That’s the pads you want… I’d not do the small bite-outs in the corners for the mounting plate fixing pads.
And this is a footprint from me for a FPC 0.5mm connector from TE I did some time ago (ignore the pin#1 marker under the footprint, bad practice):
Make sure that if you use the version where the lever COMES OUT to mark that space as a keep-free zone in your footprint and also draw in the FPC (end position inside the connector - insertion depth - and width/path outside of it for some length) - all so you don’t place other components in that area.
The insertion depth is useful once you want to specify the FPC length
for above footprint:
yellow - Cmts.User (I use this layer for collission information after assembly/during use)
light grey - F.CrtYd (contains the extended lever for this particular connector as there really should nothing be in that space ever, the FPC can probably go over flat SMD parts past that area, your pdf specifies 0.96 mm from top of board to center of FPC)
Also note that by my personal nomenclature your connector would carry a TOP in the name, depicting that the contacts on the FPC will be made on the top and not on the bottom. This might be important information down the road as this (together with the counterpart on the other board) will decide what kind of FPC you need… contacts on same side or other sides
PS: personal tip - make 100% sure you connect the correct pins from one board to the other, taking into account the flipping over of the FPC or any other stuff. Really think 3 times here and don’t be afraid to use paper+scissors to create a real life model (pin#1 markers for each end + side of connections) to make sure you got it right.