I was looking at an example board schematic provided by TI and I noticed something rather curious: vias were placed directly on SMD pads.
Is this a normal/acceptable practice to follow, or is it recommended/better to put a short trace and then have a via?
Example:


Vias in the pads are useful in high speed designs since they reduce trace length and therefore inductance (i.e. the connection goes straight from pad to plane rather than pad-trace-via-plane)
You have to check whether your PCB house can do this though, and it may cost more (via will need to be plugged and plated over to provide a smooth surface) If you can't put the via in the pad, putting directly adjacent and using more than one can help reduce inductance.
They are also useful for Micro-BGA designs, where space is very limited and traditional fanout techniques cannot be used.
A via-in-pad (or capped/plated via) is not to be confused with a "tented via", which is a standard via with soldermask covering the hole (hence "tented")
To illustrate the advantage, here is an example of a TQFP footprint fanout with standard vias and via-in-pads:

It's easy to see why the via-in-pad version is preferable for high speed designs that need to keep inductance low.
The reason it's more expensive is due to the complex process (compared to standard vias) and potential problems (e.g. plating bulging with expansion of plug, or dimpling)
This document discusses various plugging techniques.
Here is a run through of the process:








