Learning Forum

[Elizabeth Laughlin]

Hi!

I was hoping to get some clarification on something that I think may help me with my 2D VOF model. I have a closed system that is driven by the temperature wall boundary conditions (in the bottom of my pipe the temperature is set higher than the top of the pipe). Initially, the bottom half of the pipe (where the wall temperature is set high) has the liquid phase of my fluid and the top half of the pipe (where the wall temperature is set low) has the gas phase of my fluid. I hope to see some of the liquid phase evaporate because of the heat of the wall, and some of the gas phase condense because of the low temperature wall.

I used water as the fluid to start out to make sure my model could work. From the short simulation I have completed (12sec) I can see condensation and evaporation if I set very extreme wall temperatures. I am now trying to run the same evaporation/condensation model for a different fluid (adjusted the pressure and fluid temperatures according to the saturation temperature/pressure curve for the fluid of interest). ANSYS has the material properties defined for the gas phase and I defined the material properties for the liquid phase according to values I found in literature. When I initialize the model I get an error stating that the latent heat cannot be less than zero (I did not get this error when I ran the model with water). 

My understanding is that the latent heat is the difference of the the liquid phase standard state enthalpy and the gas phase standard state enthalpy. I have tried a few variations for the standard state enthalpy I define for my liquid phase; after the value I found in literature for the standard state enthalpy gave the latent heat error, I set the enthalpy to be equal and opposite that defined by the gas phase and on another try I set the enthalpy for the liquid phase to be zero. All attempts I have made give the same latent heat error though with a different latent heat value displayed (even if I check that the difference between the standard state enthalpies of the two phases is positive). 

I noticed that the standard state enthalpy defined by ANSYS for water (liquid phase) is -2.858e+08J/kgmol while the standard state enthalpy defined by ANSYS for water (vapor phase) is -2.418e+08J/kgmol. The difference of the liquid and vapor phase enthalpies in this case is not positive, so I am wondering if I have an incorrect understanding of how ANSYS Fluent defines latent heat?

I ran the model with the fluid other than water dispite the latent heat error warning. The simulation ran for a little time before quitting because of floating point error. When I look at the results there is no condensation or evaporation to be seen. I assume this has to do with the latent heat error warning which is caused by my material property definitions. I think it might be important to mention that I have checked that my mass transfer model is defined with liquid as the "from" phase and gas as the "to" phase.

I know this was long-winded. I appreciate you taking the time to read and offer any help.

Thank you!

[Prashanth]

Hi,

To avoid getting the "latent heat less than zero" warning while using the evaporation-condensation model, you can directly set the latent heat calculated @Tref to the SSE of the vapor phase and set the SSE of the liquid phase to zero. 

[Elizabeth Laughlin]

Thank you for the reply Prashanth!

How do I directly set the latent heat? I do not see a place to define the latent heat in the model anywhere. Do I have to make a UDF to define the latent heat?

I tried to set the SSE of the liquid phase to zero and kept the SSE of the vapor phase as the value defined by the Fluent Material Library (a negative value), and I got the latent heat error again. 

[Prashanth]

The SSE of vapor is higher. So, the difference (latent heat) in the SSE's of both phases is a positive value. Set that value to the SSE of vapor in materials panel. No UDF workaround is required.

[Elizabeth Laughlin]

Thank you, I did not understand that at first. I did not set the SSE to be positive in the material properties. I see evaporation in my model now, but no condensation. I think maybe it needs to run for a longer time.

I have an additional question about how the material properties are defined and how that relates to the operating pressure and operating temperature defined in the physics tab (if they relate at all). When defining material properties we have to include the reference temperature which the properties are defined for, but there is no spot for reference pressure. Does this mean that the ANSYS defined materials from the material library have properties defined for the reference temperature stated and the default operating pressure (1atm)?

My simulation is for a high pressure pipe, and the material properties have different values at different pressures (even if the temperature is the same). So I am wondering if I need to define all the fluids for the pressure I plan to operate at, and how to let ANSYS know that the properties are defined for a specific pressure (like how there is a reference temperature spot for the specific temperature the properties are defined for)?

[Prashanth]

You can also tune the evaporation/condensation model coefficients. For more information, check the docs: 23.2.10.2.5. Evaporation-Condensation Mechanism ;14.7.5. Evaporation-Condensation Model

Set appropriate material property values for the pressure you plan to operate at.