This section explains the general
guidelines for EPI H/W design and how to better realize the requirements with
Altium. Users can refer to the TM4C EPI reference design document [12] for the project files.
The AM13E230 hardware design guide
[13] lists the full guidance for MCU H/W design. Here are the EPI
guidelines to follow:
- Place the target device (memory IC or FPGA) close to the MCU to keep trace
lengths short
- Use 50Ω single-ended traces to control impedance
- Minimize reflections and crosstalk by routing signals groups on the same layer
and minimize vias and layer transitions
- Match the following trace lengths to reduce timing skew:
- Data bus: match within ±25mils
- Address and command signals: match within ±25mils
- Control signals: match within ±25mils to ±50mils
- Clock signals: match within ±5mils to ±10mils to the longest data
trace
- Route address and command signals in parallel
- Avoid stubs and keep routes as direct as possible
- Consider series termination resistors (22Ω to 33Ω) for data and clock lines,
placed close to the transmitter.
Note there is a recommendation for single trace from EPI pin to address/data, then to
other pin to minimize the signals reflections as shown in Figure 2-3.
To realize the H/W design easier with Altium:
- The address and data traces must use two different net names so user is able to
utilize length tuning to match the trace lengths. If the net name is currently
the same between both (after the resistor), then this becomes difficult to set
up in Altium. Utilizing different trace names between both is recommended and
when the traces meet at the EPI pin of the AM13E23019, the user can either use a
resistor to short them together or use a net tie component to short the nets
together at the pin.
Users can utilize trace matching by using the following steps in Altium:
- Go to Design > Rules from the top menu to open the PCB Rules and
Constraints editor.
- Expand the High-Speed category and select Matched Lengths.
- Right-click and select New Rule to name and configure the rules.
- Under the Where the Object Matches scope, select the specific net,
xSignal, or Net Class to match.
- Under the Constraints section, set up your tolerance limit. This defines
the maximum allowable difference between the shortest and longest trace in the
group.
- The user can then combine all the nets together in this tolerance group and set
the tolerance limit to 25mil.
Additionally, placing the resistors adjacent to corresponding SDRAM pins and keeping
the distance common between all pins and the corresponding resistors is the
recommended operation, so users do not need to do trace matching for that portion of
the trace.