TAGGED: energy-equation, flow-pattern, fluent
February 8, 2021 at 7:30 pmSpencerJordanSubscriber
I am trying to simulate a simple 2D situation where the walls of a cylindrical structure are cooled to 240 K and 270 K, respectively. Then, air is injected at the top of the cylinder at a certain velocity and is cooled as it flows down. My analytical calculations predict a much greater affect on the flow profile of the air from the temperature of the walls than is being shown in the simulation results - almost no change in flow profile is seen in the simulation.
Currently, I'm using the Realizable k-epsilon model with enhanced wall treatment and thermal effects. I have the energy equation enabled and I am setting my walls to constant temperatures. Should I be using a different model/parameters to model the expected thermal turbulence? Thanks!February 9, 2021 at 5:11 pmSurya DebAnsys EmployeeHello,
Do you have sufficient length to see the development of thermal boundary layer?
Also check your mesh resolution near the walls. What is the Y+ value near the walls?
Do you impose a transient boundary condition where the wall temperature cools with time?
February 10, 2021 at 5:54 pmSpencerJordanSubscriberHi Surya What length do you think would be required for this situation? The chamber I'm simulating is about 1m long. I'll attach a photo of my mesh resolution at the walls, but I have refined it several times at those boundaries. The Y+ value does seem low, it is 1.0 or lower along both of the walls. And the boundary condition is not transient, I would like to simulate with the walls being held at constant temperature.
February 10, 2021 at 6:07 pmSurya DebAnsys EmployeeHello Spencer,
Generally the Prandtl number of air is around 0.69, which indicates that thermal diffusion is faster and more dominant than the momentum diffusion. So thermal boundary layer formation should occur faster.
Are you trying to model a 2D and compare the analytical results for a 3D cylindrical case?
I would recommend you to model a 2D axi-symmetric case instead of 2D planar.
In 2D planar, you will be missing out on the additional terms.
February 10, 2021 at 7:35 pmSpencerJordanSubscriberOkay, thank you. You are correct, I am trying to compare to a 3D case so I'll give axi-symmetric a try. And the Prandtl Number I'm seeing (in the original planar simulation) is about 0.38
February 10, 2021 at 9:31 pmYasserSelimaSubscriberMake an inflating boundary ... try to decrease the mesh size of the first layer close to the boundary and let it increase as you go away from the wall.
One thing I have seen in an earlier post in this forum; someone had a completely weird flow behaviour in natural convection and the reason was selecting large timestep. So, you might take this into consideration.
Regarding Prandtl, it is almost 0.7 for air between 150 K to 1500 k ... so probably something is set wrong in the material properties if you are simulating dry air
February 11, 2021 at 11:55 pmSpencerJordanSubscriberIt seems that my issue was that I had forgotten to enable gravity in the model, therefore no thermal buoyancy effects could be calculated. I turned gravity on and made sure air's density was set to a temperature dependent model (incompressible ideal gas) and I am now seeing my predicted results.
February 12, 2021 at 7:28 amDrAmineAnsys EmployeeThanks for feedback
Viewing 7 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.