# Treatment of temperature using outflow boundary condition in Ansys Fluent

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

 May 25, 2022, 06:45 Treatment of temperature using outflow boundary condition in Ansys Fluent #1 New Member   Join Date: May 2022 Posts: 3 Rep Power: 4 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

 May 25, 2022, 07:44 #2 Senior Member   Sayan Bhattacharjee Join Date: Mar 2020 Posts: 495 Rep Power: 8 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.

May 25, 2022, 10:23
#3
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,782
Rep Power: 71
Quote:
 Originally Posted by eddie4160 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.

 May 25, 2022, 22:00 #4 New Member   Join Date: May 2022 Posts: 3 Rep Power: 4 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.

 May 26, 2022, 10:49 #5 Senior Member     Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 2,157 Blog Entries: 29 Rep Power: 39 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.

 Tags fluent, outflow boundary, temperature