[M.Shafiq]

Hi

I am new to this forum. Can anyone please help me?

Please see attached my Geometry file.
I am running a simulation of conjugate heat transfer where I have applied a constant heat flux on the top surface of rectangular plate and natural convection from the side and bottom walls of the plate. Inner wall of the tube was named as an interface and coupled condition was selected for this. But in results, it doesn't show any heat transfer from the plate to fluid.

[vinerm]

Hi Mahek

The recommendation would be to use conformal mesh instead of interface. But if you can't go back to, or don't want to go back to meshing, then define the interface as coupled when you create it. Otherwise, there won't be any thermal energy transfer across the interface. You have mentioned that coupled is selected. Then, just to test, try with a significant temperature difference across the domains. Initialize with high temperature of liquid and low temperature of solid or vice-versa, then run only energy equation. See if it shows the energy transfer. If it does, then the interface is working. Else, there is some problem with the way interface has been created. Interfaces are recommended only if there is a relative motion between two domains or if it is very difficult to get a good mesh across the two.

[M.Shafiq]

Hi Vinerm


Many thanks for your help. I am wondering if I create conformal mesh then how shall I apply boundary condition between plate and tube?

Mehak

[vinerm]

Then you don't have to. Fluent automatically takes it as coupled wall.

[M.Shafiq]

Hi Vinerm


Sorry to bother you again.

I am actually a new user of ANSYS so can't understand the errors

I have changed my mesh to conformal, still there is some no thermal energy transfer, there must be something wrong with mesh. When I did check quality, it says cannot create surface from sliding interface zone. Could you please have a look to the attached screenshots and suggest me a solution?

Many thanks
Mehak

[vinerm]

Your simulation still includes interfaces, that's the reason Fluent issues the warning that it cannot display sliding interfaces. Open Meshing tool and look at the Geometry branch. Does it list both bodies separately or is there a sub-branch under Geometry and that contains both bodies? It is the latter that you want and not the former one. That will ensure everything goes smoothly

[M.Shafiq]

In fact my geometry contains three bodies, 2 of then are solid and one is fluid. I made all of the three bodies as a single part in Design Modeler and as you said in meshing, the three bodies appear as a sub branch under Geometry. I don't know why Fluent is creating some empty surfaces.
#
Please see attached.

[vinerm]

Fluent only receives mesh and not the geometry. Your mesh has contact regions. Delete those contact regions in the Mesh, regenerate the mesh, and you will get conformal mesh without any interfaces. You just need to delete the contacts.

[M.Shafiq]

As per your suggestion I have deleted contact regions in mesh but still it didn't work. Fluent does not even solve energy equation

this is what I get this time

[vinerm]

Could you share a snapshot of your cell zones and boundary zones?

[M.Shafiq]

Hi Vinerm


Please se attached cell and boundary zones.

I just applied the constant heat flux (500 W/m2) on top surface of heat mat and leave the side walls, bottom surface and tube outer wall as zero flux. Also applied inlet velocity and pressure outlet conditions. Wall id '2' & and '10' in attached shot are automatically coupled by Fluent. Could you please guide if something is wrong with my boundary conditions?

Many thanks for bearing with me

Regards,
Mehak

[vinerm]

Though the system looks good to me, however, a sanity check can still be done. Disable flow by going to Solution Controls > Equations and ensuring that only Energy is selected. Now, initialize fluid with low temperature, say, 300 K and initialize solid with high temperature, say, 1000 K. Run the simulation as transient with time-step of 1 s for 10 s. Check the results. If the fluid heats up and solid cools down, then your setup is correct. Let me know if that is not the case

[M.Shafiq]

see for transient how to set the time-step of 1s

[vinerm]

All those details are at Run Calculation under Solution. It states Time Step Size (s). Give that as 1. Number of Time Steps as 10. Calculate

[M.Shafiq]

Many thanks Vinerm for your help

Please see attached result of transient simulation, this time tube is picking up heat near the outlet section but not fluid. And why my setup doesn't work under steady state?

[vinerm]

It does work under steady-state as well, however, diffusion of heat or momentum via molecular diffusion is very slow phenomenon. Turbulence is required to enhance it. In your work, if you calculate Reynolds number based on the diameter of the duct, I hope it is greater than 2000. If it is not, then whatever results you get with steady-state are good. If Re is greater than 2000, which I hope it is otherwise it will not work as a heat transfer device, then you have to enable turbulence model, either k- or k-. Run your simulation in steady-state and you will see the expected results.

[M.Shafiq]

I was in fact considering Laminar flow (Re = 1200)

that means I should check my setup with turbulent case.

[vinerm]

If you wish to simulate the effects of laminar flow, then keep it laminar. However, do not expect very high heat transfer for laminar flow, which is a fact.

If you want to study the effect of turbulent flow, then increase the flow rate so that the Re is really beyond 2000. Enable one of the RANS based turbulence models suggested earlier, and you will see the outcome.

[M.Shafiq]

Okay, many thanks for all of your help.

I really appreciate