CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > General Forums > Main CFD Forum

Treatment of temperature using outflow boundary condition in Ansys Fluent

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

Like Tree3Likes
  • 1 Post By aerosayan
  • 2 Post By FMDenaro

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 25, 2022, 07:45
Smile Treatment of temperature using outflow boundary condition in Ansys Fluent
  #1
New Member
 
Join Date: May 2022
Posts: 2
Rep Power: 0
eddie4160 is on a distinguished road
Hi, guys,

I am currently simulating a pipe flow with energy equation as shown in the following figure.

https://www.dropbox.com/s/ecykqukl11...screenshot.PNG

I imposed the outflow boundary condition at the outlet. I wonder what actually happened with respect to temperature at the outlet?

Does Fluent apply the Neumann boundary ∂T/∂n = 0 ? or it extrapolate the temperature from the adjacent cell to the boundary ?

I've read the user manual of Fluent, it only mentions the diffusion flux is zero.

Thanks for your help
eddie4160 is offline   Reply With Quote

Old   May 25, 2022, 08:44
Default
  #2
Senior Member
 
Sayan Bhattacharjee
Join Date: Mar 2020
Posts: 456
Rep Power: 6
aerosayan is on a distinguished road
My guess is, they don't forcefully set the temperature if you don't set a strong boundary condition that specifies temperature, and the outlet temperature is most likely to be calculated from the fluid equations.

The energy is a conserved variable, and thus, it's solved in every cell. So if you don't set a boundary condition enforcing temperature, then ANSYS won't try to enforce it.

In some cases practitioners may need to add a heating element to the boundary, and they'll specify the heat flux as a boundary condition. Such an example would be when you're trying to simulate cooling of a heated pipe, where the pipe wall is hot. That flux would be added as a source term.

So, if you use pressure outlet, or mass flow outlet, boundary conditions, only those specific conditions will be enforced. You can refer to them in the manual about the specific type of boundary condition.

Basically, ANSYS is just solving mathematical equations, and it's possible for us to create a badly defined case with unrealistic intial or boundary conditions, but they try to help us not make mistakes.
eddie4160 likes this.
aerosayan is offline   Reply With Quote

Old   May 25, 2022, 11:23
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,192
Rep Power: 66
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by eddie4160 View Post
Hi, guys,

I am currently simulating a pipe flow with energy equation as shown in the following figure.

https://www.dropbox.com/s/ecykqukl11...screenshot.PNG

I imposed the outflow boundary condition at the outlet. I wonder what actually happened with respect to temperature at the outlet?

Does Fluent apply the Neumann boundary ∂T/∂n = 0 ? or it extrapolate the temperature from the adjacent cell to the boundary ?

I've read the user manual of Fluent, it only mentions the diffusion flux is zero.

Thanks for your help


That implies zero normal derivative.
thedal and eddie4160 like this.
FMDenaro is offline   Reply With Quote

Old   May 25, 2022, 23:00
Smile
  #4
New Member
 
Join Date: May 2022
Posts: 2
Rep Power: 0
eddie4160 is on a distinguished road
Thanks for the fast reply, I've checked the temperature profile along the center line in axial direction with cell center and nodal data as shown in following link:

https://www.dropbox.com/s/ed0a0g136l...58.15.png?dl=0

The total length of my simulation is L=0.5.

It seems like it actually enforces the Neumman boundary at the outlet.
eddie4160 is offline   Reply With Quote

Old   May 26, 2022, 11:49
Default
  #5
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 1,940
Blog Entries: 29
Rep Power: 36
sbaffini will become famous soon enoughsbaffini will become famous soon enough
Send a message via Skype™ to sbaffini
Note however that it is just for the viscous part that it uses neumann conditions, which means that the viscous flux on the outflow faces is just skipped, but not the convective one.

Yet, while it is not mentioned, I'm pretty sure that they also do something for the gradient, which otherwise couldn't be computed at the outflow. But that just appears as a second order effect on the convection.
sbaffini is offline   Reply With Quote

Reply

Tags
fluent, outflow boundary, temperature

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
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 08:38
My radial inflow turbine Abo Anas CFX 27 May 11, 2018 02:44
How to set OUTFLOW boundary condition in ANSYS FLUENT using TUI? er_ijaz FLUENT 0 February 12, 2016 11:50
asking for Boundary condition in FLUENT Destry FLUENT 0 July 27, 2010 01:55
Fluent Treatment of mixed boundary condition HELP Amr FLUENT 0 May 26, 2006 06:46


All times are GMT -4. The time now is 07:21.