Carrier board design guidelines (SOM)

From DAVE Developer's Wiki
Jump to: navigation, search

WorkInProgress.gif

Info Box
Naon am387x-dm814x.png Applies to Naon
Maya 03.png Applies to Maya
Dido-main.png Applies to Dido
Lizard.jpg Applies to Lizard
Diva-am335x-overview.png Applies to Diva
Axel-04.png Applies to Axel Ultra
Axel-lite 02.png Applies to Axel Lite
Axel-02.png Applies to AXEL ESATTA
Bora5-small.jpg Applies to Bora
BORA Xpress.png Applies to BORA Xpress


Warning-icon.png The information here provided are preliminary and subject to change. Warning-icon.png

Introduction

This page provides useful information and resources to system designers in order to design carrier boards hosting DAVE Embedded Systems system-on-modules (SOM).

These guidelines are provided with the goal to help designers to design compliant systems with DAVE Embedded Systems modules and they cover schematics and PCB aspects. They apply to several products that are listed on the top right corner of this page (see "Applies to" boxes).

Basic guidelines

In this section basic hardware guidelines valid for all DAVE Embedded Systems SOMs are detailed.

Schematics

  • Check mirroring and pinout of DAVE Embedded Systems system-on-modules (SOM) connector
  • Properly decouple DAVE Embedded Systems system-on-modules (SOM) power supply with large bulk capacitor and small bypass capacitor
  • Use low-ESR X7R capacitor if possible
  • Check for correct connection of TX and RX lines
  • Add series resistors as interface needs (see interface details)

PCB

PCB Tecnology

Use a PCB technology as advised in the following table

Parameter Min Typ Max
Layers(number) 4 6 -
Power Plane Layers 2 4 -
Clearence(mils) - 6 -
Trace Width(mils) - 6 -
Vias hole (mechanical) 0,3 -
Minimum number of via for each power signal layer changes 2 3 -
Minimum number of via for each power signal SOM connector pin 1 2 -
Component package size - 0603 -
PCB Height(mm) 1,4 1,6 -
  • If vias smaller than minimum advised size are used, take care to maintain an adeguate number of via when you change layer for each power signal.
  • PCB heights less than minimum advised can produce PCB heating and mechanical issues

PCB Basics Guidelines

  • Avoid stubs
  • Isolate clock and HI-SPEED signal (see interface specifications for further details)
  • Avoid voids on planes
  • Use Solid Connection for on plane vias
  • Place bulk and ByPass capacitor near DAVE Embedded Systems system-on-modules (SOM) power supply pins
  • Place series terminator resistor near the related transmitter

SOM Connectors

This section provides information and suggestions regarding the SOM mating connectors.

SO-DIMM

SO-DIMM mating connectors from different vendors may have slight differences in mechanical characteristics. One critical point is the position of the end of the mating area (please see the picture below), that can be slightly shifted inwards or outwards in respect to the retention holes on the carrier board. This can lead to a misalignment with the holes on the SO-DIMM modules, making difficult or impossible to insert the retentions screws or locking supports.

So-dimm-mating.png

If you plan to use the holes as additional retention system, we recommend to pay attention to the mechanical characteristics when evaluating the SO-DIMM mating connectors to be mounted on the carrier board.

Interfaces Guidelines

This section provides guidelines for the most used interfaces on DAVE Embedded Systems SOMs module.
Please refer to SOM's detailed pages for specific additional information.

Ethernet 10/100/1000

Case #1: PHY is integrated on SOM

This section refers to the case of PHY integrated on SOM such as Lizard and MAYA.

