January 4, 2019 at 1:18 amkawad24Subscriber
I am trying to model flow through one channel of a heat exchanger fin using conjugate heat transfer. Air is flowing through the channel. The top wall has a constant heat flux, and the left, right, and bottom are completely insulated. I tried to model the surrounding walls and the fluid as separate bodies but am getting confused with assigning boundary conditions to all generated walls/shadows. For example, how do i know which boundaries to couple? Essentially I am trying to get the heat transfer rate of the fin and the pressure drop of the fluid. Also I am looking to change the roughness of the interior wall surface touching the fluid. How would i go about doing that? Can someone give me advice and a potential example to help me with this process?
January 4, 2019 at 5:31 amKeyur KanadeAnsys Employee
as ansys employee we can not download attachments. so if you want you can insert some images to explain the issue.
please have a look at following video which may help you.
January 4, 2019 at 11:04 pmpeteroznewmanSubscriber
My advice is in the geometry editor, use Shared Topology to simplify what is translated into Fluent. If you use Shared Topology, no Contacts are needed in Meshing and there are far fewer interfaces in Fluent.
What geometry editor is your geometry coming through: DesignModeler or SpaceClaim?
If you used a Fluent analysis system and just brought geometry straight into the Geometry cell and then into Meshing without first going through DM or SC, then you won't be able to benefit from Shared Topology.
There are a few members like me on the site who are not ANSYS employees and are able to open attachments. If you need specific advice on how to use Shared Topology, there are some discussions here, but the interface is different in DM and SC so let us know which one you are going to use. If you want to share your model, please create a Workbench Project Archive .wbpz file and attach it after you post a reply and say what release of ANSYS you use.
January 4, 2019 at 11:14 pmkawad24Subscriber
I used a solid works step file and imported it into space claim. Additionally, I am using Ansys 19.1. I uploaded my model.
January 5, 2019 at 1:56 amkawad24Subscriber
my issue is I'm having trouble deciphering which contact surface is which and where I should couple the boundary conditions (as you can see in the picture ansys created many walls, but when i click display I can't see the surface). My boundary conditions are constant heat flux on the top wall, insulated on the left, right, and bottom wall. Air is flowing through the channel and is convective. Can someone please help me? I'm new to ansys and am having a difficult time.
January 5, 2019 at 10:32 pm
January 6, 2019 at 12:28 ampeteroznewmanSubscriber
Thanks for the archive. I opened it in 19.1 and started SpaceClaim.
You want to select the FFF in the outline and change Share Topology to Share.
Then Refresh the Project and in Meshing, you can suppress all the Contacts.
In Meshing, you should see purple edges that indicate an edge is shared by more than one body. In this view, the Top body is hidden, and you see a purple line on the right but not on the left. That means that back in Geometry, the two surfaces that are near each other are not the same surface, so the shared topology is failing here.
It means the mesh isn't connected between the left body and the fluid body, while the mesh has connection problems between the fluid body and the right body. It is critical that the geometry be perfect to get a good mesh.
Some corrective action is needed in SpaceClaim.
I will post this now and post an update when I figure out how to fix this problem.
January 6, 2019 at 12:57 ampeteroznewmanSubscriber
I deleted all the solids except for the Fluid and recreated the front, back, top and bottom walls by copying the faces of the fluid.
I went into the Workbench tab in SpaceClaim and clicked on the SharePrep button. Now all the edges are purple.
Refresh the Project and start Mesh then mesh the part. You get a clean swept mesh.
Later, I would add some mesh controls to create inflation layers to the fluid region.
Now in Fluent, there are fewer BCs.
Attached is an ANSYS 19.1 archive.
January 6, 2019 at 1:13 amkawad24Subscriber
I'll take a look at this. Thank you so much for your help. I greatly appreciate it.
January 6, 2019 at 4:07 amkawad24Subscriber
Now as far as my boundary conditions, do i leave the adiabatic sides at 0 heat flux for insulated walls, the top with constant heat flux, and leave the rest coupled? I'm not sure where to specify convection for the air flowing through.
January 6, 2019 at 5:32 ampeteroznewmanSubscriber
If you want insulated walls on three sides of the fluid and constant heat flux on the top wall, you don't actually need any solids besides the fluid body.
