Have you activated the energy equation to calculate distrubution of temperature in the pipe?

Lets see below: "Please draw it until 21:36min."

https://www.youtube.com/watch?v=dF6DTLKR9Fg&ab_channel=KETIVTechnologies

Thanks Hayati! Yes I have activated energy equation, anything I have to do with convection in BCs?

...but you have generated a mesh inside the solid material of the hollow cylinder?

And next you have created in Fluent interfaces between the fluid zone and the resulting solid zone?

Then with solving the energy equation in both fluid and solid zones you should see a heat transfer through the coupled walls.

Regards,

Dr. Th. Frank.

Hi,

Select the energy equation (as commented above)

Choose a turbulent model such as k-e or k-w, these are two-equation models and require less computational resources. K-w requires more time than k-e, but the results are more stable.

Select some models for validation of your simulation, such as Dittus-Boelter and Gnielisnki correlations (this would be the hand written calculation) to compare with the simulation results. Calculate the values and set them apart.

For inlet BC you can use velocity or flow rate. For the heat flux, if you read some papers from RG or ScienceDirect, for instance, you will see that the heat flux range from 5000 W/m^2 to 10000 W/m^2.

For the outlet, you can left it as default.

Select parameter like T, friction factor and pressure to monitor the convergence. Do not monitor the default convergence only ( continuity, energy, k, epsilon, omega), sometimes they converge, but important parameters like P are still varying.

From my experience, I can assure you that there is no rule of thumb for ansys cfd simulation. Actually, you can try different values and see what goes on with the results and convergence.

Please take a look at my most recent paper on CFD simulation: Conference Paper CFD Study of the Thermal Performance Improvement of a Counte...

Good luck

Humberto

Thank you Thomas Frank . Thanks Humberto Santos for your elaborate explanation. I have tried all that, still struggling to get the solution (temperature of water is not increasing at all). Already used 'coupled wall BC', tried for 'share topology' too. Whether, I have to use convection BC in Fluent setup or not? Herewith posting some images for your ready reference. Kindly look into it..

A single cell over the thickness of the tube would not be sufficient. There will be a temperature gradient between the thermal boundary condition being applied to the outer wall of the tube and the fluid-solid interface at the inner tube wall. In your meshing there is only one cell center where the temperature of the solid could be represented. Clearly not enough to represent a temperature gradient....

I think, you should spent at least 10 mesh points for the pipe thickness.

Regards,

Dr. Th. Frank.

Sukanta,

I totally agree with Dr. Thomas Frank.

By changing the mesh on the tube domain to tetrahedral will increase the number of elements on the tube wall.

But please answer me the questions below:

1 - What are the dimensions of your physical model?

2 - I could not see exactely where the insulation is placed. Is it on the inner wall of the tube?

Thanks Thomas Frank and Humberto Santos ! Herewith posting a image for your reference with modified meshing.

@Sukanta,

I am not sure if i got it right. But were you using convection mode? Instead, use heat flux in the wall boundary condition. Let us know how it goes on

Humberto Santos No, I am not using convection mode, using constant heat flux of 10,000 W/m2

I agree with both Thomas Frank and Humberto Santos. You should fine your mesh in the solid hollow cylinder zone.

Besides that, what I could understand is that the heat flux is falling over the insulated wall. If this is correct then it is obvious that the temperature of the water would not change...

In my view, you should spend some time on the insulated boundary.

Make sure that your interfaces have been established correctly.

Before assigning interfaces to the specific surfaces, the interface walls should have adjacent the same material you want to use. For example, it happens sometimes that material is changes but not implicitly assigned to the wall and cell zone condition.

Thirdly, you should know that steel will conduct less and Al will be faster, so look at the physics. And last , I think your pipe is very long. First run an unsteady simulation.

Thank you Shamoon Jamshed and N. H. Khan sir.

Is there any specific method/tool to establish the interface correctly Shamoon JamshedShamoon Jamshed?

Actually heat flux is providing on upper surface of the pipe named as heated surface, so it is not an insulated wall N. H. Khan sir?

Sukanta Nayak

I believe that it would be simple to solve if you use only the fluid domain with the heat flux applied directly on it's surface. Actually, most papers are written this way, unless any specific characteristic of the tube is being investigated. This would be my suggestion. N. H. Khan made a good point about the insulated wall.

Fluent allows to define mesh interfaces manually.

A pre-requirement is for sure, that the involved surfaces are exposed to the CFD solver as so-called named selections from the mesher/geometry modeler.

Regards,

Dr. Th. Frank.

If you generated the mesh in ANSYS MESHER, it creates interfaces itself if you define fluid and solid regions in the mesher. It is good to have a frozen region by specifying enclosure between the hollow regions of the pipe. (i.e from inlet to outlet). The top wall will then be used for specifying heat flux.

Dear Sukanta Nayak ,

I've attached a workbench (2020 R1) fluid flow solution of your model (The file size is about 65 Mb for download.). The solution was converged and the temperature increase is observed at the outlet B.C. However, the increased temperature of your model is negligible and is around 0.25 k. It was validated with Q=m_dot*Cp*(Tout - Tin) equation.

Best regards,

Amir Sabernaeemi

(https://fluidcodes.ir/amir-sabernaeemi/)

Thank you all for your kind attention and help. For me, it is really worth learning, hope I can solve it now.