DLPS023C January   2012  – August 2015 DLPC300


  1. Features
  2. Applications
  3. Description
  4. Revision History
  5. Pin Configuration and Functions
  6. 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  I/O Electrical Characteristics
    6. 6.6  Crystal Port Electrical Characteristics
    7. 6.7  Power Consumption
    8. 6.8  I2C Interface Timing Requirements
    9. 6.9  Parallel Interface Frame Timing Requirements
    10. 6.10 Parallel Interface General Timing Requirements
    11. 6.11 Parallel I/F Maximum Supported Horizontal Line Rate
    12. 6.12 BT.565 I/F General Timing Requirements
    13. 6.13 Flash Interface Timing Requirements
    14. 6.14 DMD Interface Timing Requirements
    15. 6.15 Mobile Dual Data Rate (mDDR) Memory Interface Timing Requirements
    16. 6.16 JTAG Interface: I/O Boundary Scan Application Switching Characteristics
  7. Detailed Description
    1. 7.1 Overview
    2. 7.2 Functional Block Diagram
    3. 7.3 Feature Description
    4. 7.4 Device Functional Modes
      1. 7.4.1 Configuration Control
      2. 7.4.2 Parallel Bus Interface
      3. 7.4.3 BT.656 Interface
  8. Application and Implementation
    1. 8.1 Application Information
    2. 8.2 Typical Application
      1. 8.2.1 Design Requirements
      2. 8.2.2 Detailed Design Procedure
        1. System Input Interfaces
          1. Control Interface
        2. Input Data Interface
        3. System Output Interfaces
          1. Illumination Interface
        4. System Support Interfaces
          1. Mobile DDR Synchronous Dram (MDDR)
          2. Flash Memory Interface
          3. DLPC300 Reference Clock
        5. DMD Interfaces
          1. DLPC300 to DLP3000 Digital Data
          2. DLPC300 to DLP3000 Control Interface
          3. DLPC300 to DLP3000 Micromirror Reset Control Interface
        6. Maximum Signal Transition Time
    3. 8.3 System Examples
      1. 8.3.1 Video Source System Application
      2. 8.3.2 High Pattern Rate System With Optional Fpga
  9. Power Supply Recommendations
    1. 9.1 System Power-Up and Power-Down Sequence
      1. 9.1.1 Power Up Sequence
      2. 9.1.2 Power Down Sequence
      3. 9.1.3 Additional Power-Up Initialization Sequence Details
    2. 9.2 System Power I/O State Considerations
    3. 9.3 Power-Good (PARK) Support
  10. 10Layout
    1. 10.1 Layout Guidelines
      1. 10.1.1 Printed Circuit Board Design Guidelines
      2. 10.1.2 Printed Circuit Board Layer Stackup Geometry
      3. 10.1.3 Signal Layers
      4. 10.1.4 Routing Constraints
      5. 10.1.5 Termination Requirements
      6. 10.1.6 PLL
      7. 10.1.7 General Handling Guidelines for Unused CMOS-Type Pins
      8. 10.1.8 Hot-Plug Usage
      9. 10.1.9 External Clock Input Crystal Oscillator
    2. 10.2 Layout Example
    3. 10.3 Thermal Considerations
  11. 11Device and Documentation Support
    1. 11.1 Device Support
      1. 11.1.1 Third-Party Products Disclaimer
      2. 11.1.2 Device Nomenclature
      3. 11.1.3 Device Marking
    2. 11.2 Documentation Support
      1. 11.2.1 Related Documentation
    3. 11.3 Community Resources
    4. 11.4 Trademarks
    5. 11.5 Electrostatic Discharge Caution
    6. 11.6 Glossary
  12. 12Mechanical, Packaging, and Orderable Information

Package Options

Refer to the PDF data sheet for device specific package drawings

Mechanical Data (Package|Pins)
  • ZVB|176
Thermal pad, mechanical data (Package|Pins)
Orderable Information

10 Layout

10.1 Layout Guidelines

10.1.1 Printed Circuit Board Design Guidelines

The PCB design may vary depending on system design. Table 14 provides general recommendations on the PCB design.

