Flow through a Heat Exchanger Channel

  • 199 Views
  • Last Post 03 February 2019
  • Topic Is Solved
kawad24 posted this 04 January 2019

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?

 

 

 

 

 

 

 

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 06 January 2019

Hello Kawad24,

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.

Regards,
Peter

  • Liked by
  • kawad24
peteroznewman posted this 06 January 2019

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.

  • Liked by
  • kawad24
peteroznewman posted this 07 January 2019

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.

Attached Files

  • Liked by
  • kawad24
kkanade posted this 04 January 2019

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. 

 

peteroznewman posted this 04 January 2019

Hello kawad24,

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.

Regards,
Peter

kawad24 posted this 04 January 2019

I used a solid works step file and imported it into space claim. Additionally, I am using Ansys 19.1. I uploaded my model.

Attached Files

kawad24 posted this 05 January 2019

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.

 

kawad24 posted this 05 January 2019

These are the regions that show up after the meshing is set. I am confused about how to assign the boundary conditions for my case.

 

 

peteroznewman posted this 06 January 2019

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.

Regards,
Peter

Attached is an ANSYS 19.1 archive.

 

Attached Files

kawad24 posted this 06 January 2019

I'll take a look at this. Thank you so much for your help. I greatly appreciate it.

kawad24 posted this 06 January 2019

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.

peteroznewman posted this 06 January 2019

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.

kawad24 posted this 06 January 2019

I understand what you are saying, but what if I want to see the temperature change of the aluminum channel?

kawad24 posted this 06 January 2019

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?

not

peteroznewman posted this 07 January 2019

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.

Regards,
Peter

Attached Files

kawad24 posted this 07 January 2019

I am not able to open the file...i keep getting the following error.

 

peteroznewman posted this 07 January 2019

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

kawad24 posted this 07 January 2019

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. 

kawad24 posted this 07 January 2019

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)

Attached Files

kawad24 posted this 07 January 2019

I have a question about: would this approximation would this approximation work for forced convection?

peteroznewman posted this 07 January 2019

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.

kawad24 posted this 13 January 2019

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...

peteroznewman posted this 14 January 2019

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.

kawad24 posted this 28 January 2019

another question....how do i ensure that the mesh is good?

abenhadj posted this 28 January 2019

Check mesh quality metrics in the solver: Aspect Ratio, Skewness, Orth. Quality and cell volume change.

Best regards,

Amine

kkanade posted this 29 January 2019

make sure you have min orthogonal quality more than 0.1. 

kawad24 posted this 03 February 2019

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.

Close