External Memory Interfaces Agilex™ 7 F-Series and I-Series FPGA IP User Guide

ID 683216
Date 3/29/2024
Document Table of Contents

6.5.4. Reference Stackup

This topic illustrates the reference stackup on which EMIF routing design guidelines are based.

It is important to understand that trace geometry such as width, thickness, and edge-to-edge spacing, and the distance to reference planes, all impact trace impedance and crosstalk levels.

Table 108.  Reference stackup details
Layer Type Thickness
SM TOP 0.5
L1 signal 1.8
D1 prepreg 2.7
L2 gnd/power 1.2
D2 core 4.0
L3 signal 1.2
D3 prepreg 6.3
L4 gnd/power 1.2
D4 core 4.0
L5 signal 1.2
D5 prepreg 6.3
L6 gnd/power 1.2
D6 core 4.0
L7 signal 1.2
D7 prepreg 6.3
L8 gnd 1.2
D8 core 4
  Power 1.2
  prepreg 6.3
  power 1.2
  core 4
  gnd 1.2
  prepreg 6.3
  power 1.2
  core 4
L9 gnd 1.2
D9 prepreg 6.3
L10 signal 1.2
D10 core 4.0
L11 gnd/power 1.2
D11 prepreg 6.3
L12 signal 1.2
D12 core 4.0
L13 gnd/power 1.2
D13 prepreg 6.3
L14 signal 1.2
D14 core 4.0
L15 gnd/power 1.2
D15 prepreg 2.7
L16 signal 1.8
SM BOT 0.5
  Total 120.1
Figure 133. Reference trace geometries

The reference stackup height is selected to be 120 mil to cover maximum signal via coupling (110mil) in simulation while extracting EMIF design guideline. Intel® recommends that board designers do not exceed 110mil signal via coupling (stripline routing on inner layers) in the EMIF layout PCB design for DDR4 interfaces.

If the PCB stackup exceeds 120 mil in height, Intel® recommends routing EMIF signals on upper layers, not to exceed more than 110 mil of signal via coupling.

The reference stackup materials in the above figure are selected as FR4, to represent worst-case signal loss in design phase simulation. In case of low-loss materials, the maximum end-to-end routing length shall be larger than the recommended end-to-end routing length in the design guidelines; however, you must perform time-domain channel simulation to ensure that timing requirements are met.