MIPI PCB Design Guidelines for High-Speed Interfaces | Cadence

November 1, 2024

Cadence PCB Solutions

Key Takeaways

Differential Pair Routing: Maintain controlled impedance and continuous ground reference planes to reduce noise and ensure signal integrity.
Implement solid ground planes, via stitching, and proper shielding to enhance grounding and minimize electromagnetic interference.
Keep within-pair length differences ≤ 5 mils and between-pair mismatches ≤ 50 mils to prevent timing issues.

The MIPI PCB signaling standards have become widespread in computers, networking equipment, smart electronics, and other fields. They are crucial for enabling high data rates while maintaining relative immunity to noise.

There are a couple of major standards depending on your desired interface module. The Camera Serial Interface (CSI), Display Serial Interface (DSI), and PHY (Physical Layer) Design Guidelines are all integral components of MIPI standards, each serving a specific purpose in ensuring efficient, high-speed communication between components. Read on as we delve into each, and cover important MIPI PCB design guidelines.

Basic MIPI PCB Design Guidelines

Category	Guideline
Differential Pair Routing	Use a controlled impedance of 100 ohms ±10% (use simulation tools to verify). Continuous ground reference planes with a separation distance of 3x the trace width from other signals. Trace width and spacing should be calculated based on the PCB stack-up and material properties.>
Length Matching	Within pairs: ≤ 5 mils (use serpentine routing to adjust lengths if necessary). Between pairs: Length mismatch should be minimized to within 50 mils for high-speed differential pairs to avoid timing issues.
Minimize Crosstalk	Spacing: ≥ 3x trace width between differential pairs and other high-speed signals. Ground traces or guard bands should be added between differential pairs to further reduce crosstalk. Use simulation tools to evaluate crosstalk and adjust spacing as needed.
Grounding	Solid ground planes should be used under high-speed signal layers to provide a continuous reference. Implement via stitching every 1000 mils (1 inch) along the edges of the ground planes to enhance grounding and reduce EMI. Ensure no breaks in the ground plane under differential pairs.
Layer Stackup	It’s best to use a multi-layer PCB with at least 6 layers: Signal1, Ground1, Power, Ground2, Signal2, Ground3. Dedicated ground planes should be adjacent to high-speed signal layers to minimize EMI. Optimized stackup should ensure continuous reference planes with a spacing of 5 mils to 10 mils.
Via Management	Minimize the use of vias in high-speed differential pairs to avoid impedance discontinuities. When vias are necessary, use back-drilled vias to eliminate stub effects. Ensure vias are placed symmetrically in both traces of a differential pair to maintain balanced impedance.
Power Supply	Place decoupling capacitors (10 nF to 100 nF) close to the power pins of high-speed components. Use bulk capacitors (10 µF to 100 µF) near the power source. Separate power domains for high-speed PHY circuitry with low-dropout regulators (LDOs) and multiple decoupling capacitors.
EMI and Signal Integrity	Use ground planes, guard traces, and shielding cans to minimize EMI. Ensure proper grounding of shielding elements to avoid introducing noise.
Thermal Management	Implement thermal vias (10 mils to 20 mils diameter) under high-power components to aid in heat dissipation. Use heatsinks and ensure adequate airflow around high-speed components. Perform thermal analysis to identify hotspots and ensure reliable operation.

Camera Serial Interface (CSI) Design

The MIPI CSI interface is primarily used for camera modules in mobile devices. CSI can be adjusted to accommodate different resolutions and frame rates, making it ideal for a wide range of applications, from basic webcams to high-definition cameras in smartphones. Both CSI and DSI depend on the PHY design to guarantee efficient and reliable high-speed data transfer.

Key guidelines for CSI design include maintaining a differential signal line topology for transmitting data (Tx) and receiving data (Rx), ensuring differential impedance of 100Ω ± 20%, and keeping line lengths as short and equal as possible to minimize skew and signal degradation.

