SLLS573E December   2003  – March 2024 SN65MLVD200A , SN65MLVD202A , SN65MLVD204A , SN65MLVD205A

PRODUCTION DATA  

  1.   1
  2. Features
  3. Applications
  4. Description
  5. Device Comparison Table
  6. Pin Configuration and Functions
  7. Specifications
    1. 6.1  Absolute Maximum Ratings
    2. 6.2  ESD Ratings
    3. 6.3  Recommended Operating Conditions
    4. 6.4  Thermal Information
    5. 6.5  Electrical Characteristics
    6. 6.6  Electrical Characteristics – Driver
    7. 6.7  Electrical Characteristics – Receiver
    8. 6.8  Electrical Characteristics – BUS Input and Output
    9. 6.9  Switching Characteristics – Driver
    10. 6.10 Switching Characteristics – Receiver
    11. 6.11 Typical Characteristics
  8. Parameter Measurement Information
  9. Detailed Description
    1. 8.1 Overview
    2. 8.2 Functional Block Diagram
    3. 8.3 Feature Description
      1. 8.3.1 Power-On Reset
      2. 8.3.2 ESD Protection
    4. 8.4 Device Functional Modes
      1. 8.4.1 Device Function Tables
      2. 8.4.2 Equivalent Input and Output Schematic Diagrams
  10. Application and Implementation
    1. 9.1 Application Information
    2. 9.2 Typical Application
      1. 9.2.1 Design Requirements
      2. 9.2.2 Detailed Design Procedure
        1. 9.2.2.1  Supply Voltage
        2. 9.2.2.2  Supply Bypass Capacitance
        3. 9.2.2.3  Driver Input Voltage
        4. 9.2.2.4  Driver Output Voltage
        5. 9.2.2.5  Termination Resistors
        6. 9.2.2.6  Receiver Input Signal
        7. 9.2.2.7  Receiver Input Threshold (Failsafe)
        8. 9.2.2.8  Receiver Output Signal
        9. 9.2.2.9  Interconnecting Media
        10. 9.2.2.10 PCB Transmission Lines
      3. 9.2.3 Application Curves
  11. 10Power Supply Recommendations
  12. 11Layout
    1. 11.1 Layout Guidelines
      1. 11.1.1 Microstrip Versus Stripline Topologies
      2. 11.1.2 Dielectric Type and Board Construction
      3. 11.1.3 Recommended Stack Layout
      4. 11.1.4 Separation Between Traces
      5. 11.1.5 Crosstalk and Ground Bounce Minimization
      6. 11.1.6 Decoupling
    2. 11.2 Layout Example
  13. 12Device and Documentation Support
    1. 12.1 Documentation Support
      1. 12.1.1 Related Documentation
    2. 12.2 Receiving Notification of Documentation Updates
    3. 12.3 Support Resources
    4. 12.4 Trademarks
    5. 12.5 Electrostatic Discharge Caution
    6. 12.6 Glossary
  14. 13Revision History
  15. 14Mechanical, Packaging, and Orderable Information

Package Options

Refer to the PDF data sheet for device specific package drawings

Mechanical Data (Package|Pins)
  • D|14
Thermal pad, mechanical data (Package|Pins)
Orderable Information

Decoupling

Each power or ground lead of a high-speed device must be connected to the PCB through a low inductance path. For best results, one or more vias are used to connect a power or ground pin to the nearby plane. Ideally, via placement is immediately adjacent to the pin to avoid adding trace inductance. Placing a power plane closer to the top of the board reduces the effective via length and its associated inductance.

SN65MLVD200A SN65MLVD202A  SN65MLVD204A SN65MLVD205A Low
                    Inductance, High-Capacitance Power Connection Figure 11-6 Low Inductance, High-Capacitance Power Connection

Bypass capacitors must be placed close to VDD pins and can be placed conveniently near the corners or underneath the package to minimize the loop area. This extends the useful frequency range of the added capacitance. Small physical-size capacitors (such as 0402, 0201, or X7R surface-mount capacitors) must be used to minimize body inductance of capacitors. Each bypass capacitor is connected to the power and ground plane through vias tangent to the pads of the capacitor as shown in Figure 11-7(a).

An X7R surface-mount capacitor of size 0402 has about 0.5 nH of body inductance. At frequencies above about 30 MHz, X7R capacitors behave as low-impedance inductors. To extend the operating frequency range to a few hundred MHz, an array of different capacitor values like 100 pF, 1 nF, 0.03 μF, and 0.1 μF are commonly used in parallel. The most effective bypass capacitor can be built using sandwiched layers of power and ground at a separation of 2 to 3 mils. With a 2-mil FR4 dielectric, there is approximately 500 pF per square inch of PCB.

Many high-speed devices provide a low-inductance GND connection on the backside of the package. This center pad must be connected to a ground plane through an array of vias. The via array reduces the effective inductance to ground and enhances the thermal performance of the small surface mount technology (SMT) package. Placing vias around the perimeter of the pad connection ensures proper heat spreading and the lowest possible die temperature. Placing high-performance devices on opposing sides of the PCB using two GND planes (as shown in Figure 9-4) creates multiple paths for heat transfer.

Thermal PCB issues are often the result of one device adding heat to another, resulting in a very high local temperature. Multiple paths for heat transfer minimize this possibility. In many cases, the GND pad that is so important for heat dissipation makes the optimal decoupling layout impossible to achieve, due to insufficient pad-to-pad spacing as shown in Figure 11-8(b). When this occurs, placing the decoupling capacitor on the backside of the board keeps the extra inductance to a minimum.

It is important to place the VDD via as close to the device pin as possible while still allowing for sufficient solder mask coverage. If the via is left open, solder may flow from the pad into the via barrel, which results in a poor solder connection

SN65MLVD200A SN65MLVD202A  SN65MLVD204A SN65MLVD205A Typical
                    Decoupling Capacitor Layout (a) Figure 11-7 Typical Decoupling Capacitor Layout (a)
SN65MLVD200A SN65MLVD202A  SN65MLVD204A SN65MLVD205A Typical
                    Decoupling Capacitor Layout (b) Figure 11-8 Typical Decoupling Capacitor Layout (b)