[zargham]

I am simulating a transient conjugate heat tranfer for a furnace, that has three domians, two fluids and one solid. The solid domain is in between the two fluid domains. There are heating rods in both fluid domains. These heating rods are heated at given heating rates, in my case at 10 kelvin per minute upto 1080 kelvin. This gradual increase is given to the rods via profiles in boundary conditions. The fluid domains are heating up correctly, but the temperature for solid domain is increasing much slower as compared to fluid domains.
After 1700s flow time, the average temperature in fluid domain goes upto 510K but for solid it increases to just 365K. I think its because of the fact that the convective heat transfer rate is faster than conductive heat transfer rate. But does this correspond to the reality or not? I have added a temperature profile at a plane.
Further, the solid is 22mm thick and the temperature does not change along the thickness as well (the whole solid is at same temperature), although there are 4 heating rods in the lower fluid domain and 14 heating rods in the upper fluid domain. I have attcahed the geometry for clarification.
The interface between solid and fluid is coupled by wall and shadow wall. I have used share topology for interfaces as well. Right now, i have not included any velocity, all the walls except the interface walls are at zero heat flux. I am using SIMPLE solution method and an automatic solid time step calculation method for calculating solid time step. Is there any way to solve this issue?

[CFDKareem]

A few questions/comments:

1) Do you fluid domains have any inlets/outlets? If so, where?

2) Depending on the materials, conduction through a solid should be much faster than convective heat transfer.

3) Heating a flat plate with hot air from below is not a very efficient process and it makes sense that it will take awhile for the heat to be transferred into the solid.

4) In the real product a large amount of heat transfer from the bottom heaters will be transferred into the solid through radiation, since they are at high temperatures. Consider adding S2S radiation.

5) Plot the heat flux through each boundary to get a sense of how much heat is being transferred into the solid. From this value you could quickly estimate how long it will take for the material to increase to the target temperature.

6) Double check you set-up including the material properties and mesh. Natural convection specifically requires good refinement along the walls to accurately model the heat transfer coefficient.

[zargham]

CFD kareem, thank you very much for your comments.

Their are inlets and outlets, but for start, i am just focusing on temperature distribution in an enclosed volume, with flux zero at all outer walls. I will add the inlet velocity once i get the correct temperature distribution inside the furnace.

I am using fluent watertight workflow for meshing. The mesh is pretty much fine along the walls. But i have not turned on the gravity, and have not used temperature based density like boussinnesq desnity in the material properties for air, rather i just used constant density. So what do you suggest, should i turn on gravity and use the density that is changing with temperature?

Another thing about S2S model, should i apply this model to both fluid domains or just the lower domain and to all walls or some specific walls?

Thank you once again.

[CFDKareem]

Originally Posted by zargham

CFD kareem, thank you very much for your comments.

Their are inlets and outlets, but for start, i am just focusing on temperature distribution in an enclosed volume, with flux zero at all outer walls. I will add the inlet velocity once i get the correct temperature distribution inside the furnace.

I am using fluent watertight workflow for meshing. The mesh is pretty much fine along the walls. But i have not turned on the gravity, and have not used temperature based density like boussinnesq desnity in the material properties for air, rather i just used constant density. So what do you suggest, should i turn on gravity and use the density that is changing with temperature?

Another thing about S2S model, should i apply this model to both fluid domains or just the lower domain and to all walls or some specific walls?

Thank you once again.

If there is no forcing flow then I would definitely suggest changing the density to "incompressible ideal gas", change the pressure discretization to PRESTO! or body force weighted, and turn on gravity. Without modeling natural convection the air will act like an insulator as it will not move at all when heated.

I would try to model the natural convection first and see how it goes. After that you can add radiation if needed. Which areas to add it too will be up to you. I would definitely add it to the lower section as the lower heaters should be heating the solid. I'd also probably add it to the top as the upper heaters will radiate some energy to the top of the solid as well.