October 3, 2018 at 4:27 pmprashant kumar jhaSubscriber
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.
October 3, 2018 at 6:19 pmpawar002Subscriber
check the Courant number. courant number ≡ u*?t /?x try to use lower timestep ?t=0.0005
October 4, 2018 at 12:54 amKarthik RAdministrator
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.
October 4, 2018 at 7:38 am
October 4, 2018 at 7:47 amDrAmineAnsys Employee
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.
October 4, 2018 at 7:49 am
October 4, 2018 at 8:12 amDrAmineAnsys Employee
October 5, 2018 at 10:28 am
October 5, 2018 at 11:01 amDrAmineAnsys Employee
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
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.