Learning Forum

[prashant kumar jha]

i am modelling heat and mass transfer inside 2 dimensional thermosyphon using axisymmetry. I am using VOF model with two phase,i.e.,liquid and vapor.There are mainly three sections namely evaporator,adiabatic and condenser.I patched liquid i.e., volume fraction=1 in the evaporator section .while running calculation floating point exception appears.

[pawar002]

check the Courant number.  courant number ≡ u*?t /?x  try to use lower timestep ?t=0.0005

[Karthik R]

Hello,

Does the floating point exception error occur at the beginning or in the middle of the simulation?

You might also want to double check the boundary conditions. As recommended by Pawar002, you might want to calculate the Courant number to check for solution stability. If you are still unable to get your simulation to work, please post details explanation of your problem, along with images describing your boundary conditions.

Thank you!

Best,

Karthik

[prashant kumar jha]

here ,i am posting images .Please find the same

[DrAmine]

Do not forget to patch the right temperatures for the pure vapor and pure liquid sections. Please try first of all to use a pure implicit and diffusive scheme as required by the diffusive evaporation-Condensation process (just select implicit in Multiphase Panel and use option Sharp/Dispersed for Regime). In Solution methods Bounded second order in time, Coupled and try to start very conservative with the time step size. Very important is to use the most actually release here. Do not forget gravity and set the operating density to the one of the vapor phase. Here check the materials of both phases and ensure that the difference between standard state enthalpies time divided by molar mass is equal to the well know latent heat at the reference pressure.

[prashant kumar jha]

[DrAmine]

Do not forget to patch the right temperatures for the pure vapor and pure liquid sections. Please try first of all to use a pure implicit and diffusive scheme as required by the diffusive evaporation-Condensation process (just select implicit in Multiphase Panel and use option Sharp/Dispersed for Regime). In Solution methods Bounded second order in time, Coupled and try to start very conservative with the time step size. Very important is to use the most actually release here. Do not forget gravity and set the operating density to the one of the vapor phase. Here check the materials of both phases and ensure that the difference between standard state enthalpies time divided by molar mass is equal to the well know latent heat at the reference pressure.

 

Best regards,

Amine

[prashant kumar jha]

finally got rid of the floating point exception.As i am validating my results with a research work.Can anyone tell me how to select time step size,no. of iteration and courant no. along with its physical significance?

[DrAmine]

 A rough estimation will depend on the physics included:

Due to gravity: delta_t=/(elevation/g)^0.5

Due to surface tension: delta_t=(Mixture_Density*(Min Edge of a Cell)^(1/3)/(4*Pi*surface Tension))^0.5

Due to viscosity: delta_t=Density*(Min Edge of a Cell)^2/(2*viscosity)

General due to flow: delta_t=(Min Edge of a Cell)/velocity

A minimum of all time steps might be a good started (scaled by 0.1 or something).

Note more then 20 iterations per transient (perhaps quite more at the beginning)

Go for adaptive time stepping to have automated adaption and disable convergence by residuals to run at least 5 iterations per cycle

 

More details are included in the Theory manual