Holiday Notice: PCBWay factories will be on holiday from Sept 30th to Oct 2nd (GMT+8). Orders can be placed as usual during holidays, the delivery date shall be postponed accordingly. Read more >>



Impedance Control

In modern electronic product design, impedance control plays a crucial role. PCB impedance control involves key performance indicators such as signal transmission stability, anti-interference ability, and power consumption. Next, let's explore the relevant knowledge about impedance control.

What is Impedance?

In circuits with resistors, inductors, and capacitors, the impedance that hinders the flow of current in the circuit is called impedance. Impedance is commonly represented by the symbol "Z" and is a complex number, with the real part known as resistance and the imaginary part known as reactance. Capacitive reactance refers to the impedance offered by capacitors to alternating current in a circuit, while inductive reactance refers to the impedance offered by inductors to alternating current. The combined impedance resulting from capacitive and inductive reactance to alternating current is referred to as impedance. The unit of impedance is ohms.

What is Impedance Control?

In a circuit board, various signals are transmitted through conductors, and to enhance their data rates, it is necessary to increase their frequencies. The circuit board itself may vary in etching, layer stack-up thickness, and trace width, leading to changes in impedance and causing signal distortion. Therefore, for conductors on high-speed circuit boards, their impedance values need to be controlled within a specific range, a practice known as "impedance control."

PCB designers typically need to implement impedance control for PCBs used in high-speed digital applications, such as RF communications, telecommunications, computing with frequencies higher than 100MHz, high-speed signal processing, and high-quality analog video (e.g., DDR, HDMI, Gigabit Ethernet).

At high frequencies, PCB signal traces behave like transmission lines, and every point along the signal trace has impedance. If the impedance changes from one point to another, signal reflections occur, with the magnitude depending on the difference between the two impedances. The greater the difference, the stronger the reflection. This reflection propagates in the opposite direction to the signal, meaning the reflected signal adds to the primary signal.

As a result, the original signal becomes distorted, and what was intended to be transmitted from the transmitting end may change by the time it reaches the receiving end. The distortion could be significant enough to impair the signal's intended functionality. Therefore, to achieve distortion-free signal transmission, PCB signal traces must maintain consistent impedance control to minimize signal distortion caused by reflections. This is the first step in improving signal integrity on PCB trace routing.

Factors that Influence Impedance

When one parameter varies while keeping other conditions constant, the factors affecting impedance are as follows:

  • Trace width: Trace width is inversely proportional to impedance. Thinner trace widths come with higher impedance, while wider trace widths come with lower impedance. Controlling trace width within a tolerance of +/- 10% is necessary for better impedance control. Gaps in signal traces impact the entire test waveform, and its single-point impedance is too high, making the entire waveform uneven. Impedance lines should not be patched, and any gap in the signal trace should not exceed 10%. Trace width is primarily controlled through etching processes. To ensure trace width accuracy, engineering compensation is performed on the photomasks based on etch undercut, lithographic errors, and pattern transfer errors.

  • Dielectric thickness: Dielectric thickness is directly proportional to impedance. The thicker the dielectric, the higher the impedance. Different semicured sheets have varying resin content and thickness. The final thickness after lamination depends on the flatness of the press and the pressing plate's procedure. For any type of board material, engineering design, press plate control, and incoming material tolerances are essential for obtaining the permissible dielectric layer thickness.

  • Dielectric constant: Dielectric constant is inversely proportional to impedance. A higher dielectric constant comes with a lower impedance. Dielectric constant is primarily controlled through material selection. Different board materials have distinct dielectric constants, which are related to the resin materials used. For instance, FR4 board materials have dielectric constants ranging from 3.9 to 4.5, decreasing with increasing frequency. PTFE board materials have dielectric constants ranging from 2.2 to 3.9. High-speed signal transmission requires higher impedance values, thus necessitating lower dielectric constants.

