[ShubhCFD]

Model: I have made 3D geometry of small copper block and made computational domain around it. I want to heat this copper block to nearly about 1000°C by passing hot air from inlet at 1000°C.
I don't know what radiation model can I use here since I was trying simulation with DO model. But block is getting heated by only 1°C. But actually it should be achieving temperature nearly about 1000°C.
Please help me setup the right model for this problem.

[vinerm]

Do you want heat to be transferred by radiation or convection or conduction or a combination of these? Furthermore, DO makes sense only if air is wet and/or it has some greenhouse gas or soot particles.

[ShubhCFD]

Originally Posted by vinerm

Do you want heat to be transferred by radiation or convection or conduction or a combination of these? Furthermore, DO makes sense only if air is wet and/or it has some greenhouse gas or soot particles.

I want the combination of all modes of heat transfer.
I guess I am simulating this problem in wrong way, air is dry. Can you please throw some light on how to do modeling of this problem?

[vinerm]

Dry air will not have much of radiation effect since the emissivity is more or less 0. So, it would primarily be convection and conduction.

[ShubhCFD]

Originally Posted by vinerm

Dry air will not have much of radiation effect since the emissivity is more or less 0. So, it would primarily be convection and conduction.

At first I was using only convective modeling and by using K-epsilon model without radiation modeling there was not much increase in the temperature of copper block.
Hence now I am not sure which way to set up the model. Can you suggest something from your side?

[vinerm]

As a first step, do not solve any flow or turbulence. Just initialize the air with high temperature and solid block with low temperature. Run it as steady-state. Solve only Energy equation; keep other equations disabled. Look at the results. If it shows that solid is colder than air, then there is problem with interaction between fluid and solid domain.

[ShubhCFD]

Originally Posted by vinerm

As a first step, do not solve any flow or turbulence. Just initialize the air with high temperature and solid block with low temperature. Run it as steady-state. Solve only Energy equation; keep other equations disabled. Look at the results. If it shows that solid is colder than air, then there is problem with interaction between fluid and solid domain.

Hello, I tried the simulation and the copper block has reached the inlet temperature in steady state simulation. Thanks, I feel more confident now. But I don't know why it is not working in transient simulation. I want to know the time it requires to reach that state and the temperature changes in the block. Further help from you will be greatly appreciated.

[vinerm]

That means the fluid-solid interaction is good.

Now, try with fluid flow but use a very high thermal conductivity and very low specific heat for fluid as well as solid; increase (and decrease) the values artificially by a factor of 1000 or so. This is just to test the time required to heat it up. Once you find the time required for the solid to heat up with modified properties, then reduce change the thermal conductivity and specific heat back to normal. The time found using such method would not be accurate but will give you an idea about a scale.

In practice, diffusion time-scale is given by ratio of square of length scale and diffusion coefficient. For fluid, length scale is usually the thickness of thermal boundary layer and diffusion coefficient is thermal diffusion coefficient. This directly gives you time scale for thermal diffusion. Do note, however, that turbulence increases the diffusion coefficient almost 500 to 1000 times depending upon the turbulence structure, hence, reduces the time-scale by a large factor.

[ShubhCFD]

Originally Posted by vinerm

That means the fluid-solid interaction is good.

Now, try with fluid flow but use a very high thermal conductivity and very low specific heat for fluid as well as solid; increase (and decrease) the values artificially by a factor of 1000 or so. This is just to test the time required to heat it up. Once you find the time required for the solid to heat up with modified properties, then reduce change the thermal conductivity and specific heat back to normal. The time found using such method would not be accurate but will give you an idea about a scale.

In practice, diffusion time-scale is given by ratio of square of length scale and diffusion coefficient. For fluid, length scale is usually the thickness of thermal boundary layer and diffusion coefficient is thermal diffusion coefficient. This directly gives you time scale for thermal diffusion. Do note, however, that turbulence increases the diffusion coefficient almost 500 to 1000 times depending upon the turbulence structure, hence, reduces the time-scale by a large factor.

Thank you so much. I tried with your instructions and got the results. But I think radiation effects could also be included in the modelling as the block is heating very slowly, since surrounding is at 1000°C and block is at 25°C. So which radiation model could be suitable in this case?

[vinerm]

Since the gas is dry air, use Surface-to-Surface model

[ShubhCFD]

Originally Posted by vinerm

Since the gas is dry air, use Surface-to-Surface model

Thanks. Since optical thickness of air is zero I was also thinking of this model after you suggested it earlier.
Suppose my inlet surface is not directly facing the copper block, then also S2S can be used? That is if heated air is coming from inlets such as burners which doesn't directly face the copper block.

[vinerm]

In S2S, everything is based on the geometry, i.e., the view factors. So, even if some boundary is not facing some other boundary directly, it would have its effects via reflections or at rather acute angles with low view factors.