Schematics
  • If LAN connector with integrated magnetic is used:
    • predispose ethernet protection diodes on ethernet lines
    • Connect connector shield to an adeguate GND or shield Plane
PCB

Refer to this table for 10/100 differential pairs routing

Parameter for 10/100 differential pair Min Typ Max
Differential Impedance(ohm) - 100 -
Common Mode Impedance - 50 -
Gap than TX and RX signals 2xgap 2xgap -
Gap than other signals 2xgap 4xgap -
Intra pair matching(mils)* 0 25 150
TX and RX via # mismatch* 0 0 1

Refer to this table for Gigabit differential pairs routing

Parameter for Gigabit Differential Pairs Min Typ Max
Differential Impedance(ohm) - 100 -
Common Mode Impedance - 50 -
Gap than TX and RX signals 2xgap 2xgap -
Gap than other signals 2xgap 4xgap -
Intra pair matching(mils)* 0 10 10
Max PCB trace length 3" 5" -
TX and RX via # mismatch* 0 0 1


* Not mandatory but recommended.

  • If LAN connector with integrated magnetic is used:
    • do not route traces under the connettor, neither on opposite side
    • place filter diode near connector
    • place others signals far from connector
    • Connect connector shield to an adeguate GND or shield Plane or Copper through numerous vias
  • If on board magnetic are used
    • adeguately isolate system GND from magnetic connector side
    • Connect connector shield to an adeguate GND or shield Plane or Copper through numerous vias if necessary
  • try to match as best as possible each differential pair (intrapair matching)
  • Keep as best as possibile the same route for TX and RX traces
  • If less than minimum gap is used, use a GND trace for improve trace separation

Case #2: PHY is not integrated on SOM and a RGMII PHY is used

This section refers to the case of:

  • PHY not integrated on SOM
  • Gigabit PHY populated on carrier board and connected to SOM through RGMII interface.

This solution is implemented on NaonEVB-Mid for example.

Schematics
  • Add series resistors (RPACK resistors recommended) to RGMII lines
  • Properly decouple PHY Power Supplies rails
  • Properly decouple every supply pin of Ethernet PHY
  • Properly separate analog Supply Rails
PCB
Parameter for RGMII interface Min Typ Max
Common mode impedance(ohm) - 50 -
Gap than other ethernet diff pair 4xwidth - -
Gap than other signals 4xwidth -
Matching(mils) - - 200
Via Mismatch 0 0 1


Parameter for Gigabit Differential Pairs Min Typ Max
Differential Impedance(ohm) - 100 -
Common Mode Impedance - 50 -
Gap than TX and RX signals 2xgap 2xgap -
Gap than other signals 2xgap 4xgap -
Intra pair matching(mils) 0 10 10
Max PCB trace length 3" 5" -
TX and RX via # mismatch* 0 0 1

* Not mandatory but recommended.

  • Ground and VCC planes must be as large as possible
  • Avoid plane split and voids
  • Place bypass capacitor near every PHY supply pin
  • Connect every capacitor's pin to the plane with at least 2 vias and the shortest trace pattern
  • Place PHY device at least 1" (25mm) distance far away from connector
  • Keep MDIO clock signal isolated from other signals

Case #3: PHY is not integrated on SOM and a RMII PHY is used

This section refers to the case of

  • PHY not integrated on SOM
  • 10/100 Ethernet PHY populate don carrier board and interfaced to SOM through RMII interface.

This solution is implemented for example in MayaEVB-Lite board.

Schematics
  • If possible, place series resistor to RMII interface signals
  • Properly decouple PHY Power Supplies rails
  • Properly separate analog Supply Rails
  • Properly decouple every supply pin of Ethernet PHY
  • Use a standard RMII PHY that supports correct clock mode (see SOM specification for further details)
PCB
Parameter for RMII interface Min Typ Max
Reccomended Common mode impedance(ohm) - 50 -
Gap between other signal 2xW -
  • Since RMII signals are not critical such as RGMII, is not necessary a strong matching between signal
  • Avoid use of long traces
  • Avoid stubs
  • Keep as best as possibile the same routing for all RMII traces


Parameter for Ethernet Differential Pairs Min Typ Max
Differential Impedance(ohm) - 100 -
Common Mode Impedance - 50 -
Gap than other TX and RX signals 2xgap 2xgap -
Gap than other signals 2xgap 4xgap -
Intra pair matching(mils)* 0 25 150
TX and RX via # mismatch* 0 0 1

* Not mandatory but recommended.