Table 14. PCB General Recommendations for MDDR and DMD Interfaces

Configuration Asymmetric dual stripline
Etch thickness (T) 0.5-oz. (0.18-mm thick) copper
Single-ended signal impedance 50 Ω (± 10%)
Differential signal impedance 100 Ω differential (± 10%)

10.1.2 Printed Circuit Board Layer Stackup Geometry

The PCB layer stack may vary depending on system design. However, careful attention is required in order to meet design considerations listed in the following sections. Table 15 provides general guidelines for the mDDR and DMD interface stackup geometry.

Table 15. PCB Layer Stackup Geometry for MDDR and DMD Interfaces

Reference plane 1 Ground plane for proper return
Er Dielectirc FR4 4.2 (nominal)
H1 Signal trace distance to reference plane 1 5 mil (0.127 mm)
H2 Signal trace distance to reference plane 2 34.2 mil (0.869 mm)
Reference plane 2 I/O power plane or ground

10.1.3 Signal Layers

The PCB signal layers should follow these recommendations:

  • Layer changes should be minimized for single-ended signals.
  • Individual differential pairs can be routed on different layers, but the signals of a given pair should not change layers.
  • Stubs should be avoided.
  • Only voltage or low-frequency signals should be routed on the outer layers, except as noted previously in this document.
  • Double data rate signals should be routed first.

10.1.4 Routing Constraints

In order to meet the specifications listed in Table 16 and Table 17, typically the PCB designer must route these signals manually (not using automated PCB routing software). In case of length matching requirements, the longer signals should be routed in a serpentine fashion, keeping the number of turns to a minimum and the turn angles no sharper than 45 degrees. Avoid routing long traces all around the PCB.

Table 16. Signal Length Routing Constraints for MDDR and DMD Interfaces

DMD_D(14:0), DMD_CLK, DMD_TRC, DMD_SCTRL, DMD_LOADB, DMD_OE, DMD_DRC_STRB, DMD_DRC_BUS, DMD_SAC_CLK, and DMD_SAC_BUS 4 in (10.15 cm) 3.5 in (8.8891 cm)
MEM_CLK_P, MEM_CLK_N, MEM_A(12:0), MEM_BA(1:0), MEM_CKE, MEM_CS, MEM_RAS, MEM_CAS, and MEM_WE 2.5 in (6.35 cm) Not recommended
MEM_DQ(15:0), MEM_LDM, MEM_UDM, MEM_LDQS, MEM_UDQS 1.5 in (3.81 cm) Not recommended

Each high-speed, single-ended signal must be routed in relation to its reference signal, such that a constant impedance is maintained throughout the routed trace. Avoid sharp turns and layer switching while keeping lengths to a minimum. The following signals should follow these signal matching requirements.

Table 17. High-Speed Signal Matching Requirements for MDDR and DMD Interfaces

DMD_D(14:0), DMD_TRC, DMD_SCTRL, DMD_LOADB, DMD_OE, DMD_DCLK ±500 (12.7) mil (mm)
DMD_DRC_STRB, DMD_DRC_BUS DMD_DCLK ±750 (19.05) mil (mm)
DMD_SAC_CLK DMD_DCLK ±500 (12.7) mil (mm)
DMD_SAC_BUS DMD_SAC_CLK ±750 (19.05) mil (mm)
MEM_CLK_P MEM_CLK_N ±150 (3.81) mil (mm)
MEM_DQ(7:0), MEM_LDM MEM_LDQS ±300 (7.62) mil (mm)
MEM_DQ(15:8), MEM_UDM MEM_UDQS ±300 (7.62) mil (mm)
MEM_A(12:0), MEM_BA(1:0), MEM_CKE, MEM_CS, MEM_RAS, MEM_CAS, MEM_WE MEM_CLK_P, MEM_CLK_N ±1000 (25.4) mil (mm)
MEM_LDQS, MEM_UDQS MEM_CLK_P, MEM_CLK_N ±300 (7.62) mil (mm)

10.1.5 Termination Requirements

Table 18 lists the termination requirements for the DMD and mDDR interfaces.

