The designers are constantly challenged to improve the performance of an electronic product. At the same time, the designers need to consider the effects of high-speed signals in a PCB design since continuously increasing clock frequencies and decreasing rise times may lead to signal integrity issues. This requires higher frequencies to be used, and frequencies of 50MHz to 3GHz have become very common.
Designing high-speed PCBs is crucial to support real-world applications. Signal transmission problems are prominent when a PCB deals with high-speed signals. An excellent high-speed board is the one that integrates various components and routing while avoiding signal integrity issues. The three main challenges that we are facing in high-frequency boards are signal integrity, EMI/EMC, and dielectric loss.
In this blog post, we will be discussing the following factors that require attention while dealing with high-speed signals in a PCB design:
- What is a high-speed signal in PCB?
- Why is there always a signal distortion at high-frequency?
- When do we need to take care of signal integrity in high-speed PCB design?
- Techniques to overcome signal integrity issues in high-speed PCB Design
- Quick tips for high-speed PCB designers
- Materials for high-speed PCBs
- Why is it important to include design simulations and checks in high-speed PCB design?
What is a high-speed signal in a PCB?
Signals with frequencies ranging from 50 MHz to as high as 3 GHz are considered high-speed signals such as clock signals. Ideally, a clock signal is a square wave, but it is practically impossible to change its ‘LOW’ level to ‘HIGH’ level (and vice versa) instantly. It has a specific rise and fall time due to which it appears to be a trapezoid in the time domain. It is worth noticing that the amplitude of the higher frequency harmonics of the clock signal in the frequency domain depends upon its rise and fall time. If the rise time is longer than the magnitude of the harmonics will become smaller.
Why is there always a signal distortion at high-frequency?
At low frequency (>1kHz), the signals remain within the data characterization limits, and the system performs as intended. When speed increases, the higher frequency impact comes at play, resulting in ringing, crosstalk, reflections, ground bounce, and impedance mismatch issues. It not only affects the digital properties of the system but the analog properties as well. These issues are more prone to increasing data rates for I/O interfaces and memory interfaces. Practically, these issues can be avoided by employing advanced PCB design services or by following strict layout guidelines. The signal routing, termination schemes, and power distribution techniques can help the designers to realize an effective PCB.
When do we need to take care of signal integrity in high-speed PCB design?
Signal integrity: Ideally, in a PCB, a signal should travel from a source (Tx) to a load (Rx) unimpaired/ unadulterated. But practically, it does not happen. The signal reaches the load with some losses (impedance mismatch, crosstalk, attenuation, reflection, switching issues). Signal integrity (SI) is the term defined to measure these signal distortions in the high-frequency regime. Signal integrity helps to predict and understand these critical issues by providing practical solutions.
High-speed PCB design requires traces to be visualized as transmission lines instead of simple wires. Identification of the highest operating frequency in the design helps to target the traces that should be treated as transmission lines. If the traces exceed about 1/10 of the wavelength of that frequency, then they can be treated as the transmission lines. These transmission lines require digital as well as analog analysis.
PCB substrate: Substrate material used during the PCB construction contributes to signal integrity problems. Each PCB substrate has a different relative dielectric constant (εr) value. It determines the length at which the signal traces must be considered as transmission lines, and of course, in such scenarios, the designers need to take care of signal integrity threats.
Using εr value, designers can evaluate the velocity (Vp) at which the signal flows and propagation delay (tPD). These parameters help to determine the length at which the trace should be considered as a transmission line. The below-mentioned graph depicts how insertion loss increases with signal frequency. The insertion loss (per inch) is measured for FR-4 (glass epoxy) and high-frequency Rogers RO4350B material. Higher insertion loss may lead to more attenuation. Click here for more insight on high-speed PCB laminates.
Techniques to overcome signal integrity issues in high-speed PCB design
Designers can implement the following design techniques in a high-speed PCB:
1. Impedance matching in high-speed PCB design
This parameter is important for faster and longer trace runs. The three factors that affect impedance control are substrate material, trace width, and height of the trace from the ground/power plane.
