Suppose after a particular simulation has been done, one wants to use the temperature distribution after that run,as the initial distribution for the second part of the problem with different boundary conditions, how does one go about it?

Menu > Initialisation > Restart for all variables

this will put in FINIT value the word READFI, that means that the new initialisation field will be read from the phi file in your working directory. You have to sure that the size of the grid of your new simulation is of the same size of the phi file that you are reading.

You can make a combination of READFI and other values in this part of the main menu. In some particular cases, with problems of convergence, I start with a kemodel or laminar, then I add temperature starting with the pressure and velocity field obtained from my recently simulation, so it's something like this:

Variable P1 U1 W1 ... TEM1 FINIT Value READFI READFI READFI 50

If you put READFI in TEM1, and your phi file does not have it, the program will initialize it in cero (1.0e-10).

As you may know don't try to start with something like this:

Variable P1 U1 W1 ... TEM1 FINIT Value READFI 1.0 0.0 50

Becuase the pressure and velocity field are linked, and this maybe will take more time that if you start from cero (it depends on your problem).

Good luck

Javier Larrondo "Not an expert, only a user trying to understand Phoenics"

Basically you are solving for the temperature after the velocity field is converged. Without restarting, this can be attained by writing ISWC1=Sweep number in q1 file(this can be given thro' VR-editor also), which means the solution of energy equation will be started after that sweep number. Yes, here you have to know approximately the number of sweeps required for the velocity field to be converged. Good Luck.

Dipak