  • Copper thickness: Copper foil thickness is inversely proportional to impedance. The thicker the copper, the lower the impedance. Copper thickness can be controlled through pattern electroplating or selecting base material copper foil with the appropriate thickness. 

  • Soldermask thickness: Soldermask thickness is inversely proportional to impedance. Within a certain range, the thicker the soldermask, the lower the impedance. Typically, printing one pass of solder mask reduces single-ended impedance by 2 ohms and differential impedance by 8 ohms. The reduction value doubles when printing two passes compared to one pass. After printing three times or more, the impedance value no longer changes.

PCBWay Impedance Design & Control 

(only sampling 100Ω differential impedance)

  • Design stackup. The min. dielectric thickness between layers should be 50um.


  • Design circuit width and space width. According simulation calculation design circuit trace.

      the trace/space width for stackup 1# is 70/130um;

      the trace/space width for stackup 2# is 95/140um;

      the trace/space width for stackup 3# is 125/130um;

      the trace/space width for stackup 4# is 105/150um.

  • Determine the process parameters  by first article inspection,  control the process paramaters.

  • Random check the impedance in production and random check the finished product.

Considerations for Impedance Calculations

  • Choose wider trace width, not narrower.

There is a limit to how narrow traces can be in the fabrication process, whereas there is no limit to how wide they can be. If, during fabrication, the PCB manufacturer needs to reduce the trace width to achieve a specific impedance and reaches the narrow limit, it can lead to complications. This might result in increased costs, relaxed impedance control, or design modifications. Therefore, when calculating, aiming for relatively wider trace width means slightly lower target impedance, for example, if the target impedance is 50 ohms, we should aim for around 49 ohms, avoiding calculations close to 51 ohms.

  • Overall trends in impedance control.

Our design may have multiple impedance control targets, either bias toward larger or bias toward smaller values. Avoid cases where, for example, the 100 ohms bias toward larger values and the 90 ohms biased toward smaller values.

  • Consider copper balance and resin flow.

When one side or both sides of the semi-cured sheets involve etched traces, during the lamination process, the resin will fill the gaps left by the etched traces, resulting in reduced resin thickness between the layers. The lower the copper balance, the more resin will be added, leaving less remaining. So, if you need a semi-cured sheet thickness of 5 mils between two layers, choose a slightly thicker semi-cured sheet based on the copper balance.

  • Specify glass fabric type and resin content.

Different glass fabrics and resin content in the semi-cured sheets or core materials lead to different node coefficients. Even with approximately the same height, there can be differences between 3.5 and 4, which can cause a variation of about 3 ohms in single-line impedance. Additionally, the glass effect and the size of the glass fabric openings are closely related. If you are designing for 10Gbps or higher speeds and your stack-up does not specify the materials, and the PCB manufacturer uses single sheet 1080 material, it could lead to signal integrity issues.

  • Communicate with the PCB manufacturer.

Sometimes, there may be calculation errors in copper balance and resin flow, and the dielectric constant of new materials might not match the nominal values. Some PCB manufacturers may not have the required glass fabric in stock, leading to difficulties in implementing the stack-up or causing delays. When encountering such situations, the best approach is to communicate with the PCB manufacturer from the beginning of the design, asking them to design a stack-up based on the designer's requirements and their own experience. Through multiple rounds of communication and confirmation, an ideal stack-up can be achieved with a few iterations, which will facilitate the subsequent design process.

Welcome to use our impedance calculation tool. To accommodate more design types, we will upgrade it in the future.

Impedance Calculation>>

コメント (3)
ここでのメッセージは、上記の内容を補足するものであり、注文などの取引操作を対象としたものではありません。 緊急の質問や注文の問題がある場合は、営業担当者にお問い合わせください。
アップロードできるファイルは合計で1つのみです。 各ファイルは2MBを超えることはできません。 JPG、JPEG、GIF、PNG、BMPをサポート
0 / 10000