And System Design, Volumes 1 and 2,’ written by Lee Ritchey and published by Speeding Edge. These books (or digital versions of them) can be purchased online from the website

The question “What is the current carrying capacity of a through-hole via when used to move power into and out of power planes?” comes up when it is time to design the entry of power or current from a DC-to-DC converter into the planes of a PCB or from the power blades of a connector into the planes of a PCB. The question is usually: “How many vias will be needed to ensure there is a good path into the planes?” A further question might be: “How well do these vias perform when used to conduct current into the power pins of a component, such as a BGA, from the power planes?” This article will examine both of these issues.

Vias are cylinders of plated copper that connect from one side of a PCB to the other. When used to conduct power into or out of the planes of a PCB, only the portion of the plated through-hole between the plane in question and the surface is of interest. Figure 1 is a cross section view of a via piercing a PCB.

Figure 1. Cross section of a plated through-hole.
Figure 1. Cross section of a plated through-hole.

The part of the via that is of interest in this discussion is the plating on the walls of the drilled hole. The current carrying capacity question has two parts. One is the DC resistance and potential heating and voltage drop. The other is the AC resistance or reactance and the

potential voltage drop with a changing current.

Since the question usually refers to the DC voltage drop issue, let’s examine this first.

DC voltage drop and heating in a via

In order to answer the question of current­carrying capacity of a via, it is necessary to determine its DC resistance. One way to do this is to look at the plating in the hole as a sheet of copper that has been bent into a cylinder. Using this approach, a 12-mil outer diameter (0,33 mm) plated cylinder when unfolded into a flat sheet of copper would be approximately 37 mils (0,94 mm) wide by the length of the via.

Figure 2 is a plot of the resistivity of traces versus length in the three common weights of copper foil.

Figure 2. Copper trace conductivity.
Figure 2. Copper trace conductivity.

Good PCB fabrication practice calls for a minimum plating thickness of 1 mil (25,4 microns) in a plated through-hole or via. One ounce copper is 1,4 mils (36 microns) thick. Half ounce copper is 0,7 mils (18 microns) thick. Therefore, the plating in the hole is roughly 0,75 ounce copper or midway between one ounce and one half ounce. From Figure 2 it can be seen that a 12” long trace, 18 mils (0,46 mm) wide, has roughly 0,33 Ω of resistance. A trace twice as wide, or 36 mils (0,91 mm), has a resistance of half that or approximately 0,165 Ω.

There are 12 000 mils in 12” (30,5 cm), so the resistivity of our 37 mil (0,94 mm) wide trace is approximately 13,7 μΩ per mil of length. Suppose the length of the via were 100 mils (2,54 mm). Its resistance along its length would be approximately 1,3 mΩ. From this, voltage drop calculations as well as heating calculations can be made.

Suppose the current flow were 3 A. The voltage drop would be 3,9 mV and the power would be 11,7 mW. Clearly, there would be no heating problem at this current level. With a 3,9 mV voltage drop, it is unlikely that this would ever be an issue either. This example presumes that the current must travel along the entire 100 mil length of the via. In reality, the planes are normally midway into the PCB, so only a part of the via is involved resulting in an even smaller voltage drop.

The current flowing in the via must pass into the plane where the plating in the hole meets the copper in the plane. How robust this

connection is depends on how thoroughly the copper edge of the plane has been cleaned after drilling and before plating the copper into the hole. Being a pessimist, I expect that some, perhaps not many, of these holes are imperfectly cleaned. To allow for this reduction in contact area, I have rated my vias at a maximum of 3 A. This is the usual rating for the connector pins in many of the connectors that are used to deliver power into a PCB so it all works out.

A more likely source of significant voltage drop might be in the plane itself. On page 127 of the book ‘Right The First Time, A Practical Handbook on High Speed PCB and System Design, Volume 1’, the method for calculating voltage drops in a power plane is discussed.

Via inductance and AC voltage drop

Current flowing into a PCB from a DC-DC converter is primarily DC or very low in frequency. As a result, the inductance of the via has little effect on this part of the power delivery process. However, current flow out of the planes through the vias into the ICs that consume the energy may have frequency components well into the hundreds of megahertz.

Figure 3 is a plot of via inductance as a function of via length for the most common drill size used with 1 mm pitch BGAs, 12 mils or 0,3 mm. The formula for calculating via inductance is listed on Page 143 of Volume 1. The approximate inductance for a 12 mil drilled and plated via is 35,5 pH per mil of length. This may vary slightly depending on the presence of surface pads and nonfunctional pads but, for this purpose, this value is close enough to illustrate the effect of via inductance on power delivery to a BGA. The inductance is little affected by the thickness of plating which is normally at least 1 mil thick.

Figure 3. Via inductance vs. length.
Figure 3. Via inductance vs. length.

As can be seen from the graph, the inductance gets quite large as the reach down into the PCB to connect with planes grows. This has two adverse effects on power delivery systems.

The first is this inductance adds to the parasitic inductance of the bypass capacitors that are part of the power delivery system (PDS). Even at 15 mils in length, this added inductance is often larger than the parasitic inductance of the capacitors themselves. It is for this reason that choosing ultra-low inductance capacitors, such as IDCs, is not of much help when these capacitors must be connected to planes with vias.

