# flue gas condensation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 March 31, 2020, 07:42 flue gas condensation #1 New Member   Jay Join Date: Mar 2020 Posts: 3 Rep Power: 6 Problem statement: A flue gas is flowing inside a horizontal tube with certain mass flow rate and temperature. Cold air with a certain temperature is passed over tube in cross flow arrangement. Desired output: Variation of condensate mass flow rate over the entire length of tube. Inputs: Gas inlet temperature, gas mass flow rate, mass fraction of different species. Length of tube, diameter of tube. Cold air inlet temperature. My setup: 1.Multiphase model: Eulerian , (3Phases) 2.Viscous model-k-epsilon, standard and enhanced wall treatment. 3.Species Transport: ON 4.Coupled interfaces. 5.Boundary Conditions: Inlet: Temperature and mass flow rate of gas and air Outlet: Pressure -outlet. 6.Domains : 1-Inlet gas domain 2-Outlet air domain 3-Tube wall 7. Phases : 1- phase1 - Mixture 2- phase2- Water-liquid 3- phase3- Air 8.Phase interaction : Phase1 (vapor species) to Phase 2(water-liquid); evaporation-condensation Problem facing : 1.In cell zone condition mixture is being defined at inner domain as well as outer domain, but i want only air in outer domain. 2.The solution diverges after 50 iteratios and" floating point error" arrises. It would be helpful if you would guide me through the setup for this problem. :

 April 1, 2020, 04:20 Multiphase Modeling #2 Senior Member     Vinerm Join Date: Jun 2009 Location: Nederland Posts: 2,946 Blog Entries: 1 Rep Power: 36 Fluent does not allow choosing a material for a cell zone when Multiphase model is used. It is mixture everywhere, however, you can restrict it to a particular phase and a particular specie of that phase by initializing with that value. So, if you have air and vapor as one phase and water as second phase, initialize with volume fraction of 1 and mass fraction of 1 for air in the outer domain. This way, you will only have air. You can fix the value of mass fraction to 1 to ensure that it stays so. You do not need to add air as third phase. __________________ Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.

 April 16, 2020, 10:31 Flue gas condensation #3 New Member   Jay Join Date: Mar 2020 Posts: 3 Rep Power: 6 Thank you for the clarification of the doubt. Further i am facing another problem. I know the gas will not condense immediately throughout the tube, first it will reach the dew point temperature, and then it will loose its sensible heat. I have achieved the desired results of variation of mass flow rate with respect to length via coding, but with fluent i am facing following problems: Patching: I assigned water-liquid volume fraction as "0" in the domain. 1. The volume fraction of water-liquid should increase continuously, but in case of fluent simulation, its volume fraction increases for certain length and then decreases to 0. 2.1. The volume fraction of gas mixture should decrease continuously, but in case of fluent simulation, its volume fraction increases for certain length and then increases to 1.

 April 16, 2020, 10:39 Evaporation-Condensation #4 Senior Member     Vinerm Join Date: Jun 2009 Location: Nederland Posts: 2,946 Blog Entries: 1 Rep Power: 36 The phase change model you are using is thermal model, i.e., everything depends on temperature. If the temperature starts rising again due to any reason, the liquid will evaporate again. Also note that densities of water-liquid and water-vapor have a ratio close to 2000, i.e., if vapor condenses, only 1/2000th of the originally occupied volume is required to keep water. If vapor is being modeled as incompressible, it cannot expand to fill the space, hence, leading to pressure reduction, which could lead to re-evaporation if you have provided saturation temperature as a function of pressure. So, vapor or vapor-air mixture, whichever you are using, must be modeled as ideal gas. __________________ Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.

 April 21, 2020, 07:56 #5 New Member   Jay Join Date: Mar 2020 Posts: 3 Rep Power: 6 Thankyou so much sir for your reply. I implemented the same and now the mass transfer rate and VOF are showing the actual trend as per the analytical solution. But the only problem i am facing is the mixture temeprature is changing by only 2K, where it decreases from 300K to 285K. Whereas inlet Temperature of the mixture is 473K. I have triend 2-D steady state and transient simulation also. Their also i am facing the same problem. Expected Problem: It is taking the same temperature with wich it is being initialized that is 300K I am using Hybrid initialization, with patching of Volume fraction of "0",inside the domain. It would be helpful if you clarify the initialisation and patching technique to be used for such problems.

 April 21, 2020, 08:16 Initial Condition #6 Senior Member     Vinerm Join Date: Jun 2009 Location: Nederland Posts: 2,946 Blog Entries: 1 Rep Power: 36 You need to ensure that there is at least a very small amount of vapor initially. So, each phase should have a positive volume fraction. If ideally you want it to be all liquid, start with liquid volume fraction of 0.99999 but vapor of 0.00001 but not 1 and 0. __________________ Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post kevinmccartin CFX 12 October 13, 2022 21:43 AdidaKK CFX 75 August 20, 2018 05:37 cuteapathy CFX 14 March 20, 2012 06:45 Marc FLUENT 0 November 30, 2006 11:44 Dan Moskal Main CFD Forum 0 October 24, 2002 22:02

All times are GMT -4. The time now is 05:58.

 Contact Us - CFD Online - Privacy Statement - Top