June 28, 2019 at 6:03 pmdnelo13Subscriber
Hi there, it's Daniel. I want to make a 3d simulation of the heating of a cool product inside a box which is closed. The main idea is tha the box is under air convection so it is heated by the ambient by a heat conduction coeficient. As the walls of the box get hot, the air inside the box get hot too and heat the product inside the box. What would be the boundary conditions? How could I relate the air inside the box with the walls of the box? It would be a transient analysis.
June 30, 2019 at 2:37 ampeteroznewmanSubscriber
A simple additional boundary condition is the bottom of the box. Assume the box is sitting on an insulated surface.
For simplicity, let the cool product on the inside be a cube sitting on the bottom of the box in the center with air all around it.
In DesignModeler, create the cube solid and the box solid, using Add Frozen, so you have two separate solids. Then use Boolean to Subtract the cube from the box, using Keep Tool so you have two solids, the cube and the box with the cube shaped hole in the bottom. Now select these two solids and Form New Part to share topology.
This is about the simplest geometry you can make to do this simulation. The box solid represents the air inside the box. Five faces of the box can have a convective boundary condition with the warm outside air temperature. On those five faces, you can also define a wall thickness and conductivity for the box material. The cube solid represents the product, and you will need to define that as a solid with a specific heat capacity and give it an initial temperature. The air inside the box can have the same initial air temperature. You will want Gravity included to allow the natural convection to occur inside the box.
You will also need to imprint a small square face into the side of the box solid to represent a pressure equalization hole. As the air inside the box warms up, it will expand and a small volume will need to exit the box. The face on the side of the box is defined as a Pressure Outlet boundary condition.
Here are a few relevant discussions.
July 1, 2019 at 8:33 pmdnelo13Subscriber
thank you so much for your advices. I've just create the geometry, separating the two bodies, and I have set up the convective boundary condition at the five external faces of the box.
However, I don't know where can I define the conductivity box material. I've attached the boundary condition I defined.
Besides, how could I define the cool product temperature if it is define as an interior?
July 1, 2019 at 9:13 pmpeteroznewmanSubscriber
I'm also learning Fluent, so I don't know everything, but I am good at guessing. I see a Material Name on the lower left side of that dialog box with an Edit... button next to it. Does that let you define a conductivity?
I believe you can set the initial temperature on the cold solid and the cold air in the box in the Solution Initialization panel.
On one of the five faces, did you make a very small imprinted face to have a pressure outlet?
July 6, 2019 at 3:09 pmdnelo13Subscriber
I have set up a 2D simulation for an easily calculation. I have defined the material box conductivity and I have applied the air convection to the exterior walls, however, when I define the interior temperature of the cube, it keeps like a constant, and it has no variation with the ambient inside the box.
I've attached the boundary condition that I've defined.
July 7, 2019 at 6:39 pmpeteroznewmanSubscriber
Do not apply a Boundary Condition of Temperature to the Product wall. That forces the solution to keep it at that temperature through all time, which is what you got. Delete that Boundary Condition.
The product and the air should both get an Initial Condition of 3 C to start the simulation, then the convection from the warm air outside the box will heat the air inside the box and the airflow will heat the product over time.
Where is your small edge on the box defined as the Pressure Outlet to accommodate the increase in air volume as it warms up?
July 8, 2019 at 7:25 amdnelo13Subscriber
Thank you for your advices.
I though I defined wrong the boundary conditions because it was a very good insulation box, but everything is okay.
The pressure outlet is defined at the bottom of the box, I think it's okay.
July 8, 2019 at 11:17 ampeteroznewmanSubscriber
If the entire bottom face is an outlet, then cool air that descends near the surface of the product will leave the domain. That is not correct. It should hit a floor and flow out toward the warm box wall, be heated up and rise. You only need a very small outlet on the edge, maybe somewhere in the center of the box wall.
July 10, 2019 at 3:59 pmRobAnsys Employee
You also need ideal gas (assuming it's a gas) to model a sealed domain: this allows the temperature & pressure to float to maintain the volume.
- 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.
- 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
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.