August 7, 2019 at 8:47 pmhrennisonSubscriber
I am working on a thermal analysis of a cold plate in a cooling system. The cooling system is designed with stainless steel cold plates, a chiller and plastic tubing. The point of the cooling system is to sustain the temperature of a unit on top of the cold plate through conduction. The unit would be sitting on top of the cold plate, which has cool water flowing through it. I would like to use ANSYS to understand where the temperature changes and by how much. So far I have created the model and mesh. I am not able to accurately produce a model that takes the unit heat into effect. How would I continue this?
August 8, 2019 at 12:51 ampeteroznewmanSubscriber
Reply with more detail about your model. Insert images of the geometry and the boundary conditions. If you do File > Archive and create a .wbpz file (< 120 MB) you can attach that after you reply. Someone might download your model for a close look, but the ANSYS staff are not permitted to do that, they can only go by what you post.
Do you have experimental data to compare the model with the physical system?
When you say you are "not able to accurately produce a model that takes the unit heat into effect" I'm not sure what you mean. You can assign a heat flux to a face or a body in the model.
Are you planning to build this model in Mechanical as a Steady State Thermal model or in Fluent? Both solvers can model this system.
Are you planning to include convective heat transfer to the surrounding air?
August 8, 2019 at 9:49 pmhrennisonSubscriber
I have the physical system in my place of work, but not a lot of data to go on. I am attempting to predict the maximum heat flux that will sustain the steady state temperature of the cooling water flowing through the plate.
When I run the model now it shows a constant temperature along the flow of the cooling water. I expect the water to increase in temperature along the flow because it should be picking up heat from the plate. It is highly likely that the model is not accurate to what I want, so I would like as much feedback, in terms of my boundary conditions, to produce accurate results.
Currently running it in Fluent, was thinking I would need both Fluent and Mechanical as a Steady State. Is that not the case?
For now not planning to include the convective heat transfer of the air, because the main goal is to get the basic concept of the model to work, then the surrounding air will be the next task.
August 10, 2019 at 1:00 ampeteroznewmanSubscriber
If you have a model in Fluent, you don't need Mechanical.
I expect you have a mistake in the model if the water doesn't change temperature.
You want feedback but you haven't provided your model for inspection or images of your model in your post. How do you expect us to help you?
August 12, 2019 at 12:44 pmhrennisonSubscriber
I am so sorry I meant to post my model on Thursday. Here it is now.
August 12, 2019 at 5:14 pmpeteroznewmanSubscriber
What Release of ANSYS are you using?
August 12, 2019 at 6:42 pmhrennisonSubscriber
Academic Student 2019 R2
FENSAP-ICE 2019 R2
August 12, 2019 at 7:29 pmpeteroznewmanSubscriber
Create a Multi-body part in DM by selecting the four solids and Form New Part.
In Mechanical, define the three rods as Fluid, repair the Named Selections. If you get an automatically generated Contact, delete it.
Use a Sweep Method on the fluids and use Inflation on the circular holes.
In Fluent, for each pipe-wall Boundary Condition, change the Thermal setting to Coupled. (I think this is correct, the CFD experts can correct me if I'm wrong).
The velocity of the water at the outlet is 0.77 m/s on a diameter of 9.525 mm. If you calculate the Reynolds Number, you will find this is Turbulent flow. You have selected Laminar in the Models. Change to Turbulent.
The plate is a six sided box. You have defined a heat flux on one face, but on the other five faces, you have specified a temperature of 310 K. That seems odd. They could be just insulated faces. Why are these five sides maintained at a constant temperature? I changed them to zero heat flux (insulated).
I notice you have three water inlets with three different temperatures: 290, 293 and 296 K. Why do the inlets have different temperatures?
Here are the contours of temperature on a plane at the center of the block.
If you cut the inlet mass flow rate by a factor of 10, then you get an x gradient.
August 12, 2019 at 10:15 pmhrennisonSubscriber
Why would you recommend to couple it?
The box has one heat source, which is why there was only one heat flux and the rest of the temperatures were 310. I will fix that though.
The inlets have different temperatures, just to assume some numbers.
August 12, 2019 at 10:43 pmpeteroznewmanSubscriber
I read the Fluent User's Guide: section 184.108.40.206.8. Thermal Conditions for Two-Sided Walls
If the wall zone has a fluid or solid region on each side, it is called a “two-sided wall”. When you read a mesh with this type of wall zone into ANSYS Fluent, a “shadow” zone will automatically be created so that each side of the wall is a distinct wall zone. In the Wall dialog box, the shadow zone’s name will be shown in the Shadow Face Zone field. You can choose to specify different thermal conditions on each zone, or to couple the two zones:
To couple the two sides of the wall, select the Coupled option under Thermal Conditions. (This option will appear in the Wall dialog box only when the wall is a two-sided wall.) No additional thermal boundary conditions are required, because the solver will calculate heat transfer directly from the solution in the adjacent cells.
Coupling is definitely the right choice here.
A constant temperature boundary condition on a face, such as 310 K, implies heat transfer into or out of the face in order to maintain that temperature. So if there is only one heat source (heat flux on one face), a constant temperature boundary condition seems like the wrong choice for the other five faces.
A credible choice for those five faces is insulated, which is entered as a 0 for Heat Flux.
August 13, 2019 at 2:22 pmhrennisonSubscriber
In the version I have of ANSYS, there is not a turbulent option for the viscous model. The options are as follows:
Spalart-Allmaras (1 eqn)
k-epsilon (2 eqn)
k-omega (2 eqn)
Transition k-kl omega (3 eqn)
Transition SST (4 eqn)
Reynolds Stress (7 eqn)
Scale-Adaptive Simulation (SAS)
Detached Eddy Simulation (DES)
Large Eddy Simulation (LES)
What would you recommend?
I also want to thank you so much for helping me and taking time to make comments and explain the best choices.
August 13, 2019 at 9:07 pmpeteroznewmanSubscriber
You're welcome. All the models after Laminar are Turbulent models.
I'm not an expert at Turbulence models, but k-epsilon is widely used. Once you select that, there is another choice of Wall Functions. I choose Realizable because that was used in the edX course I took. Maybe I'll take a course on Turbulence later this year...
- You must be logged in to reply to this topic.
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.