I would like to know how the static pressure within the run-process is treated. AFAIK there is a smallest possible absolute pressure, that an element with the set fluid properties can reach. This will be the vapor pressure which is defined for that specific material. Now i would like to know if Simulation CFD will adjust the calculated theoretical pressure (which could possibly drop to a value below zero) at the end of every Iteration or only once at the very last Iteration.
I am thankful for any help
Solved! Go to Solution.
I think that you need to make sure you have entered the vapor pressure of the fluid in "Phase" option. Many of the default liquids (say kerosene etc) have their vapor pressure set. Thus if computed pressure at any point is below the set vapor pressure, it is reset to the vapor pressure, if cavitation is disabled. If cavitation is enabled, these regions will have the vapor phase (in terms of bubbles etc). Aparrently, if vapor pressure is not specified, it is taken as zero.
Now, when cavitation is enabled, the mathematical formulation suggests that at each iteration, the scalar transport equation of volume fraction uses the liquid phase source term which is defined as a function of local pressure (p) and vapor pressure (pv) and also depends on the sign of (p-pv). The volume fraction and subsequently the density is calculated which is further used to solve continuity/momentum equations. This implies that correction is taking place at every iteration and not at the end. This should be true, intuitively, even when cavitation is not enabled but the vapor pressure is non-zero. The only change will be that volume fraction scalar equations are not solved but the low pressures are reset to vapor pressure.
thank you omkar,
I have set the vapor pressure in the material properties, but deselected the cavitation check box in the advanced physics. I know that the minimum static pressure is capped at vapor pressure, but i would like to know, if Simulation CFD
a) just simply swaps the negative pressure values with the vapor pressure at the very end of the simulation
b) resets the negative pressure values at the end of each Iteration and uses those values for the calculation of future solution values
€: well i'd say it is b) intuitively too, but it would be awesome if royce could confirm that
The solver is swapping out the values every iteration for both cases with and w/o cavitation. It is not just a post-processed result of clipping the values. As I recall, if you set the vapor pressure to 0 that will ignore all clipping and allow the pressure to reach a negative absolute pressure.