TMDS181: PCB Layout - HDMI Connectors on the same side

Davide Ballo

Intellectual 550 points

Part Number: TMDS181

Hello,

I'm working on TMDS181 layout and I need to place the HDMI connectors on the same side, please see attached photo.

The PCB will be 4 layers.

Can this solution be fine?

Working with video signals is very critical and I wouldn't come across issues due to a wrong pcb layout.

Thanks.

Best Regards,

Davy

over 6 years ago

0 Gerasimos Madalvanos66 over 6 years ago

TI__Intellectual 1350 points

Hello Davide,

We are looking into your issue and will get back to you as soon as we can.

Best,
Gerasimos

0 Davide Ballo over 6 years ago in reply to Gerasimos Madalvanos66

Intellectual 550 points

Hello Gerasimos,

thanks for your reply. I await your feedback.

Best Regards,

Davy

0 Gerasimos Madalvanos66 over 6 years ago in reply to Davide Ballo

TI__Intellectual 1350 points

Hi Davy,

For best results, I believe you should rotate the chip 90 degrees and move it closer to the two HDMI ports to make your traces as short as possible. I would also try to avoid routing other signals under your tx/rx pairs. If you route your signals through vias, I would put stitching vias to ground around your vias. Also make sure your lengths are matched, just from a look they do not appear matched.

Best,
Gerasimos

0 Davide Ballo over 6 years ago in reply to Gerasimos Madalvanos66

Intellectual 550 points

Hi Gerasimos,

thanks for your reply.

I try to apply your advice and I will reply soon.

Thank very much.

Best Regards,

Davy

0 Davide Ballo over 6 years ago in reply to Gerasimos Madalvanos66

Intellectual 550 points

Hi Gerasimos,

what do you think about this solution?

Thanks.

Best Regards,

Davy

0 Gerasimos Madalvanos66 over 6 years ago in reply to Davide Ballo

TI__Intellectual 1350 points

Hello Davide,

This document should help with your layout. Nothing should be placed in between pairs of signals. Does your board have a ground plane? You need to have a ground plane on your board underneath the high speed pairs. The stitching vias should only be adjacent to your vias through the board.

Best,
Gerasimos.

0 Davide Ballo over 6 years ago in reply to Gerasimos Madalvanos66

Intellectual 550 points

Hello Gerasimos,

thanks for the document!

The board has a ground plane which is shown in the picture below.

I follow your advice. I matched the lengths of the differential pairs and removed everything between pairs.

I routed the clock signal 50 mils far from the closer differential pair.

I can't place the stitching vias for all vias because they will be among the pairs of signal.

What do you think about this solution?

Thanks again

Best Regards,

Davy

0 Gerasimos Madalvanos66 over 6 years ago in reply to Davide Ballo

TI__Intellectual 1350 points

Hello Davide,

The last minor tweak I would make is to shift the leftmost lane over on the source to make some more room for those middle two sets of stitching vias. Other than that, looks great.

Best,
Gerasimos

0 Davide Ballo over 6 years ago in reply to Gerasimos Madalvanos66

Intellectual 550 points

Dear Gerasimos,

sorry for my late reply.

I didn't understand the change to do.

Please see attached file, is it correct?

Thanks.

Best Regards,

Davy

0 Davide Ballo over 6 years ago in reply to Davide Ballo

Intellectual 550 points

Hi Gerasimos,

can you confirm that I need to move left the signal pair marked in the picture?

Thanks.

Best Regards,
Davy

0 David (ASIC) Liu over 6 years ago in reply to Davide Ballo

TI__Guru**** 160826 points

Davy

Your understanding is correct, the two middle set lanes currently do not have GND via. So you need to push the left most trace out a bit to create room for the GND via. GND via provides current return path, you want the current return path to follow the signal trace as close as possible. So every time a via is utilized, a ground via should also be utilized next to the signal via. This allows the return current to flow near the signal current flow. If not, current will find way to return, but it will not be the current next to signal trace and this could cause signal integrity problem.

The other issue I am seeing is that the GND via are not placed in equal distance from the signal via. Please see attached for the recommended GND via placement.

Thanks

David

0 Davide Ballo over 6 years ago in reply to David (ASIC) Liu

Intellectual 550 points

Hi David,

thanks for your reply. Please see the attached picture.

Is it ok now?

Thanks.

Best Regards,

Davy

0 David (ASIC) Liu over 6 years ago in reply to Davide Ballo

TI__Guru**** 160826 points

Davy

Yes, now the signal via and GND via look better.

Please double check the TMDS181 land pattern and make sure it follows the recommended land pattern data in the TMDS181 datasheet.

Thanks

David

0 Davide Ballo over 6 years ago in reply to David (ASIC) Liu

Intellectual 550 points

Hi David,

thanks very much for your support and thanks also to Gerasimos.

I've checked the land pattern and it is ok.

Thanks again.

Davy

Interface

Interface forum

TMDS181: PCB Layout - HDMI Connectors on the same side