For applications where the routed distance of the mDDR or DMD signal can be kept less than 0.75 inches, then this signal is short enough not to be considered a transmission line and should not need a series terminating resistor.

Table 18. Termination Requirements for MDDR and DMD Interfaces

DMD_D(14:0), DMD_CLK, DMD_TRC, DMD_SCTRL, DMD_LOADB, DMD_DRC_STRB, DMD_DRC_BUS, DMD_SAC_CLK, and DMD_SAC_BUS Terminated at source with 10-Ω to 30-Ω series resistor. 30 Ω is recommended for most applications as this minimizes over/under-shoot and reduces EMI.
MEM_CLK_P and MEM_CLK_N Terminated at source with 30-Ω series resistor. The pair should also be terminated with an external 100-Ω differential termination across the two signals as close to the mDDR as possible.
MEM_DQ(15:0), MEM_LDM, MEM_UDM, MEM_LDQS, MEM_UDQS Terminated with 30-Ω series resistor located midway between the two devices
MEM_A(12:0), MEM_BA(1:0), MEM_CKE, MEM_CS, MEM_RAS, MEM_CAS, and MEM_WE Terminated at the source with a 30-Ω series resistor


10.1.6 PLL

The DLPC300 contains one internal PLL that has a dedicated analog supply (VDD_PLL, VSS_PLL). As a minimum, the VDD_PLL power and VSS_PLL ground pins should be isolated using an RC-filter consisting of two 50-Ω series ferrites and two shunt capacitors (to widen the spectrum of noise absorption). TI recommends that one capacitor be a 0.1-µF capacitor and the other be a 0.01-µF capacitor. All four components should be placed as close to the controller as possible, but it is especially important to keep the leads of the high-frequency capacitors as short as possible. Note that both capacitors should be connected across VDD_PLL and VSS_PLL on the controller side of the ferrites.

The PCB layout is critical to PLL performance. It is vital that the quiet ground and power are treated like analog signals. Therefore, VDD_PLL must be a single trace from the DLPC300 to both capacitors and then through the series ferrites to the power source. The power and ground traces should be as short as possible, parallel to each other and as close as possible to each other. See Figure 20.

10.1.7 General Handling Guidelines for Unused CMOS-Type Pins

To avoid potentially damaging current caused by floating CMOS input-only pins, TI recommends that unused controller input pins be tied through a pullup resistor to its associated power supply or through a pulldown to ground. For controller inputs with internal pullup or pulldown resistors, it is unnecessary to add an external pullup/pulldown unless specifically recommended. Note that internal pullup and pulldown resistors are weak and should not be expected to drive the external line. The DLPC300 implements very few internal resistors and these are noted in the pin list.

Unused output-only pins can be left open.

When possible, TI recommends that unused bidirectional I/O pins be configured to their output state such that the pin can be left open. If this control is not available and the pins may become an input, then they should be pulled up (or pulled down) using an appropriate resistor.

10.1.8 Hot-Plug Usage

Note that the DLPC300 provides fail-safe I/O on all host-interface signals (signals powered by VCC_INTF). This allows these inputs to be driven high even when no I/O power is applied. Under this condition, the DLPC300 does not load the input signal nor draw excessive current that could degrade controller reliability. Thus, for example, the I2C bus from the host to other components would not be affected by powering off VCC_INTF to the DLPC300. Note that TI recommends weak pullups or pulldowns on signals feeding back to the host to avoid floating inputs.

10.1.9 External Clock Input Crystal Oscillator

The DLPC300 requires an external reference clock to feed its internal PLL. This reference may be supplied via a crystal or oscillator. The DLPC300 accepts a reference clock of 16.667 MHz with a maximum frequency variation of 200 ppm (including aging, temperature, and trim component variation). When a crystal is used, several discrete components are also required as shown in Figure 19.