  • Ground and VCC planes must be as large as possible
  • Avoid plane split and voids
  • Place bypass capacitor near every PHY supply pin
  • Connect every capacitor's pin to the plane with at least 2 vias and the shortest trace pattern
  • Place PHY device at least 1" (25mm) distance far away connector
  • Keep MDIO clock signal isolated from other signals


USB

Schematics

  • Create schematic in accordance with DAVE Embedded Systems system-on-modules (SOM) USB specification ( see SOM detailed pages )

PCB

Parameter for USB Differential Pairs Min Typ Max
Differential Impedance(ohm) 80 90 100
Common Mode Impedance 40,5 45 49.5
Gap than other signals 3xgap 5xgap -
Intra pair matching(mils) 0 25 150
Max allowed stubs - - 0
Max traces length - - note 1
Max allowed plane split under traces - - 0

note 1 see SOM detailed specifications

  • If a stub is unavoidable in the design, no stub should be greater than 200 mils.
  • Place a continuos reference plane underneath differential pair

HDMI

Schematics

  • Add a Transmitter Port Protection to HDMI lines
  • Use certified HDMI connector
  • Connector shield must be properly connected

PCB

Parameter for HDMI Differential Pairs Min Typ Max
Differential Impedance(ohm) 85 100 115
Gap than other signals 3xgap 5xgap -
Intra pair matching(mils) at 225MHz clock 0 20 250
Inter pair matching(mils) at 225MHz clock 0 250 1"
Max allowed stubs - - 0
Max allowed plane split under traces - - 0
  • Place a continuos reference plane underneath differential pair
  • Try to match lines as best as possible

SATA

Schematics

  • Use certified SATA connector

PCB

Parameter for SATA Differential Pairs Min Typ Max
Differential Impedance(ohm) 80 100 120
Common Mode Impedance(ohm) 51 60 69
Gap than other signals 2xgap - -
Intra pair matching(mils - - note 1
Inter pair matching(mils) - - note 1
Max allowed stubs - - 0
Max allowed plane split under traces - - 0
Max allowed length - - note 1

note 1 see SOM detailed specifications

  • Place a continuos reference plane underneath differential pair
  • Minimized vias use
  • No strong matching required between TX and RX, but keep same route for every differential pair

PCI Express

PCB

Parameter for PCI Express Differential Pairs Min Typ Max
Differential Impedance [Ohm] - 100 -
Common Mode Impedance [Ohm] - 60 -
Gap than other signals (reccomended) - 2xgap -
Intra pair matching [mils]* - - 10
Max Total Length [in]* - - 12
Maximum allowed stub - - 0
Max allowed vias - - 6
  • * Including SoM trace length
  • Preferred underneath plane over entire trace length GND.

LVDS

PCB

Parameter for LVDS Differential Pairs Min Typ Max
Differential Impedance [Ohm] 85 100 115
Common Mode Impedance [Ohm] 46.75 55 63.25
Gap than other signals (reccomended) - 2xgap -
Intra pair skew [mils]* - - 5
Inter pair skew [mils]** - 400 -
Maximum allowed stub - - 0
  • Prefer to route traces on TOP layer, referring them to a continuos GND plane.
  • * Not includes SOM's length.
  • ** Typical value can be relaxed depending on LVDS clock frequency

LCD Interface

Schematics

  • Please refer to DAVE Embedded Systems system-on-modules (SOM) carrier board documentationfor further information
  • Predispose series resistor terminator (RPACK for LCD data and single resistor for Clock and H-SYNC and V-SYNC)
  • Series resistor value may vary depending by PCB and schematic

