To reduce the reflection phenomenon during high-speed signal transmission, it is necessary to maintain impedance matching at the signal source, receiving end, and transmission line. The specific impedance of a single-ended signal line depends on its line width and its relative position to the reference plane. The line width/spacing of differential pairs with specific impedance requirements depends on the chosen PCB stackup structure. Since the minimum line width and minimum spacing depend on the type of PCB and cost requirements, the selected PCB stackup structure must meet all impedance requirements on the board, including inner and outer layers, single-ended and differential lines, etc.

1. PCB Stackup Design

Principles for defining layer design:

1) The main chip should be adjacent to the ground plane, providing a reference plane for device surface wiring;

2) All signal layers should be as close to the ground plane as possible;

3) Avoid having two signal layers directly adjacent;

4) The main power supply should be as close to its corresponding ground as possible;

5) Symmetrical structure design should be adopted in principle. Symmetry includes: symmetry in the thickness and types of dielectric layers, copper foil thickness, and the distribution types of patterns (large copper foil layers, line layers).

Recommended PCB layer definition scheme: When setting specific PCB layers, the above principles should be flexibly grasped, and the arrangement of layers should be determined according to actual needs, avoiding rigid application. The following provides common layer arrangement recommendations for reference. When setting layers, if there are adjacent wiring layers, the spacing between adjacent wiring layers can be increased to reduce interlayer crosstalk. For cross-segment situations, ensure that key signals must have a relatively complete reference ground plane or provide necessary bridging measures.

RK3588 currently uses 10-layer 1st stage, 10-layer 2nd stage, and 8-layer through-hole PCBs. The following stackup structure serves as an example and can assist customers in the selection and evaluation of stackup structures. If other types of stackup structures are chosen, please recalculate the impedance based on the specifications provided by the PCB manufacturer.

2. 8-Layer Through-Hole Board 1.6mm Thickness Stackup Design

In the 8-layer through-hole board stackup design, the reference plane for the top layer signal L1 is L2, and the reference plane for the bottom layer signal L8 is L7. The recommended stacking is TOP-Gnd-Signal-Power-Gnd-Signal-Gnd-Bottom, and the base copper thickness should all be 1 oz, with a thickness of 1.6mm. The detailed stackup design is shown in Table 1-1.

Table 1-1 8-Layer Through-Hole Board 1.6mm Thickness Stackup Design

3. 8-Layer Through-Hole Board 1.6mm Thickness Impedance Design

① Outer single-ended 40-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width to be 5.8 mils. Since L1 and L8 layers are designed symmetrically, the single-ended routing for L1 and L8 layers is 5.8 mils. As shown in Figure 1-1.

Figure 1-1 Outer Single-Ended 40 Ohm Routing Impedance Design

② Outer single-ended 50-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width to be 3.8 mils. Since L1 and L8 layers are designed symmetrically, the single-ended routing for L1 and L8 layers is 3.8 mils. As shown in Figure 1-2.

Figure 1-2 Outer Single-Ended 50 Ohm Routing Impedance Design

③ Outer differential 80-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 4.3/3.7 mils. Since L1 and L8 layers are designed symmetrically, the differential routing for L1 and L8 layers is 4.3/3.7 mils. As shown in Figure 1-3.

Figure 1-3 Outer Differential 80 Ohm Routing Impedance Design

④ Outer differential 85-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.9/4.1 mils. Since L1 and L8 layers are designed symmetrically, the differential routing for L1 and L8 layers is 3.9/4.1 mils. As shown in Figure 1-4.

Figure 1-4 Outer Differential 85 Ohm Routing Impedance Design

⑤ Outer differential 90-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.6/4.4 mils. Since L1 and L8 layers are designed symmetrically, the differential routing for L1 and L8 layers is 3.6/4.4 mils. As shown in Figure 1-5.

Figure 1-5 Outer Differential 90 Ohm Routing Impedance Design

⑥ Outer differential 100-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.3/7.7 mils. Since L1 and L8 layers are designed symmetrically, the differential routing for L1 and L8 layers is 3.3/7.7 mils. As shown in Figure 1-6.

Figure 1-6 Outer Differential 100 Ohm Routing Impedance Design

⑦ Inner single-ended 40-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width to be 6.8 mils. Since L3 and L6 layers are designed symmetrically, the single-ended routing for L3 and L6 layers is 6.8 mils. As shown in Figure 1-7.

Figure 1-7 Inner Single-Ended 40 Ohm Routing Impedance Design

⑧ Inner single-ended 50-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width to be 4.2 mils. Since L3 and L6 layers are designed symmetrically, the single-ended routing for L3 and L6 layers is 4.2 mils. As shown in Figure 1-8.

Figure 1-8 Inner Single-Ended 50 Ohm Routing Impedance Design

⑨ Inner differential 80-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 4.0/4.0 mils. Since L3 and L6 layers are designed symmetrically, the differential routing for L3 and L6 layers is 4.0/4.0 mils. As shown in Figure 1-9.

Figure 1-9 Inner Differential 80 Ohm Routing Impedance Design

⑩ Inner differential 85-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.6/4.4 mils. Since L3 and L6 layers are designed symmetrically, the differential routing for L3 and L6 layers is 3.6/4.4 mils. As shown in Figure 1-10.