The effect this added inductance has on the performance of a bypass capacitor is to drive its useful frequency lower than might be expected based on the manufacturer’s data sheet. It also raises the Q or quality factor of the capacitor as installed, which increases the height of the

anti-resonance peak when it forms a parallel tuned circuit with the plane capacitance of the PCB. These effects are covered in detail in Chapter 34 of Volume 1.

The second effect is that this via inductance is directly in the path of current drawn from the PDS to charge transmission lines, such as a parallel data or address bus to a DDR memory bank or a PCI bus. Figure 4 illustrates the current flow path for transitions from a logic 0 to a logic 1. As can be seen, the current must flow through the inductance in the total current path which includes the inductance of the bypass capacitors, the inductance of the vias connecting the IC to the VDD plane, the inductance of the ball, the inductance of the IC package, the inductance of the connection between the package and the IC, and the inductance in the power path on the IC itself. Notice that the VSS or ground connection is not involved in this transition.

Figure 4. Current flow when switching from logic 0 to logic 1.
Figure 4. Current flow when switching from logic 0 to logic 1.

As charge is withdrawn from the capacitance of the PDS, its terminal voltage drops, resulting in what is commonly called ripple or rail collapse. Remedies for excessive ripple are covered in the power delivery sections of Volumes 1 and 2. This rapidly changing current also develops a voltage drop across the inductance between the VDD rail and the VDD terminal of the IC, known as VDD or VCC bounce. This voltage drop or spike drives the VDD rail on the IC negative and, in most cases, drives the entire die and all of the outputs negative as well. This VDD bounce appears as a noise spike on all of the outputs whether they be at a logic 0 or a logic 1. Those at a logic 1 experience a noise spike that can induce a logic failure if the spike is large enough.

The charge drawn from the PDS charges up the parasitic capacitance of the transmission line and the input capacitance of any loads attached to the line from a low voltage to a high voltage.

Figure 5 is an example of VCC or VDD bounce on a quiet output of an FPGA driving a 64-bit data bus. This is a 2,5 V system. The magnitude of the VDD spike is 276 mV or more than 10% of the signal swing – enough to cause logic failures.

Figure 5. V<sub>CC</sub> bounce and noise on V<sub>DD</sub>.
Figure 5. VCC bounce and noise on VDD.

Figure 6 illustrates the current flow path for transitions from a logic 1 to a logic 0. Notice that the PDS is not involved in this transition. The charge put on the transmission line is being removed at this time. The current flow that results develops a voltage drop or spike across the inductances in this path which include the via inductance, the ball inductance, the package inductance and the inductance on the IC.

Figure 6. Current flow when switching from logic 1 to logic 0.
Figure 6. Current flow when switching from logic 1 to logic 0.

This voltage spike drives the VSS terminal positive with respect to the VSS rail on the PCB. As with the VDD bounce, this voltage spike appears on all of the outputs. Those outputs that are at a logic 0 will experience a noise spike that will erode the logic level and, if large enough, will cause a logic failure.

These VDD and ground bounce spikes are essentially the same amplitude in most CMOS components due to the fact that the power and ground paths into the IC are symmetrical. Either can cause a logic failure. Notice that VDD bounce is accompanied by rail collapse or a negative going voltage spike on the VDD rail. These two noise transients add together to create one large drop in the output voltage of all outputs set at a logic 1.

It is common for systems to fail from this type of noise spike. What makes failures from this mechanism so elusive is that they occur only when all or most of the lines in a wide, parallel bus simultaneously switch from one logic state to another. For a 64-bit wide bus, this is once in 264 times or once in 131 072 times. Systems failing from this source are often described as ‘flaky’.

The equation V = L(di/dt) is used to calculate the voltage drop across an inductance. What can readily be seen is that the magnitude of the voltage rises with increased inductance or increased current and with decreasing time. As IC technologies have migrated down the feature size curve from 250 nm to 130 nm to 90 nm and, as of the publishing of this article, 65 nm, the dt value or switching time of CMOS ICs has dropped dramatically to as little as 200 picoseconds for DDR2 memory outputs.

Table 1 illustrates the size of the voltage spike for parallel, single-ended buses with widths from 16 bits to 256 bits wide. This example is typical of DDR buses that commonly operate at 2,5 V. The rise time in this example is 0,5 nanoseconds and was a common rise time for ICs made with the 130 nm process. The total magnitude of the voltage spike is calculated for total inductance in the current path varying from 0,1 nH to

0,5 nH. What can be seen is that the total inductance in the current path must be kept very small as bus widths grow wide and as rise times grow small.

Table 1. V<sub>CC</sub> or ground bounce vs. package inductance and bus width.
Table 1. VCC or ground bounce vs. package inductance and bus width.

A PCB design engineer has little or no control over the inductance in the IC package other than to exercise care when choosing new components to ensure that the package has been properly designed. The one place where a PCB design engineer can influence the inductance in the current path is the choice of the location of the power layers in the PCB stackup. Clearly, the closer these two layers (power and ground) are to the component side of the PCB, the lower the added parasitic inductance of the power vias will be.