Suppress all other bodies in Mesh and just transfer the fluid body.
Increase the mesh density on the fluid body, add inflation layers.
Convection is achieved by having gravity turned on and temperature dependent density.
Read this discussion for more details.
January 6, 2019 at 6:32 amkawad24Subscriber
I understand what you are saying, but what if I want to see the temperature change of the aluminum channel?
January 6, 2019 at 5:12 pmpeteroznewmanSubscriber
I misunderstood when you said insulated walls. I thought you meant that the material on the side of the fluid was an insulator. In that case, you don't need a solid wall for the channel. But you want the channel wall to be aluminum and so is thermally conductive, and the insulated wall is on the outside of the aluminum. Then you need the solid walls.
It's a good practice to develop models in stages. You could get the fluid solution working with insulated walls as the first stage, then add the solid conductive walls in as the second stage.
January 6, 2019 at 9:06 pmkawad24Subscriber
For some reason the inflation meshes are failing in the fluid body. I noticed that it might be because when creating meshes the fluid body is transparent in some areas...the geometry in space claim shows it completely solid however. I'm not really sure what the problem is. It might be a shared topology problem?
January 7, 2019 at 1:28 ampeteroznewmanSubscriber
There is some defect in rendering the faces of the solid, but it is only rendering, the mesher is not bothered by this defect.
Here is a nice inflation layer on the fluid domain.
The solids that make up the walls were suppressed for this mesh.
I redefined the Named Selections so a model could be built without the extra solids.
January 7, 2019 at 1:59 am
January 7, 2019 at 2:15 ampeteroznewmanSubscriber
Sorry, I forgot you were on ANSYS 19.1. I did that in 19.2 but there is no going backward so you will have to do the work yourself.
Or you could upgrade to 19.2
January 7, 2019 at 2:37 amkawad24Subscriber
ok, with your method, are you saying it is ok to not include the thickness of the aluminum solids surrounding the edges even if I want to see the temperature of the aluminum in my model? I see in the pictures you only have the fluid now.
January 7, 2019 at 5:25 amkawad24Subscriber
Can someone check my boundary conditions. I am trying to do constant heat flux on top (12.5 W/m^2) and insulated on the bottom, right, and left side. I used the Boussinesq approximation to simulate the convection of air flowing through the channel. I think I went wrong somewhere but am unsure where. (used Ansys 19.1)
January 7, 2019 at 9:41 pmkawad24Subscriber
I have a question about: would this approximation would this approximation work for forced convection?
January 7, 2019 at 10:04 pmpeteroznewmanSubscriber
It's a good practice to develop models in stages. You could get the fluid solution working with insulated walls as the first stage in a smaller model, then add the solid conductive walls in as the second stage of a larger model.
January 7, 2019 at 10:56 pmpeteroznewmanSubscriber
You selected bodies in your named selection whereas I believe you were meant to select the outer faces to define the faces that have a constant heat flux crossing the face.
The same goes for the insulated faces, they would be the outer faces of the lower aluminum bodies. However, I believe any face not defined is automatically an insulated face.
I don't know if you got to defining the materials, but the air in your file shows a constant density, and you said you were going to use boussinesq.
January 13, 2019 at 8:56 pmkawad24Subscriber
Does anyone know how to simulate forced convection? i feel like my simulation isn't as accurate to the model i want because the boussinesq simulation is for natural convection...
January 14, 2019 at 2:38 ampeteroznewmanSubscriber
The air in the channel has an inlet velocity and a pressure outlet, so the air is experiencing forced convection by virtue of the imposed velocity. If it was a closed space with no inlet velocity, then the air would experience only natural convection.
January 28, 2019 at 2:48 pmkawad24Subscriber
another question....how do i ensure that the mesh is good?
January 28, 2019 at 3:24 pmDrAmineAnsys Employee
Check mesh quality metrics in the solver: Aspect Ratio, Skewness, Orth. Quality and cell volume change.
January 29, 2019 at 3:37 amKeyur KanadeAnsys Employee
make sure you have min orthogonal quality more than 0.1.
February 3, 2019 at 9:26 pmkawad24Subscriber
where do I check the min orthogonal quality? Im having trouble figuring out if my mesh is too coarse, however if I make it finer it takes a long long time to load.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- Exporting Data Results