CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Temperature profile with isothermal steady state simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 2 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 6, 2019, 08:22
Default Temperature profile with isothermal steady state simulation
  #1
New Member
 
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 15
Procyon is on a distinguished road
Hello everybody,


I would like to do a steady-state simulation with an Aungier-Redlich-Kwong 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 steady-state, 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
Procyon is offline   Reply With Quote

Old   November 6, 2019, 08:44
Default
  #2
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
"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.
karachun is offline   Reply With Quote

Old   November 6, 2019, 09:16
Default
  #3
New Member
 
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 15
Procyon is on a distinguished road
Quote:
Originally Posted by karachun View Post
"Isothermal" means that temperature remains constant in domain and time and there is no heat transfer.
I know. The temperature distribution that I want to apply should stay constant and not change with time. It should change with position (x,y,z), not with velocity, pressure, density, ...

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.
Quote:
Originally Posted by karachun View Post
Change Domain Heat Transfer model to Thermal Energy or Total Energy to be able to use temperature distribution.
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.
Procyon is offline   Reply With Quote

Old   November 6, 2019, 09:38
Default
  #4
Senior Member
 
karachun's Avatar
 
Join Date: Nov 2015
Posts: 244
Rep Power: 11
karachun is on a distinguished road
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. Steady-State 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.
karachun is offline   Reply With Quote

Old   November 6, 2019, 10:21
Default
  #5
New Member
 
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 15
Procyon is on a distinguished road
Quote:
Originally Posted by karachun View Post
1) Plz. read definition of term "isothermal". Domain will have single temperature. There is no variation of temperature in space. OK?
I know what isothermal means.


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.
Procyon is offline   Reply With Quote

Old   November 6, 2019, 14:24
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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.
Procyon and karachun like this.
Opaque is offline   Reply With Quote

Old   November 11, 2019, 12:06
Thumbs up
  #7
New Member
 
Procyon
Join Date: Jan 2011
Posts: 8
Rep Power: 15
Procyon is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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.

Thank you! This is exactely what I was looking for!
Procyon is offline   Reply With Quote

Reply

Tags
isothermal flow, steady state, temperature distribution

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 19:18.