Search FAQs on the left to see if your question has been answered. Click on the dropdown to view all of the documents associated with the product. If you can't find your question, click on Ask a Question

HDMI Layout Guideline


This FAQ presents a general guideline to laying out HDMI traces on circuit boards.  Many of the problems we see in the forum threads can be traced back to routing and layout issues.  The rules and notes I present here have been gleaned from various boards I have designed and seen over the years.  I can not reference back to the original sources for this information however simple web searches will reveal many documents covering this topic.


HDMI 1.4b specification defines signaling up to 3 GHz requiring board designers to be very careful with HDMI signal integrity during layout.  Following is a good set of rules that will allow you to transmit 3 GHz across FR-4 PCBs.


First Some Math

Let's assume we have a transmitter routed to a connector and we want to transmit a format with 297MHz clock rate.

  • Tbit = time duration for a single bit across a TMDS channel
  • Tcharacter = 10 x Tbit
  • CLK = 297MHz
  • Data = 10 x CLK
  • Propagation Delay for FR4 ~= 6.67ps/mm
  • Intra-pair skew = 0.15 Tbit
  • Inter-pari skew = 0.20 Tcharacter


  • Data rate = 10 x 297MHz = 2.97GHz = 336.7ps
  • Intra-pair skew in time = 0.15 x 336.7ps = 50.50ps
  • Intra-pair skew in distance = 50.50ps / 6.67ps/mm = 7.57mm

Layout Rules

Layout is key.  The following is a general set of rules that has become part of my layout specification for boards.  They are a bit tighter then the math above indicates but are easily met during layout.  These rules can be added directly as constraints to your schematic or as part of the layout specification document.

  1. Each HDMI channel is comprised of 4 TMDS pairs.
  2. Each HDMI channel set shall be routed primarily on the top or bottom layer as a group or alternately routed as a group on internal layers.
  3. Each TMDS signal shall have single ended impedance of 50 Ω ± 10%.
  4. Each TMDS pair shall have differential impedance of 100 Ω ± 5%.
  5. Signals within a TMDS pair shall have matching lengths of ± 3mm.
  6. Signals within a TMDS pair shall not have any 90 degree corners. Corners shall be chamfered.
  7. TMDS signal chamfer length to trace width ratio shall be 3 to 5.
  8. TMDS signal distance between bends should be 8 to 10 times the trace width
  9. TMDS pairs in each HDMI channel shall have matching lengths of ± 3mm.
  10. TMDS pairs shall be separated from adjacent TMDS pairs by a minimum of 1.2 mm.
  11. TMDS pairs shall be separated from adjacent non-pair signals by a minimum of 7.8 mm.
  12. HDMI channel sets shall be separated from other HDMI channel sets by a minimum of 7.8 mm.
  13. HDMI channel sets shall be referenced to an adjacent solid ground plane.
  14. If a HDMI channel set must transition to another reference ground plane then ground plane to ground plane vias must be added adjacent to the channel transition vias.

Fabrication Notes

The following is a general set of instruction notes placed on the PCB fabrication drawing.  They allow the PCB fabricator to tweak the gerbers to match their process and materials.

  1. Characteristic impedance of all signal layers to be 50 Ω ± 10%
  2. Differential impedance of 0.127 mm traces with 0.192 mm gap shall be 100Ω ± 10%.  Vendor may adjust trace widths, trace spacings and dielectric thickness as required. (this note is for the TMDS pairs only, extra information may need to be passed on to the fabricator to indicate exactly which traces are part of a HDMI channel set)

How to handle reference plane transitions

Analog Devices HDMI components are designed so routing is a straight shot from the device pin to the connector pin.  However sometimes you need to change layers the HDMI routing is done on, often changing the reference ground plane in the process.  The transition vias should be symmetrically placed in the path and ground to ground vias to handle the signal integrity of reference plane jumping as illustrated below

This particular example is from an eight layer board, the red trace is on the top layer, the blue trace is on the bottom layer and the dark green layers are the solid ground planes adjacent to the top and bottom layers.  Note that the vias are place symmetrically in the path and separated by 1.14mm.  Also note the 2 ground vias adjacent to the 2 trace vias.

In this example if the differential pair jumped from layer 1 to layer 3, no ground to ground vias would need to be added since you are not jumping reference ground planes.

It is best to keep the number of differential pair vias to a minimum since each via introduces impedance changes.

It is also a good idea to stitch ground to ground vias along the trace path every 2 cm or so.  This aids in general signal integrity control.

How far can you go?

Normally HDMI traces on boards are very short, directly from the connector to the receiver/transmitter.  Many times we get the question of how long can I make HDMI traces.  The HDMI specification does not define maximum length, only expected impedance.  As long as you follow the layout rules above you should be able to run HDMI traces over 20-30cm easily.  Longer if you are careful.


ESD Protection

ESD protection devices are often added to increase ESD protection levels.  I suggest devices with signal flow through like Semtech RClamp0524.  They allow HDMI signals to flow directly under the part while providing low capacitance ESD protection.  There are many vendors producing these types of low capacitance TVS arrays.


HDMI Differential Routing Example

Here's an example HDMI routing from a horizontal HDMI connector on the left to an ADV7850 receiver port. 

Things to Note:

  • Smooth flow through from connector through ESD protection and to the ADV7850
  • Jog in TMDS pair used to equalize pair to pair lengths
  • Pair to pair separation where feasible
  • Pair to non-HDMI channel signal separation


The Big Picture

Designing a HDMI transmitter or receiver board is just part of the of the whole system.  You must always keep in mind that you are often connecting through a cable to a source/sink.  The connection from the board to the cable and from the cable to the source/sink are transition points.  Most HDMI connectors are 100 Ω ± 15% and cables have attenuation proportional to the length.  Poor transition points can cause reflections causing poor signal integrity.  Long cables will attenuate signals decreasing the swing voltage at the receiver dropping the received signal out of specification.  All these problem become more prevalent at higher resolution like 1080p or 4K.

Analog Devices Inc provides many reference board designs from which you can copy layouts from.

I recommend using signal integrity tools to verify HDMI trace layouts meet specifications.


  • These guidelines are what I use designing HDMI circuit boards.  They are not intended to be definitive in any way but are intended to aid other designers understanding what to do and look out for.


  • High-Definition Multimedia Interface 1.4b
  • DVP PCB Layout Recommendations (??need link??)