
[Sponsors] 
Temperature profile with isothermal steady state simulation 

LinkBack  Thread Tools  Search this Thread  Display Modes 
November 6, 2019, 08:22 
Temperature profile with isothermal steady state simulation

#1 
New Member
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 14 
Hello everybody,
I would like to do a steadystate simulation with an AungierRedlichKwong fluid model. I have a temperature distribution, i.e. a function Temperature(x, y, z) that was measured in a test rig (actually, it does not matter. It could be the result of another simulation or something else). Now I want CFX to use this temperature distribution. Every time I insert an expression into the "Fluid Temperature" field in Details of Domain > Fluid Models > Heat Transfer, CFX complains that only a constant value or an expression evaluating to a constant is allowed. Is there a way to specify a temperature distribution for a steadystate, isothermal simulation? The problem is that I need to match the measured temperature distribution, but I do not know any heat fluxes at the walls. Thank you for your answers, Sincerely, Procyon 

November 6, 2019, 08:44 

#2 
Senior Member
Alexander Karachun
Join Date: Nov 2015
Location: Mykolaiv, Ukraine
Posts: 239
Rep Power: 10 
"Isothermal" mean that temperature remain constant in domain and time and there are no heat transfer. Change Domain Heat Transfer model to Thermal Energy or Total Energy to be able to use temperature distribution.


November 6, 2019, 09:16 

#3  
New Member
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 14 
Quote:
Actually I just want the solver to evaluate fluid properties (density, viscosity, etc) at a prescribed temperature T(x,y,z) that varies with position and not at a constant temperature T. That only allows me to set an initial temperature distribution. The Temperature distribution in the domain will immediately change unless heat flux boundary conditions match the conditions in the test rig. But since I do not know the heat flux boundary conditions, this is not possible, or involves a lot of trial and error. 

November 6, 2019, 09:38 

#4 
Senior Member
Alexander Karachun
Join Date: Nov 2015
Location: Mykolaiv, Ukraine
Posts: 239
Rep Power: 10 
1) Plz. read definition of term "isothermal". Domain will have single temperature. There is no variation of temperature in space. OK?
https://en.wikipedia.org/wiki/Isothermal_process 2) If you know only initial temp. distribution then you can only calculate transient problem and observe how temperature change over time. SteadyState mean that time is infinite and temperature will change to value affected by BC setting, you can use different initial distribution, result will be the same. 

November 6, 2019, 10:21 

#5  
New Member
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 14 
Quote:
The point is, in an isothermal simulation the energy equation is not solved and the temperature field is not a result of the calculation. The temperature is needed only to calculate fluid properties. Therefore, it does not matter to the solution procedure if the temperature is constant or if it varies with position. Ansys could have easily implemented this feature. If they did, then the term "isothermal" would be misleading, and "prescribed temperature field" would be much more accurate. My question was whether there is a (hidden?) way to prescribe a temperature field. 

November 6, 2019, 14:24 

#6 
Senior Member
Join Date: Jun 2009
Posts: 1,688
Rep Power: 29 
It is not a good idea to mix vocabulary based on behavior.
Isothermal means the same temperature in the domain; therefore a single value must be provided. The models that provided temperature variation are Thermal Energy/Total Energy. Therefore, you must select one of them. Now that you have the ability to provide a temperature profile, you want to freeze the solution just after the initial value has been provided, and before the solution of the heat transfer model starts. you can realize that behavior by Use Thermal Energy option Initialize using Automatic with Value = YourTemperatureProfile Inset the Solver/Expert Parameters panel, and choose "solve energy = f" in the appropriate tab. You should get the behavior you want. Now you have to be very careful the solution makes any sense since you have removed the ability to satisfy energy conservation. 

November 11, 2019, 12:06 

#7  
New Member
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 14 
Quote:
Thank you! This is exactely what I was looking for! 

Tags 
isothermal flow, steady state, temperature distribution 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Domain Reference Pressure and mass flow inlet boundary  AdidaKK  CFX  75  August 20, 2018 05:37 
Convergence in steady state simulations vs transient ones  cardioCFD  CFX  5  January 21, 2018 10:59 
How to split a steady state simulation  streamline90  OpenFOAM Running, Solving & CFD  8  October 19, 2017 15:55 
Averaging during a steady state simulation  say  CFX  3  November 3, 2015 09:18 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 03:32 