2
\$\begingroup\$

I have a 6 layer FR4 PCB, and want to achieve 100ohm impedance on HDMI differential pairs. I am only using top and bottom layer for differential pairs, and following are my parameters: Trace width= 3.75mils Trace gap: 12mil Trace thickness: 1.4mil Dielectric Constant Er: 3.8-4.2 (taken from PCB manufacturer) I am not sure what the Dielectric thickness would be. My PCB has a thickness of 62mil, but I am not sure if that is considered dielectric thickness or not.

I have tried different online calculators and none of them are close to 100ohm differential impedance.

I would really appreciate your suggestions! Thank you

\$\endgroup\$
1
\$\begingroup\$

With the track and gap parameters you have, you won't get 100 ohms differential impedance with any standard (if any at all) core / prepreg thicknesses.

You will need to make the gap much less and widen the traces somewhat. I don't use less than 4 thou track widths due to the fact that a minor etching issue can introduce errors that are a large percentage of the track width.

Some numbers that work:

Track width 4 thou, track separation 4 thou, depth to plane 6 thou on 1 oz copper gets you pretty close according to the Saturn PCB toolkit.

These are all pretty standard values for PCB design.

Notes on coupling.

Tightly coupled pairs (within a pair) are quite common and this has the advantage of having a somewhat higher single ended impedance on a per track basis within a differential pair which is often easier to implement. 100 ohm differential pairs that are tightly coupled have a typical single ended impedance of around 65 ohms.

Loosely coupled pairs have a single ended impedance of half the differential impedance.

This coupling is not the same as pair to pair coupling (where a decent gap is required).

There are a lot of values that would work, and a great deal depends on the specifics of the core / prepreg material used by the vendors as the dielectric constants for prepreg (in particular) varies widely by manufacturer. If I ask 3 PCB vendors for suggested geometries I will usually get 3 different answers.

\$\endgroup\$
  • \$\begingroup\$ If I reduce the track separation to 4mil, wouldn't that cause coupling problems? Isn't there a rule for high speed signals to have more than 2x separation than the track width? \$\endgroup\$ – Sam Mar 5 '19 at 16:08
  • 1
    \$\begingroup\$ @Sam isn’t coupling a problem for independant signals? Here, you have a differential pair; that’s not a pair of independant signals. \$\endgroup\$ – user2233709 Mar 5 '19 at 16:29
  • \$\begingroup\$ I apologize! This is my first time laying out a PCB with differential pairs, so I am not aware of all these rules. So I should be good with 4mil width and a 4mil gap? \$\endgroup\$ – Sam Mar 5 '19 at 16:37
  • \$\begingroup\$ Updated answer with notes on coupling. \$\endgroup\$ – Peter Smith Mar 5 '19 at 16:56
  • \$\begingroup\$ What's a 'thou'? It's advisable to use common units, preferably SI. \$\endgroup\$ – asdfex Mar 5 '19 at 19:12
1
\$\begingroup\$

You are missing the most important parameter here, which is the thickness of the dielectric between the layer 1 and 2 and the one between layers 5 and 6.

The only ones who can help you is the PCB manufacturer, who will give you these values based on what material they have in stock. The alternative is for you to specify the thicknesses, but it is most likely to cost you much more and take much longer, if the manufacturer doesn't have the material in stock.

Once you have these values, you can calculate the tace widths with free tools such as Saturn's PCB toolkit.

\$\endgroup\$
  • \$\begingroup\$ I will get the dielectric thickness and will calculate again. Thank you \$\endgroup\$ – Sam Mar 5 '19 at 16:06
  • \$\begingroup\$ PCB manufacturer gave me thickness of 3.5mil between layer 1 and 2, and 3.5mil as well between layer 5 and 6. So in Saturn, do I add 3.5 as Conductor height or do I add 7? \$\endgroup\$ – Sam Mar 8 '19 at 14:55
  • \$\begingroup\$ you add 3.5, as you are looking at one layer pair at the time. As the board is symmetrical, the track width and spacing will be the same for both the top and bottom side of the board. \$\endgroup\$ – Elmesito Mar 8 '19 at 15:17
  • \$\begingroup\$ Based on that, my initial trace width of 3.75mil with a spacing of 12mil gives 92ohm differential impedance. \$\endgroup\$ – Sam Mar 8 '19 at 15:28
  • \$\begingroup\$ I would like to add.. my differential pair traces go from top to bottom and then bottom to top layer per signal. Even then it would be 3.5mil? \$\endgroup\$ – Sam Mar 8 '19 at 15:29

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.