DLPC300 cry_oscill_lps023.gif
A. CL = Crystal load capacitance (Farads)
B. CL1 = 2 × (CL – Cstray_pll_refclk_i)
C. CL2 = 2 × (CL – Cstray_pll_refclk_o)
D. Where
  • Cstray_pll_refclk_i = Sum of package and PCB stray capacitance at the crystal pin associated with the ASIC pin pll_refclk_i.
  • Cstray_pll_refclk_o = Sum of package and PCB stray capacitance at the crystal pin associated with the ASIC pin pll_refclk_o.
Figure 19. Recommended Crystal Oscillator Configuration

If an external oscillator is used, then the oscillator output must drive the PLL_REFCLK_I pin on the DLPC300 controller, and the PLL_REFCLK_O pins should be left unconnected. The benefit of an oscillator is that it can be made to provide a spread-spectrum clock that reduces EMI. However, the DLPC300 can only accept between 0% to –2% spreading (that is, down spreading only) with a modulation frequency between 20 and 65 kHz and a triangular waveform.

Similar to the crystal option, the oscillator input frequency is limited to 16.667 MHz.

It is assumed that the external crystal or oscillator stabilizes within 50 ms after stable power is applied.

Table 19 contains the recommended crystal configuration parameters.

Table 19. Recommended Crystal Configuration

Crystal circuit configuration Parallel resonant
Crystal type Fundamental (first harmonic)
Crystal nominal frequency 16.667 MHz
Crystal frequency tolerance (including accuracy, temperature, aging, and trim sensitivity) ±200 PPM
Crystal drive level 100 max uW
Crystal equivalent series resistance (ESR) 80 max Ω
Crystal load 12 pF
RS drive resistor (nominal) 100 Ω
RFB feedback resistor (nominal) 1
CL1 external crystal load capacitor See Figure 19 pF
CL2 external crystal load capacitor See Figure 19 pF
PCB layout A ground isolation ring around the crystal is recommended

10.2 Layout Example

A complete schematic and layout example is provided in the DLP 0.3 WVGA Chipset Reference Design, which is implemented in the DLP LightCrafter EVM. The PCB stack up for this design can be seen in Table 20.

Table 20. Driver Board PCB Stackup and Impedance(1)

Layer Material Type Thickness (mil) Refer Layer Impedance
50 Ω (Single End) 100 Ω (Differential Pair)
SolderMask 0.80
Add Plating 1.04
L1 - Top L1 0.46 L2 5.5 mil (50.4 Ω) 4 mil /6 mil spacing /4 mil (99.1 Ω)
Prepreg 3.49
L2 - GND L2 1.10
Prepreg 3.39
L3 - Signal L3 1.10 L2/L4 3.5 mil (49.5 Ω)
Prepreg 5.32
L4 - GND L4 0.70
Core 12
L5 - PWR L5 0.70
Prepreg 5.27
L6 - Signal L6 1.10 L5/L7 3.5 mil (49.5 Ω)
Prepreg 3.45
L7 - GND L7 1.10
Prepreg 3.5
L8 - Bottom L8 0.46 L7 5.5 mil (50.4 Ω) 4 mil /6 mil spacing /4 mil (99.1 Ω)
(1) Total thickness = 46.82 mil; Total thickness = 1.19 mm
DLPC300 PLL_flt_layout_lps023.gifFigure 20. PLL Filter Layout
DLPC300 board_1_lps023.pngFigure 21. Top Board Layer
DLPC300 board_2_lps023.pngFigure 22. Internal Layer
DLPC300 board_3_lps023.pngFigure 23. Bottom Board Layer

10.3 Thermal Considerations

The underlying thermal limitation for the DLPC300 is that the maximum operating junction temperature (TJ) not be exceeded (see Recommended Operating Conditions). This temperature depends on operating ambient temperature, airflow, PCB design (including the component layout density and the amount of copper used), power dissipation of the DLPC300, and power dissipation of surrounding components. The DLPC300 package is designed primarily to extract heat through the power and ground planes of the PCB. Thus, copper content and airflow over the PCB are important factors.