HDMI flat cable extender design troubleshooting - Page 1
Forum section: electronics / projects

author: silviustro
author_rank: Contributor
timestamp: November 25, 2017, 10:53:33 pm
content: Hello everyone!I am currently designing a board that requires extending an HDMI connector from one board to another. My idea was to use a flat flex cable to extend the HDMI, I've seen it done before in products like this one:https://www.alibaba.com/product-detail/HDMI-Mini-Right-Angle-Flat-Ribbon_60473623769.htmlI designed both the board that plugs into the source board and the receiver board. There are no electronics in between, the traces on the PCB are meant only for extending the connector from one board to another. The FFC connectors are 0.5mm pitch and the traces are 0.25mm wide (about 10 mil). I measured the distance between the traces, keeping in mind we're dealing with differential signaling, and they're about 99% the same length.I soldered the connectors by hand, checked them under a microscope and did a continuity test. Everything seemed fine. Even tough extender works a little in one TV, there is significant glitching and snow on the screen. Other screens i tested it on didn't even display anything.I wanted to know if there is a major flaw in my design i'm overlooking. Or if i just did a bad soldering job and just need to try again or use a reflow oven instead. Maybe the solder flux residue is causing this?Any input would be appreciated.

author: Ian.M
author_rank: Super Contributor
timestamp: November 25, 2017, 11:17:19 pm
content: With a single ground at one side of the flat flex, that's totally FUBARed and NFG. You need controlled impedance traces run in pairs, which would mean a custom double sided flat flex with a ground plane. See:https://ez.analog.com/docs/DOC-11303You *MAY* get something usable (but not to spec) if you add a ground in the off-the-shelf flat flex between *every* TDMS signal pair and the next one, and between all other individual signals.

author: silviustro
author_rank: Contributor
timestamp: November 25, 2017, 11:49:21 pm
content: Thanks for the reply.Because I am extending the HDMI connector pin for pin, there is a TDMS ground in between every pair. The last pin on the FFC is just connected to the connector ground.While making a prototype for this board I hand wired 20 thin cables from one side of the board to the other, and the screen displayed the image no problem. So i didn't think i would need to change the design when implementing the FFC.My question is, what would be the difference between me doing this on a PCB with a Flat Flex Connector, and someone doing it with a flat cable? I mean, i'm essentially creating a cable from one side to the other.Sorry if my questions seem dumb, I haven't worked with HDMI signals before. I have read about the controlled impedance, but I didn't understand how to calculate it in PCB design very well.Which would be the safest and best way of achieving what I want without introducing so many variables into the design of the PCB? would using a ribbon or a normal cable be better?I looked up how these extenders work:https://www.adafruit.com/product/3551And they seem to be using standard Flat Flex cables, nothing special or custom, they even chose the same FFC type I'm using.

author: nuno
author_rank: Frequent Contributor
timestamp: November 26, 2017, 02:24:58 am
content: I've seen and successfully replicated similar things. The GND pins go (via) immediately to the opposite side of the board at the connectors - otherwise you're notgiving a symmetrical distance from the GND line to both differential pins, one will be closer than the otherkeeping differential lines close together and are having them close to other signals. Add a few vias as "guards" on both sides (left and right) of the traces - GND plane on both sides of the board.The flat cables I've seen being used for board-to-board HDMI are composed of micro-coax cables, meaning each pin's signal travels inside a coax cable. These cables have no shielding, just the tiny "wires", one per pin (each "wire" is a full coax cable!).update: gnd spacing was not what I meant to say

author: silviustro
author_rank: Contributor
timestamp: November 26, 2017, 03:11:38 am
content: Thanks for your reply nuno.I have read a lot of HDMI PCB design since posting my first thread. The "micro coax cable" ribbon cable you mention is quite interesting, but a bit out of my price range and complexity.I've seen this done successfully with standard flat flex. I only need to extend about 15cm of signal from one board to another. Never thought it'd be such a headache....I will design a new "draft" board with what both you and Ian suggested (keeping signals close and putting a ground in between TMDS pairs) and report back with my design.Thanks again for your feedback.

author: silviustro
author_rank: Contributor
timestamp: November 26, 2017, 03:25:01 am
content: After taking into consideration the suggestions above, this is the new board layout i have come up with.I put one signal shield in between each TMDS pair, so they're essentially "sandwiched" together in there.Any feedback would be appreciated

author: nuno
author_rank: Frequent Contributor
timestamp: November 26, 2017, 03:49:12 am
content: If you put the GND vias underneath the connector (route "back" instead of forward) you'll have the signal pairs close for more of the path length.I would do a continuous GND plane on the back. With a full plane, electrons will pick the best pathNot sure if better to keep the S+.GND.S- pattern on the flat cable connector (asymmetric distance from the signal lines to their respective GND line on that cable) or as you have with a GND line separating 2 lines of different signal pairs (crosstalk). Maybe you'd need to keep the S+.GND.S- pattern and add one unused pin between pairs to add distance. There's Gbits traveling on these lines.More top GND to bottom GND vias (say 5 each side), and can be closer to the lines (say inside the connector's area).

author: silviustro
author_rank: Contributor
timestamp: November 26, 2017, 04:06:55 am
content: Thanks once again for your reply.I was checking the Texas Instruments HDMI layout guide, and noticed they link all shields together to ground.Unfortunately there are not enough pins to keep the S+, GND, S- pattern and add one unused pin between pairs. Just two of the 20 pins are unused.I chose the GND, S+, S-, GND layout because i thought the signals should be close together, as mentioned in various design guidelines. To be honest, i don't really know which one is best.I've attached my new layout, once again, any feedback will greatly be appreciated!

author: nuno
author_rank: Frequent Contributor
timestamp: November 26, 2017, 05:05:23 am
content: Ok, looks nice to me.Mind the top/bottom planes sides stitching with vias.Then let us know how things worked out.

author: silviustro
author_rank: Contributor
timestamp: November 26, 2017, 05:59:53 am
content: I still gotta design the male HDMI board as well! But I'll use the same guidelines.I will then order the boards and tell you guys how it worked out.Thanks again for the help!