At low frequency, a PCB track is defined by its DC characteristics. It can be considered as an ideal circuit, devoid of resistance, capacitance, and inductance. When frequency rises, inductance and capacitance associated with the track start impacting its performance. Impedance mismatch in traces due to via stubs and imperfections in traces don’t allow the signal to be fully absorbed within the receiver (load); that’s why the extra energy is reflected towards the transmitter (source). This process repeats again and again until all the energy is absorbed. At high data rates, it causes signal overshoot, undershoot, and ringing, which generate signal errors. To solve this problem, these transmission lines are provided with ground planes underneath them and termination resistances.
It is important to calculate the impedance of the line. (It is calculated by combining the line thickness, the dielectric constant of the board, and the distance between the line and the ground plane.) Sometimes, the transmission line needs to traverse between different layers, and therefore, the distance between the line and the ground plane changes. In such a case, the line impedance can be maintained at the same value by changing the line thickness.
Note: For high-frequency, high-speed designs, PCB tracks are considered as transmission lines.
1.1 Impedance control measures in high-speed PCB design
Impedance mismatch can be controlled by implementing adequate termination schemes. The selection of the termination scheme depends upon the application. Let us discuss some of them.
1.1.1 Parallel termination scheme: In this scheme, the termination resistor (RT) is equal to the line impedance. This termination resistor is placed as close to the load as possible for maximum efficiency. The current loading of this termination resistor is maximum at a high-output state.
1.1.2 Thevenin termination scheme: It is an alternative to the parallel termination scheme, where the terminating resistor (RT) is split into two separate resistors, which is equal to the line impedance (when combined). This scheme reduces the total current draw from the source and adds current drawn from the power supply because the resistors are placed between VCC and ground.
1.1.3 Active parallel termination: Here, the terminating resistor equal to the line impedance (Z0) is placed in the path of bias voltage. The bias voltage is arranged so that the output drivers can extract current from both high and low-level signals. This technique requires a separate voltage source that can sink and source currents to match the output transfer rates.
1.1.4 Series-RC parallel termination: In this scheme, the resistor and capacitor (>100pF) combination act as terminating impedance. Here, the terminating resistor (RT) is equal to Z0 and the capacitor blocks the low-frequency signal components and passes the high-frequency components. So, the DC loading effect of RT does not impact the driver.
1.1.5 Series termination: It matches the impedance at the signal source instead of matching it at the load. This scheme helps attenuate secondary reflections. The line impedance varies depending on the distribution of the load. Therefore, a single resistor value does not apply to all conditions. This method requires only a single component at the source rather than multiple components at each load but delays the signal path by increasing the RC time constant.
1.1.6 Differential pair termination: It requires a termination resistor between the signals at the receiving device. The termination resistor must match the differential load impedance (typically 100Ω).
DOWNLOAD OUR DIFFERENTIAL PAIR eBOOK:
2. Attenuation in high-speed PCB design
A high-frequency transmission medium makes it difficult for the receiver to interpret the correct information. The following transmission losses occur due to transmission media:
2.1 Dielectric absorption: The signal in the high-frequency medium causes the PCB dielectric material to absorb signal energy. It reduces the signal strength. It can only be controlled by choosing a perfect PCB material.
2.2 Skin effect: High-frequency signals are also responsible for generating waveforms with varying current values. Such signals have their self-inductance values, which initiate an increased inductive reactance at high frequencies. It is responsible for the reduction in the conductive area on the PCB surface, more resistance, and attenuation in the signal strength. The skin-effect can be reduced by increasing the track width but it is not feasible always.
Attenuation control in high-speed PCB design
Along with a careful selection of PCB insulator material and track layout, signal attenuation can also be reduced by including programmable differential output voltages, pre-emphasis, and receiver equalization. Increment in the differential output voltages helps to improve the signal at the receiver. Pre-emphasis is the way of only strengthening the high-frequency signal component by increasing the level of the first transmitted symbol. Receiver equalization circuitry attenuates the low-frequency signal components to cover the transmission line losses.