Figure 1-10 Inner Differential 85 Ohm Routing Impedance Design

⑪ Inner differential 90-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.3/4.7 mils. Since L3 and L6 layers are designed symmetrically, the differential routing for L3 and L6 layers is 3.3/4.7 mils. As shown in Figure 1-11.

Figure 1-11 Inner Differential 90 Ohm Routing Impedance Design

⑫ Inner differential 100-ohm impedance design: Using the Huaqiu DFM tool, select the outer single-ended impedance model, input the corresponding parameters, and calculate the corresponding line width/spacing to be 3.3/7.7 mils. Since L3 and L6 layers are designed symmetrically, the differential routing for L3 and L6 layers is 3.3/7.7 mils. As shown in Figure 1-12.

Figure 1-12 Inner Differential 100 Ohm Routing Impedance Design

The overall impedance routing line widths are shown in Table 1-2:

Table 1-2 8-Layer 1.6mm Overall Impedance Routing Line Width

4. 8-Layer Through-Hole Board 1.2mm Thickness Stackup Design

In the 8-layer through-hole board stackup design, the reference plane for the top layer signal L1 is L2, and the reference plane for the bottom layer signal L8 is L7. The recommended stacking is TOP-Gnd-Signal-Power-Gnd-Signal-Gnd-Bottom, and the base copper thickness should all be 1 oz, with a thickness of 1.2mm. The detailed stackup design is shown in Table 1-3.

Table 1-3 8-Layer Through-Hole Board 1.2mm Thickness Stackup Design

5. 8-Layer Through-Hole Board 1.2mm Thickness Impedance Design

According to the stackup design parameters shown in Figure 1-3, use the Huaqiu DFM software for impedance calculation. The calculation method is the same as for the above 8-layer 1.6mm through-hole board, and the impedance line widths and spacings calculated are shown in Table 1-4.

Table 1-4 8-Layer Through-Hole Board 1.2mm Thickness Impedance Design

6. 8-Layer Through-Hole Board 1.0mm Thickness Stackup Design

In the 8-layer through-hole board stackup design, the reference plane for the top layer signal L1 is L2, and the reference plane for the bottom layer signal L8 is L7. The recommended stacking is TOP-Gnd-Signal-Power-Gnd-Signal-Gnd-Bottom, and the base copper thickness should all be 1 oz, with a thickness of 1.0mm. The detailed stackup design is shown in Table 1-5.

Table 1-5 8-Layer Through-Hole Board 1.0mm Thickness Stackup Design

7. 8-Layer Through-Hole Board 1.0mm Thickness Impedance Design

According to the stackup design parameters shown in Table 1-5, use the Huaqiu DFM software for impedance calculation. The calculation method is the same as for the above 8-layer 1.6mm through-hole board, and the impedance line widths and spacings calculated are shown in Table 1-6.

Table 1-6 8-Layer Through-Hole Board 1.0mm Thickness Impedance Design

8. 10-Layer 1st Stage HDI Board 1.6mm Thickness Stackup Design

In the 10-layer 1st stage board stackup design, the reference plane for the top layer signal L1 is L2, and the reference plane for the bottom layer signal L10 is L9. The recommended stacking is

TOP-Signal/Gnd-Gnd/Power-Signal-Gnd/Power-Gnd/Power-Gnd/Power-Signal-Gnd-Bottom, where L1, L2, L9, and L10 are recommended to be 1 oz, and other inner layers are recommended to be HoZ. As shown in Figure 1-13 is the reference stackup for 1.6mm board thickness.

Figure 1-13 10-Layer 1st Stage HDI Board Stackup Design

9. 10-Layer 1st Stage HDI Board 1.6mm Thickness Impedance Design

According to the stackup design parameters shown in Figure 1-13, use the Huaqiu DFM software for impedance calculation. The calculation method is the same as for the above 8-layer through-hole board, and the calculated single-ended impedance line widths and spacings are shown in Figure 1-14, and the differential impedance line widths and spacings are shown in Figure 1-15.

Figure 1-15 10-Layer 1st Stage HDI Board Single-Ended Impedance Design Diagram

Figure 1-16 10-Layer 1st Stage HDI Board Differential Impedance Design Diagram

10. 10-Layer 2nd Stage HDI Board 1.6mm Thickness Stackup Design

In the 10-layer 2nd stage board stackup design, the reference plane for the top layer signal L1 is L2, and the reference plane for the bottom layer signal L10 is L9. The recommended stacking is TOP-Gnd-Signal-Gnd-Power-Signal/Power-Gnd-Signal-Gnd-Bottom, where L1, L2, L3, L8, L9, and L10 are recommended to be 1 oz, and other inner layers are recommended to be HoZ. Figure 1-17 is the reference stackup for 1.6mm board thickness.

Figure 1-17 10-Layer 2nd Stage HDI Board Stackup Design

11. 10-Layer 2nd Stage HDI Board 1.6mm Thickness Impedance Design

According to the stackup design parameters shown in Figure 1-17, use the Huaqiu DFM software for impedance calculation. The calculation method is the same as for the above 8-layer through-hole board, and the calculated single-ended impedance line widths and spacings are shown in Figure 2-18, and the differential impedance line widths and spacings are shown in Figure 1-19.

Figure 1-18 10-Layer 2nd Stage HDI Board Single-Ended Impedance Design Diagram

Figure 1-19 10-Layer 2nd Stage HDI Board Differential Impedance Design Diagram