Thermal Resistance, PCB Operating Temperature and PCB Self Heating
What does Maximum PCB operating Temperature for a PCB in general
  depend upon?


A number of things, Tg is a limiting factor for the laminate (not to destruction but for other reasons - see below) but it is usually the mounted components that limit normal operating temperature as their maximum operating temperatures are usually well below Tg; note that Tg is not a sudden change in most PCB materials and the listed temperature is usually in the middle of the nominal range of temperatures.

There are a number of different laminate materials with differing glass transition temperatures (and may be referenced against a standard).

High reliability designs usually have a 'High Tg' laminate (Tg >= 170C) such as this one (a very commonly used material)

The importance of Tg is during reflow where the temperature will always exceed the nominal Tg for some time (for a Tin Lead process the peak temperature is around 205C to 215C and for lead free using a SAC type solder paste it is between 235 and 250C).

The time above Tg is a key consideration; for products with dense via fields a high Tg is recommended; above Tg the Z axis expansion increases a lot (from typically 35 to 55 ppm depending on material to over 230 ppm); above Tg this puts great stress on the copper via barrels because they prevent Z axis expansion locally which forces the material to expand in the X / Y axes instead and can break vias.

Minimising the time above Tg by using a high Tg material reduces the risk of via damage.

I have seen this happen with low Tg materials and no amount of bare laminate testing will show it up as it is an effect of reflow  - the bare laminate will not have been subjected to these temperature and even 100% netlist testing (which is common) cannot predict this so you end up with defective product only after assembly.

This is not to say you cannot use a lower Tg material, but it does mean you need to evaluate the effect. Most assembly houses can offer advice on the specifics of a particular design.

PCB self-heating is due to the heat from mounted components and from temperature rise on power supply tracks and planes or other high current paths such as backplane drivers (you can find a calculator for that here or get the Saturn PCB toolkit which I personally highly recommend and has much more than just a temperature rise calculator).

When a component heats up due to internal power dissipation, the local PCB temperature will rise; as the thermal conductivity of most types of epoxy laminate is quite low (0.4W / mK from the linked laminate datasheet) (K = Kelvin, m = metre) there will be localised heating - this is the reason many such devices have a metal pad on the bottom of the package to help spread the heat out to copper on the PCB).

For your example, TI has an application report that details exactly how those figures are measured which I am not going to repeat here; an important point is that they use a specific PCB (specific number of layers, specific amount of copper) which will necessarily be different in most cases from the actual application. To get the values shown you need to provide at least the same amount of copper on the indicated layers as the test so always consult the report or the datasheet which will often reference a JEDEC standard PCB from JESD 51).

The junction to ambient thermal resistance is the effective thermal resistance of all possible paths to ambient; there are are series and parallel paths and this is shown in the application report which I highly recommend you read.