Learning Forum

[Bran]

Hello,

 

I am working on a problem where I have a room with an airconditioner and various heat sources. I applied a volumetric heat generation term to the heat source and have an inlet velocity from the air conditioner at 273 K for cooling.

 

I want to add a few additional fans into the room that function to improve the cooling in the room. 

 

When I set the inlet velocity of the additional fans, it is set at 300K which I believe messes up the air conditioner cooling of the room and components.

 

How do I make these fans just add circulation into the room?

[Rob]

You shouldn't have an inlet velocity for internal surfaces (fans), if you're setting the velocity it sounds like you're adding mass to the system. Have a read through the boundary condition section of the User's Guide: you want to look a the "fan" condition. 

[Bran]

Hi, thank you very much for pointing me to that boundary condition.

I have been trying to implement this in simulation, but am having several problems, even after reading the user guide.

 I created an interface in the workbench meshing application between the face that I want the fan to be and the fluid domain face. I have added images outlining my problems, I hope they convey the right information.

After running the mesh check, I get several messages shown below:

WARNING: 537 pair(s) of adjacent faces with different orientation on zone 7.

Error: jump zone 7 has wrong types of cell zones (cell and cell).

5: Adjacent faces have different orientation: Face 187, zone 7, (ID: 34377811): at location ( 3.17346e-01, -3.33962e-01,  1.85309e+00).

My boundary conditions are shown below:

 

 

[Rob]

The interiors you've highlighted are the cell zone facets and should be left alone (we're hiding those in 2019R3 to reduce confusion). 

The fact you have interface zones means you've not connect the geometry (share topology or multibody parts: SpaceClaim & DesignModeler respectively). If you do that you'll have an interior surface (label it too) at the same location as the second image second block above. Then use the fan bc. 

[Bran]

Thanks again so much for your help. I have been trying to use share topology on SpaceClaim shown in the attached pictures. Unfortunately when I go into the meshing application, I cannot select the faces that I want to name as inlet and outlet. Nor can I select any faces are that are in the enclosure, except the topology that I shared.

How can I share the topology of the battery fan, but also be able to select the faces in the enclosure for inlet and outlet specifications in meshing?

Another note is that I have shown all hidden faces, so I do not believe that is one of the problems.

picture 1

picture 2picture 3picture 4

[Rob]

Does the circular face exist in the CAD?  When building the model you should finish up with a volume for the room, and separate volumes for all the kit. 

[Bran]

Thank you so much for your support with this problem, your patience and guidance is much appreciated. The circular face does exist in the CAD, it was a circle drawn on top of the solid body, as shown in the pictures. I am able to select the faces that I need to select using box tool, but not select tool.

When I generate the volume for the room, I use the enclosure tool that creates a negative volume for all the batteries and battery fans at once. 

I come across a problem where the adjacent cells do not match the cells I am trying to turn into a fan. To get over this problem, I turn the fan casing into a fluid zone, is this the correct way for the boundary condition setting?

Using the fluid region setting, I obtained the results shown below:

My concern is that the streamlines are not showing from the fan and the pressure contour is in its own region. I did share topography, so I am not sure what is occuring to cause it to be in its own region.

 

 

[Rob]

The fan (circle) should probably be the fan boundary condition. The volume inside the casing should probably be fluid, but the other surfaces around the volume may need to be walls?  Which direction should the air blow out of the volume? 

We're very limited in how much we can help with the application: this is due to export rules. As a result we need you to think through the problem and we can give hints. 

[Bran]

Hi rwoolhou,

unfortunately I am still having problems with this boundary condition. Thanks for your continued support.

sharing topology on spaceclaim causes a weird problem in the mesh editor where i am selective body meshing is not being recorded. After doing some searching, I found that I can RMB and clear generated data. After this, I can generate the mesh without seeing the message.

I can walk you through my methodology to see if I can get any hints on what I have been doing wrong, because i cannot even get a solution due to my energy residuals. I do have most of my steps shown in the above messages.

1. spaceclaim: created a domain using enclosure

2. spaceclaim: share topology, hiding solid bodies other than battery fan

3. spaceclaim: share topology ONLY on the battery fan circle

4. mesh: create a contact between battery and fluid domain (bonded-no separation)

5. mesh: select the circle that represents the fan and named selection interior-fan

 6. mesh: body and face sizing (giving me the selective body meshing error after) (at this point a message appears: The selective body meshing is not being recorded, so the meshing may not be persistent on an update. If you want to record the order of the body meshing, please use the Mesh Worksheet to track the meshing steps. Please see Selective Meshing documentation for more details) -> at this point I RMB on mesh, clear generated data and then generate the mesh and the message goes away.)

7. fluent: in cell zone condition: turn the fan body into a fluid type

8. fluent: in boundary conditions: turn the interior-fan into a fan boundary condition

9. fluent: set constant pressure jump

10. fluent: heat source generation terms for battery

11. fluent: inlet temperature and velocity set (this is the HVAC which will add cold air into the container), other conditions set (convection, materials)

12. standard initialization at inlet

13. Run

after 50-100 iterations energy begins to diverge

[Rob]

Do shared topology on everything (it connects faces and doesn't delete anything). You'll also need to used named selections on all the internal walls. 

Selective meshing is to mesh volumes in an order you choose, unless you plan on needing to adjust the geometry & remesh the recording doesn't matter. It's a warning rather than an error so (in this case) can be ignored. 

If it's diverging there's (usually) a reason for that. Check mesh quality but also review the results as it starts to go wrong. The latter usually highlights where your problems are. 

[Bran]

Hi rwoolhou,

Thank you for your help. I have been reviewing my results, which look promising. My energy is still having problems converging, but i will try to review thoroughly using your advice, and identify what the cause can be.

For diverging energy I will: look at the sizing of my components and mesh quality. 

Looking at my streamline and velocity results, I am wondering if you can provide guidance on the issue I have identified:

I would like the air to be moved from inside the fluid domain, rather than from the fan housing, which is also set as a fluid domain (picture attached). I tried to add just a surface (that would represent the fan face) into the fluid domain, which would act as my fan boundary condition. But this does not work, as the surface does not appear on the mesher or Fluent. Is there a way to connect the two fluid domains or is there a way for me to incorporate just a face into the domain to represent the fan face?

 

 

 

[Rob]

You can only have faces that are part of volumes, so for an internal fan unit I'd tend to split out the fan box, and then use share topology & give it a separate fluid label. You can label the fan box faces to suit.