Use continuous ground planes and ground vias to ensure robust signal integrity. Power line topology guidelines for CSI emphasize low resistance (≤ 30mΩ) and inductance (≤ 2.8nH/5ch), with capacitors placed close to the package pins to minimize ripple noise and enhance power stability.

Display Serial Interface (DSI)

The MIPI DSI interface is designed for display modules in mobile and embedded devices. It supports high-resolution and high-refresh-rate displays. DSI enables the transmission of high-quality graphics and video, ensuring smooth and superior display performance.

The Display Serial Interface (DSI) design within the MIPI (Mobile Industry Processor Interface) standards ensures efficient, high-speed data transfer between display modules and host processors. DSI utilizes a differential signal line topology for both transmission (Tx) and reception (Rx), adhering to a differential impedance of 100Ω ± 20%.

Designers should aim to minimize line length differences and maintain line lengths as short and equal as possible. Proper line spacing, especially a minimum of three times the spacing (3S) between differential pairs and adjacent signals, is crucial to reduce electromagnetic interference and crosstalk.

For power line topology, DSI requires low resistance (≤ 30mΩ) and inductance (≤ 2.8nH/5ch) in the PCB design, with capacitors placed near the package pins to minimize ripple noise and maintain stable power supply (MIPI PCB).

MIPI PHY Design Guidelines

MIPI (Mobile Industry Processor Interface) PHY defines the physical layer specifications for various MIPI interfaces, including D-PHY, C-PHY, and M-PHY. These PHY layers are crucial for high-speed data transmission. The PHY (Physical Layer) design guidelines for MIPI are crucial for ensuring reliable high-speed data transfer.

MIPI standards include three primary PHY layers: D-PHY, C-PHY, and M-PHY, each tailored for specific applications:

MIPI M-PHY: Designed for data-intensive applications such as transferring high-resolution images, high-frame-rate video, and data transfer between mobile displays and memory. It is also used in mobile communications and storage.
MIPI D-PHY: Commonly used in smartphone cameras and displays, providing high-speed communication between the device and its processor. It is also utilized in automotive systems, including radar, cameras, infotainment systems, and dashboard displays.

Both M-PHY and D-PHY use typical differential signaling, but with different clocking methods. D-PHY uses a source-synchronous clock, while M-PHY uses an embedded clock.

MIPI C-PHY: Initially created for mobile cameras and displays, it is now also used in wearables, IoT camera systems, and automotive displays/cameras. C-PHY can share the same physical layer and device pins as D-PHY, allowing designers to use a system-on-chip (SoC) that operates in both modes. MIPI C-PHY Utilizes a more complex differential signaling scheme with three pins per lane, employing three signal levels sensed differentially, similar to bipolar-return-to-zero (bipolar-RZ). This scheme requires 50 Ohm characteristic impedance for each line and 100 Ohm differential impedance between lines, with a total of three lanes. These differential lines must be length-matched on the PCB to ensure that the rising edges coincide, accurately detecting signal levels and suppressing common mode noise.

MIPI PHY design guidelines include ensuring equal lengths for both differential pairs to reduce signal skew and degradation. It’s best to maintain a minimum of three times the spacing (3S) between differential pairs and adjacent signals, to mitigate electromagnetic interference and crosstalk

Overall, these guidelines ensure that various sensors, imaging components, peripherals, and SoCs can effectively communicate and operate across different interfaces by leveraging the appropriate physical layer for their applications.

Implementing MIPI PCB design guidelines is essential to ensure high-speed data transfer in PCBs. With Cadence tools, specifically the OrCAD X platform, designers can efficiently manage the complexities of MIPI interface designs.

Cadence’s PCB Design and Analysis Software —specifically the OrCAD X platform, aids in adhering to these guidelines. Through specialized tools like the constraint manager, you can create custom rules and ensure that you follow MIPI PCB design guidelines.

Leading electronics providers rely on Cadence products to optimize power, space, and energy needs for a wide variety of market applications. To learn more about our innovative solutions, talk to our team of experts or subscribe to our YouTube channel.