# Parameters affecting high-speed PCB transmission line design

I am designing an I/O board for an NVIDIA Jetson Nano SOM module. The board contains the HDMI, USB2.0, CSI, SD card and power system and GPIOs.

So for USB 2.0 90 ohm impedance is required, so I calculated the following:

There I have selected 1 oz copper thickness and FR4 material. My PCB manufacturer has a capability of minimum 0.15 mm spacing and 0.15 mm track width. So after entering all the details, I got 0.77 mm as track width and 0.15 mm as track spacing.

For my reference I have downloaded the official Rpi CM4 IO board Kicad files, which are using 0.15 mm as width and 0.25 mm as gap. I have verified the copper core thickness is 1 oz.

So could you please help me to understand, what's the parameter which is causing the difference in width and gap?

• You're using a two layer board so the traces have to be very wide. On a 4 layer they'd be much smaller due to the extra ground plane. May 5, 2021 at 14:17

The difference is the H value. 60 mil is 1.524 mm, which suggests you are using a standard 2 layer board. For high speed interfaces like the ones you mention, you should use a 4 layer board. That way the reference plane is much closer, so your H value will be smaller. Here's JLC's standard 4 layer dimensions:

And here's their 2 layer:

In the 4 layer stack, the Prepreg value corresponds to H in your software. In the 2 layer stack, the Core value corresponds to H. Try experimenting with the values there, and you'll come closer to the values you've observed on the CM4 carrier board.

• So how can I use this tool to calculate the W and S for 4 layer board ?? May 5, 2021 at 14:21
• Just copy the relevant values your PCB manufacturer provides about their stackup. For example, for the 4 layer one I've linked, you'd set H = 0.18 mm, T = 0.035 mm. I can't see what H_t is on your software's graphic, but cross reference it like the ones I've shown. May 5, 2021 at 14:25
• I received the following stackup details from the manufacture. link. And after putting the prepreg value in "H" get impedance different. Please help what I am doing wrong May 6, 2021 at 9:40
• @Abhishekbhatia Note in your link that they are quoting the Single impedance, not differential. Your $Z_O$ looks wrong, Saturn PCB Design (and some others online) give a value close to the manufacturer's value. May 6, 2021 at 10:04
• Hope by using this stackup details,I can calculate S and W itself from tool and W=17.5 mil and S=5 mils ryt ? May 6, 2021 at 10:21