There are many designs that are based on four-layer stackups, with one plane close to the component side of the PCB and the other 40 to 50 mils away at the bottom of the PCB. In such cases, it is not possible to keep both planes close to the IC drawing power from them. Looking at Figure 3, one or the other of the vias will have an inductance of approximately 2 nH. This would suggest that wide parallel memory buses won’t work on four-layer boards.

The PC industry has built hundreds of millions of PC motherboards that are four layers and all of them have large, fast DDR and DDR2 memory systems on them. A fair question might be, “How do they work in view of the forgoing discussions?” The methodology for solving this problem is discussed in another article.

Supplied By: EDA Technologies
Tel: +27 12 665 0375
Fax: 086 691 4210
  Share on Facebook Share via Twitter Share via LinkedIn    

Further reading:

  • Altium Designer gets 2019 update
    30 April 2019, EDA Technologies, Design Automation
    Altium Designer 19, the latest version of the company’s flagship PCB design software, introduces new features aimed at making the design of complex, high-quality projects easier, faster and more accurate, ...
  • Continued success for Zetech’s stencils division
    30 April 2019, Zetech, Manufacturing / Production Technology, Hardware & Services, News
    Best known for supplying SMT (surface mount technology) equipment and consumables for printed circuit board assembly for 33 years, Zetech is enjoying success with its more recently established stencils ...
  • How to analyse blind via hole failures
    27 March 2019, This Week's Editor's Pick, Manufacturing / Production Technology, Hardware & Services
    It has become common practice to use blind, filled and stacked vias in many portable electronics products. Experience has shown that this method of interconnection is reliable, provided the fabrication process is well defined and controlled.
  • PCB microsectioning – paying attention to detail
    27 March 2019, Cirtech Electronics, This Week's Editor's Pick, Manufacturing / Production Technology, Hardware & Services
    In our high-tech world, it’s easy to overlook the importance of the humble printed circuit board (PCB). Buried in each electronic gadget or appliance there’s always at least one PCB and each one has ...
  • X-ray dose considerations
    27 March 2019, MyKay Tronics, Manufacturing / Production Technology, Hardware & Services
    The benefits of using X-ray technology in the electronics industry to inspect printed circuit board assemblies are well proven. This article summarises X-ray radiation dose, and the techniques that ...
  • Product development issues explored in new video
    27 March 2019, Manufacturing / Production Technology, Hardware & Services
    Printed circuit broker, Elmatica, recently released a new film about product development, explaining why cooperating with an experienced partner could be a smart move. “We have several times seen the ...
  • Flux management system earns APEX award
    27 March 2019, MyKay Tronics, Manufacturing / Production Technology, Hardware & Services
    BTU International was awarded a 2019 NPI award in the reflow soldering category for its new Aqua Scrub flux management technology. The award was presented to the company during a ceremony that took place ...
  • Solder dross recovery system
    27 March 2019, Electronic Industry Supplies, Manufacturing / Production Technology, Hardware & Services
    Stannol’s Solder Saver is a mechanical device to reduce dross, which occurs as an unavoidable side effect in wave soldering systems. According to its manufacturer, solder consumption can be reduced by ...
  • Water-soluble solder paste
    27 February 2019, Techmet , Manufacturing / Production Technology, Hardware & Services
    Indium has released Indium6.6HF solder paste – a new water-soluble, halogen-free solder paste that is compatible with both tin-lead and lead-free alloys. It is designed to provide enhanced stencil printing ...
  • Affordable soldering station
    27 February 2019, Electronic Industry Supplies, Manufacturing / Production Technology, Hardware & Services
    The Industa 550 soldering station, available from Stannol, is an affordable unit characterised by easy operation and universal fields of application. The temperature is easy to set using a potentiometer, ...
  • Stencil underside cleaning and manual post-cleaning
    27 February 2019, Testerion, Manufacturing / Production Technology, Hardware & Services
    According to experts, between 60 and 70% of all defects and failures during or after the soldering process are attributable to defects in the printing process (Figure 1). In general, these are faulty ...
  • What you need to know about the Hermes standard
    EMP 2019 Electronics Manufacturing & Production Handbook, Manufacturing / Production Technology, Hardware & Services
    Taking advantage of modern TCP/IP communication and XML data format technologies, Hermes is effectively a replacement of the more than 20-year-old SMEMA standard.

Technews Publishing (Pty) Ltd
1st Floor, Stabilitas House
265 Kent Ave, Randburg, 2194
South Africa
Publications by Technews
Dataweek Electronics & Communications Technology
Electronics Buyers’ Guide (EBG)

Hi-Tech Security Solutions
Hi-Tech Security Business Directory

Motion Control in Southern Africa
Motion Control Buyers’ Guide (MCBG)

South African Instrumentation & Control
South African Instrumentation & Control Buyers’ Guide (IBG)
Terms & conditions of use, including privacy policy
PAIA Manual


    Classic | Mobile

Copyright © Technews Publishing (Pty) Ltd. All rights reserved.