PCB

  • If possible, use 50ohm common mode lines
  • Match LCD parallel signals in accordance with Pixel Clock frequency (further details in SOM specifications)
  • Avoid use of long traces connection (max 10" on PCB)
  • Avoid stubs

VIN Interface

Schematics

  • Please refer to DAVE Embedded Systems system-on-modules (SOM) carrier board documentationfor further information
  • Predispose series resistor terminator (RPACK for LCD data and single resistor for Clock and H-SYNC and V-SYNC)
  • Series resistor value may vary depending PCB and schematic

PCB

  • If possible, use 50ohm common mode lines
  • Match VIN parallel signals in accordance with Pixel Clock frequency (further details in SOM specifications)
  • Avoid use of long traces connection (max 10" on PCB)
  • Avoid stubs

TVOUT

Schematics

  • Please refer to DAVE Embedded Systems system-on-modules (SOM) carrier board documentationfor further information

PCB

Parameter for SATA Differential Pairs Min Typ Max
Common Mode Impedance(ohm) - 75 -
Gap than other signals 2xwidth - -
  • Keep analog TVOUT signal far from noise signals

I2C Interface

Schematics

  • Predispose properly pullup resistors on line in accordance with DAVE Embedded Systems system-on-modules (SOM)
  • Do not overload I2C lines with too much devices
  • Ensure that I2C devices are being properly initialized during power up

PCB

  • Isolate I2C clock from noise sensitive signals
  • Avoid stub

SD/MMC Interface

Min Typ Max
Common Mode impedance SOM(ohm) - 50 60
Matching required* - - -
Max allowed parallel routing(mils) - - 1000
Max trace Length** - - -
Max # of vias allowed - - -

*This is not mandatory, however it is suggested in case trace length exceeds 10cm

**Overall trace length - i.e. Bora + carrier board - should not exceed 10cm. If this is not possible, try to avoid parallel routing in order to reduce crosstalk, and refer them to a ground plane.

CAN Interface

Min Typ Max
Differential Mode impedance(ohm) 108 120 132
Matching required - - -
Min Interpair spacing - 4xgap -
Max allowed parallel routing(mils) - - -
Max trace Length - - -
Max via allowed - - -

Functional guidelines

Sudden power off management

From the architectural standpoint, modern embedded systems often resemble traditional PCs. For example:

  • they implement a rich set of I/O interfaces (large displays, Ethernet ports, USB ports, SDIO sockets etc.)
  • they likely run complex operating systems that derive from desktop world (linux, Android, Windows CE etc.)
  • they implement complex storage schemes (raw NAND, SSD, eMMC etc.).

One of the main difference between such systems and PCs is that the formers are - if appropriately designed - inherently resilient to sudden power fails. In any case, system designer should take into account these events and decide if and how manage them explicitly. Here are some typical techniques used to deal with this situation:

  • in case the system is used by human operators, the use of clean shutdown - triggered by the user himself - should be encouraged to prevent sudden power off. Technically speaking, this can be done via GUI (soft button) or mechanical device (push buttons and alike). In the latter case, push button controllers such as Linear LTC2954 can be very useful to implement this feature
  • in case no human operators interact with the system, more complex solutions might be required. This strategy is strongly dependent on hardware characteristics of SOM and must be approached on a case-by-case basis.

Thermal Management

Heat is generated by all semiconductors while operating and it is dissipated into the surrounding environment. This amount of heat is a function of the power consumed and the thermal resistance of the device package. Every silicon device on an electronic board must work within the limits of its operating temperature parameters (eg, the junction temperature) as specified by the silicon vendor.

Failure to maintain the temperature within safe ranges reduces operating lifetime, reliability, and performances and may cause irreversible damage to the system. Therefore, the product design cycle should include thermal analysis to verify that the device works within its functional limits. If the temperature is too high, component or system-level thermal enhancements are required to dissipate the heat from the system.

For detailed information, please refer to the following documents: