SD reader relocation - poor signal integrity?

[zzattack]

I'm trying to relocate a micro-sd slot from an embedded device to a more accessible location on its enclosure.
I have therefore drawn a 0.8mm thick board that slots into the micro-sd slot on the device, and routed the data signals to a 15-pin FPC connector, with trace lengths matched and all traces separated with a GND pour. On the receiving end, traces are kept short as can be toward the micro-sd connector. Both ends are connected through a 15cm AWM20624 FPC flex cable.
While this works, the SD reader must be initialized in HS25 mode to be reliable. The reader is normally able to work at 208MHz.

Unsure how to diagnose, let alone solve this. Am I missing any bad practices? The only improvement I could think of is voltage drop, but on both ends for the VDD to the card this is neglible, so I don't think adding another trace there would help.
Suggestions or ideas are very welcome!

[georgian]

All I can think of is the voltage drop in short bursts. When the µSD card needs a lot of power for very short periods, the power traces can't keep up. You can try and solder a small capacitor in the µSD card socket. If it helps, increase the trace thickness.

[selcuk]

This may be a signal integrity issue. The ground tracks on both sides of the signal tracks cannot act as signal return planes. They are grounded only on one side. Is that a 2-layer PCB? You may use 4-layer, and use two inner layers as ground planes.

You can try to stick a copper tape on the board and ground it on multiple points, and check for any improvements. That will be ground plane of the PCB.

If you have near field probes and a spectrum analyzer, you can observe SD card clock and its harmonics. And you can compare it after adding the plane. Those signal may lead to crosstalk problems.

Additionally, some application notes about sd cards recommend termination resistors to prevent ringing. I don't know whether signal reflections are the problem here. You may consider if you do the layout again.

[wraper]

Add VDD decoupling. Also GND fill between traces with no via stitching to solid GND plane is worse than none of it. You basically put a bunch of antennas between data traces.

[moffy]

My concern would focus more on the 15cm cable than the few mms of PCB trace, not that they aren't important, but that they are so much shorter than the cable. Try the smallest cable you can find and see if it works, and if not what frequency it stops working at. Then try it with a longer cable to see if that makes the problem worse or the same.

[zzattack]

Thanks for the suggestions. I've also picked up a trick where the CLK wire gets a 330 pull up employed on some SD card extenders, will evaluate if that provides any benefit.
 - 4 layers on the board where the actual SD card plugs in
 - via's to ground littered all around the signal traces
 - thicker trace for VDD and using 2 instead of just 1 track on the flex cable
 - decoupling cap near VDD on the slot
 - vias littered around the part that slots into SD connector

Gonna give it another shot. Cheap prototyping is quite nice these days.

[selcuk]

If you haven't ordered, you can add more vias around sd-card slot. You can connect USB connectors' shield to GND. You can widen the tracks between USB GND pad and GND plane. They are barely seen.

[zzattack]

Another update here, proto boards came in. With the suggestions from this topic I retain full speed (UHS-II/156MB/s) with the 20cm extension cord. So great success, thanks all for the help!