3. Crosstalk in high-speed PCB design
Being electronic industry enthusiasts, we all know when current, say signal, travels through a wire it generates magnetic fields around its vicinity. If two wires are nearby, then there is the possibility that the two magnetic fields will interact, causing energy cross-coupling between two signals called crosstalk. Prominently, inductive coupling (current induced by the magnetic field from source wire on the idle wire) and capacitive coupling (coupling of the electric field when the idle wire is exposed to the amount of current proportional to the rate of change of voltage in the source wire) are responsible for energy cross-coupling leading to crosstalk.
Crosstalk is of two types; vertical and horizontal. Vertical crosstalk is caused by signals on the other layers or inter-layer, while signals on the same layer or intra-layer are responsible for horizontal crosstalk.
Note: The maximum crosstalk value is the difference between the expected voltage at the receiver and the receiver threshold.
3.1 Crosstalk control in high-speed PCB design
Crosstalk can be prevented by separating the traces, by placing ground planes between the layers, and by using low dielectric material.
3.1.1 Traces separation: The center-to-center separation between the two traces should be at least 3 times their trace width. Without disturbing the separation between two traces, reducing the distance between the trace and the ground plane up to 10 mils helps in mitigating the crosstalk.
3.1.2 Placement of solid ground planes: Crosstalk between different layers can be prevented by placing solid ground planes between them. Though adding planes increases cost, they resolve SI problems like controlling trace impedance, reducing bypass capacitor current loop, and power supply impedance, etc.
3.1.3 Low dielectric constant material: Material with low dielectric constant overcomes crosstalk by reducing the mutual capacitance/stray capacitance between traces.
4. Impact of right-angle traces and vias in high-speed PCB design
Trace routing and vias location affect signal integrity by increasing reflections, crosstalk, and changing the impedance values. A trace having the right angle can cause more radiation since it increases the capacitance value in the corner region, resulting in a change of characteristic impedance followed by reflections.
Solution: Reflections can be minimized by replacing right-angle bend with two 45 degrees corners. To obtain a minimum impedance change, round-bend routing is the best.
- Vias are important for routing, but including them add to the inductance and capacitance values. This changes the characteristic impedance value, increasing in reflections.
- Vias also add to the trace length. Refrain from adding vias in different traces.
5. Use of different routing techniques in high-speed PCB design
- Orthogonal routing to direct signal on different layers and to minimize the coupled region.
- Minimize parallel run lengths (>500 mils) between signals. Route with short parallel runs only.
- Reduce drive fanout (number of loads)
6. Switching effects: Ground bounce in high-speed PCB design
Unlike analog, digital circuitry requires fast on-off time since it works on switching between ‘0’ and ‘1’ and ‘1’ and ‘0’ signal levels. When speed increases, the switching period decreases. When several outputs switch simultaneously from ‘HIGH’ logic to ‘LOW’, the charges stored in the I/O load capacitances flow into the device. This current exits the device through the internal ground through pins that have impedance onto the ground. The switching current develops a voltage in this impedance. Thus, there is a voltage difference between the device and the board ground. This voltage difference is known as ground bounce. The ground bounce causes a ‘LOW’ output to be seen as ‘HIGH’ by other devices on the board. Ground bounce can be reduced by adopting solutions like:
- Pin slew rate control (allows the designer to slow down the driver so that the bounce rate could be reduced). Fast slew rate is responsible for reflection, crosstalk, and ground bounce; that’s why its reduction is a must.
- Provide multiple power and ground pins (allow locating a high-speed I/O pin close to a ground pin to mitigate the switching effects).
6.1 Design considerations for ground bounce reduction in high-speed PCB
While dealing with high-speed signals in a PCB, a designer should consider the following design considerations:
- Add decoupling capacitors for the corresponding VCC/GND pair. Add the decoupling capacitors as close as possible to the supply and ground pins of the device. If the power and GND come to the pins through vias then the decoupling capacitor should be placed between the pins and the vias.
- Add external buffers at the output to minimize the loading on device pins.
- Control the load capacitance by buffering loads with an external device, such as a buffer IC.
- Minimize the number of outputs that can switch simultaneously and distribute them uniformly throughout the device.
- Remove pull-up resistance wherever possible (use pull-down resistors).
- Use multi-layer PCBs that provide separate VCC and ground planes.
- Develop synchronous designs. Such designs will not be affected by instantaneous pin-switching.
