I’m working on a 6-layer FR4 PCB and need to achieve 100-ohm impedance for HDMI differential pairs. I’m using only the top and bottom layers for these differential pairs, and here are the parameters I have so far: Dielectric constant (Er): 4, Trace width: 3.8 mil, Trace thickness: 1.4 mil and Trace gap: 12 mil.
I’m uncertain about the dielectric thickness. The overall PCB thickness is 62 mil, but I’m not sure if that refers to the dielectric thickness or something else. I’ve tried several online impedance calculators, but none of them seem to give me a value close to 100-ohm differential impedance. Any advice on how to calculate or adjust the design to meet the 100-ohm impedance requirement would be appreciated!
With your current track width and gap parameters, achieving 100-ohm differential impedance will be challenging using standard core or prepreg thicknesses. You’ll need to reduce the gap between the traces and slightly increase the trace width to get closer to your target. I typically avoid trace widths below 4 mil, as even minor etching issues can introduce significant errors relative to the trace size. For reference, a combination that works well is a 4 mil trace width, 4 mil trace separation, and a 6 mil depth to the plane with 1 oz copper. You can confirm this with any online tools. These are pretty standard values for PCB design, and they should help you achieve the desired impedance.
Regarding coupling, tightly coupled pairs are common, and they have the advantage of a slightly higher single-ended impedance per trace within a differential pair, which is often easier to implement. For 100-ohm differential pairs, tightly coupled traces typically result in a single-ended impedance around 65 ohms. Loosely coupled pairs, on the other hand, have a single-ended impedance that is half the differential impedance. Also, remember that pair-to-pair coupling is different—make sure you leave enough spacing between pairs to avoid unwanted interaction.
Lastly, different PCB manufacturers may give you different suggestions based on their core/prepreg materials, as dielectric constants can vary widely, especially for prepreg. It’s always a good idea to consult with your vendor for recommendations based on their specific materials.
The crucial detail you’re missing here is the dielectric thickness between layers 1 and 2, as well as between layers 5 and 6. This thickness directly impacts the impedance, and without knowing these values, it’s difficult to achieve accurate impedance calculations.
Your PCB manufacturer is the best source for this information, as they can provide the specific dielectric thicknesses based on the materials they have in stock. Alternatively, you could specify the thickness yourself, but keep in mind that this could increase costs and lead times if the required material isn’t readily available. Collaborating closely with your manufacturer is key to ensuring you meet the 100-ohm impedance target efficiently.
The impedance is determined by these factors:
(1) Dk of material (prepreg or core) between signal layer and the adjacent plane
(2) Thickness of the prepreg or core
(3) Width of the traces used in the differential pair
(4) Gap width between the pair
(5) Thickness of any solder resist over the top of the pair
It assumes that there will be a significant distance between the pair and any other metal structures. Usually go with a gap greater than 3x the gap between the pair.
There are a few other things that might be useful:
(1) Stack-up.
(a) Signal/Power - GND - Signal/Power - Signal/Power - GND - Signal/Power: best if you have a lot of interconnections to make in a small space.
(b) Signal/Power - GND - Power - Power - GND - Signal/Power: best if you have more space than above.
In both of the above, best results come if the prepregs/cores immediately adjacent to the GND copper are thin (say 0.1mm). The core right at the centre of the board should be the only thick core to minimise coupling between the layers on either side (and maximise the coupling with GND).
The worst layer stack is this:
(a) Signal - GND - Signal - Signal - Power - Signal
The EMC lab will prove why this is never a good choice. But if this is what you actually do, remember that the HDMI signals that come from the bottom of the board will all have been referencing the power plane, but the shielded HDMI cable references everything to GND, therefore you must makes sure that you have local decoupling capacitors very close to the connector pins to link the power layer to GND and so complete the displacement current paths for both signals in the pair.
Giving your stackup and layer thicknesses to the PCB supplier and getting them to give you the precise stack-up details is the safest way of getting the dimensions right for the 100 Ohms impedance. If you don’t do it this way, there are online tools that can help but make sure you include all the factors. The one that is easiest to miss is that real boards usually have a solder resist layer, and that layer does affect the impedance.
For precise impedance control, I recommend using our Sierra Circuits impedance calculator It allows you to input detailed parameters, such as dielectric thickness, copper weight, and trace geometry, to fine-tune your design. This tool also helps in selecting appropriate trace and gap adjustments based on the material stack-up provided by your PCB manufacturer, ensuring that you meet your 100-ohm target.
Feel free to experiment with the values and work closely with your manufacturer to get the dielectric thickness or stack-up details for more accurate impedance calculations.
the exact trace width and trace gap that you have mentioned may or may not be achieved. the main reason is the dielectrics provided by material manufacturer do not have all the thickness. they only have discrete values.
I have uploaded a couple of calculations from our impedance calculator with some assumptions about the dielectric information.