- Implement a bigger via size to connect the capacitor pad to the power and ground plane to reduce the inductance in decoupling capacitors.
- Place the via close to the capacitor pad.
- Use surface-mount capacitors to minimize lead inductance.
Note: System noise can be reduced by providing uniformly distributed power through power planes.
7. EMI reduction in high-speed PCB design
PCBs also affect the EMI/EMC performance of the system. Auto-routed boards generally abide by the design rules (DRC) and do not meet the electromagnetic compatibility requirements. Such boards require fixes such as ferrites on cables and shielded enclosures. That’s why it’s always advised to ensure that components are properly placed and traces are optimally routed. It helps to realize products that fulfill all electromagnetic compatibility and signal integrity requirements on time within the given budget. Designing an electromagnetic-compatible PCB can improve the overall system’s performance. Learn more about PCB design guidelines for EMI and EMC.
Every PCB is susceptible to electromagnetic interference. It can be reduced through the following ways:
- Use low-inductance components, like surface mount capacitors having low ESR and effective series inductance (ESL).
- Provide proper grounding to achieve the shortest current return path and the shortest current loops.
- Always use solid ground planes next to the power/signal planes.
Quick tips for high-speed PCB designers
- Identify the highest frequency net and calculate the fastest rise time in the system.
- Check the electrical specifications at the inputs and outputs of the sinks and sources.
- Give a thought about controlled impedance values, termination, and propagation delay on a trace.
- Choose between microstrip (refers to a trace routed on an outside layer of the PCB separated by a dielectric from the reference plane (GND or VCC) and stripline (refers to a trace routed on an inside layer with two reference planes) routing techniques. Simulate to identify which method is more EMC-compliant and can give better signal integrity results?
- For quality signal transmission also consider clock and differential routing techniques.
- Think about the number of different supply voltages. Do they have their power plane, or is it possible to split them?
- Create a diagram for functional groups like transmitter path, receiver path, analog signals, digital signals, etc.
- Is there any interconnection between at least two independent functional groups? Pay attention to them and always consider the return current and crosstalk to other traces.
- Think about space width clearance.
- What should be the minimum distance between the two layers?
- What are the minimum Drill and Via requirements? Is it feasible to use blind and buried vias?
DOWNLOAD OUR HIGH-SPEED PCB DESIGN GUIDE:
High-speed PCB Materials
The most commonly used laminate material is FR-4. It is very cost-effective as long as the board frequencies kept in the range from 2.5 to 3 GHz. At high-speed, materials, like Rogers RO4350, have better properties than the FR-4. The only trade-off is cost. Non-FR-4 materials are expensive.
The velocity of the signal travelling through the PCB depends upon the dielectric constant of the PCB. Let’s have an example: when frequency surpasses 5 GHz, the dielectric constant of FR-4 (4.7) drops to 4. On the other hand, the dielectric value of Rogers RO4350 remains constant (around 3.5) till 15 GHz. If the dielectric constant of the PCB will keep on changing with the frequency then different frequency components of the signal will acquire different velocities and will reach the load at different times, resulting in signal distortion. A more detailed explanation is available in our post on high-speed PCB laminates.
Why is it important to include design simulations and checks in high-speed PCB design?
Signal integrity checks are essential to maintain design transparency. If it’s not performed during the design, then it cannot be eradicated once the board has been built. In view of this, the PCB design software comes with a signal integrity check so that the PCB layout can be optimized to minimize the errors. Do you want to learn more about how to simulate a channel for identifying and resolving signal integrity problems? Then watch our tutorial with Keysight on the basics to solve signal integrity problems.
In high-speed designs, signal integrity and EMC understanding and implementation during design play an important role.Signal integrity is all about identifying and eliminating factors responsible for degrading a signal’s quality when it travels through a medium from one point to another on a PCB. Signal integrity becomes very critical when a PCB operates at high-frequency since signal rise times are low. Adopting adequate termination schemes, attenuation control, crosstalk and ground bounce prevention can help the designers to realize a PCB that can work seamlessly at high-frequency. Additionally, an EMI-compliant design is also essential.
DOWNLOAD OUR PCB TRANSMISSION LINES eBOOK: