Natural convection in closed domain
 

https://imageshack.com/i/mzvkkgj

Above is the link of my geometry file. I am modeling a heat generating bar in an enclosed chamber of air. The flow is setup by natural convection. I have tried a number of approaches about modeling this problem. I use surface heat flux at the boundaries of the bar.

1....
Solver- pressure based, steady
Gravity - -9.81m/s2.(-y)
material - air-
density - boussinesq (1kg/m3)
thermal exp. coeff. (3.2e-03)
Result- convergence in 460 steps
Following is the temperature contour:
https://imageshack.com/i/mu5tgkj

2....
Solver -pressure based, steady
gravity - -6.69e-05m/s2 (y)
mtrl - air -
density - boussinesq(1kg/m3)
thermal exp coeff- 3.2e-03

Result- convergence in 102 steps
Following is the temperature contour:
https://imageshack.com/i/n95ohzj

3....
solver- pressure based, steady
gravity - -9.81m/s2 (y)
op temp - 350K
material - air -
density - ideal gas
No convergence even after 1000 iterations
temp contour after 1000 iterations:
https://imageshack.com/i/j6sq8bj

I cannot decide which is the correct approach.. My next step is to model this in 3D and try get the same results on a plane in the domain. Please help...

Why did you effectively turn off gravity for the second problem? For a gravity-driven flow that's a serious change.

It will be hard to get a steady solution here, natural convection is very unsteady physically.

Your choice of the pressure-based solver probably doesn't help either. For such a density driven problem I would used a coupled solver on density.

Well i reduced gravity value as I got a tutorial on natural convection and radiation together. Here they had mentioned that gravity needs to be normalised to suit the Rayleigh and other non-dimensional numbers in the flow.
Yes, natural convection convergence is bit tricky. In a thread on this forum, they had mentioned that, start by putting gravity value as 1m/s2. obtain convergence for that value. then increase it in steps and reach 9.81m/s2.
I will try now with coupled solver. Will let you know the results.

Hi dreamz:

I am expecting a behaviour more close to the sim3 and sim1. The results for the sim2 looks, at least, wierd. Your flow should be bouyancy driven (regarding your Raileigh numer)... I do believe that it is mandatory activate the gravity an the buoyancy. Mesh resolution is quite vital for any CFD simulation specially where the temperature gradients are critical. Special attention should be taken to the "turbulence model/wall bounded flow modeling", once the buoancy effects should be considered.

The non-symmetric temperature field mainly in sim1 is quite interesting/wierd...

Regards

I tried with coupled solver but did not get any convergence. The residuals diverge haphazardly, for all the three cases.

You can always do a transient simulation of natural convection cases if you are unable to achieve convergence with a steady-state simulation.

@flotus1
Hearty, thanks for your suggestion. I have a small doubt.

What step size should I take for the transient simulation? For a similar problem I did carry out a transient simulation. When I put step size as 0.1 even after 20000 iterations it did not show convergence. But when I put 0.01 as time step after some 200 iterations it showed that solution converged for that time step.
So, how should I decide about the time step for transient formulation.

Exactly like you did it.
Well before running a simulation, you can estimate the order of the time scale
Where is the characteristic length and is the estimated fluid velocity.

Divide the result by 20 and you have a time step size to start with.
If the simulation converges well, you can still try to increase the time step size to speed up the simulation.
If it does not converge, decrease the time step size untill it does.

@flotus:
I tried steady as well as transient simulation in 3D. As mentioned earlier I did not get convergence however the temperature contour which I plotted seems correct. Following is the link to the file.
https://imageshack.com/i/mvk9mzj


I did try transient as mentioned by you to get convergence. I got convergence in each time step. I used a step size of 0.01 and number of time steps as 400, with the 20 as the max iterations/time step.

However, the contour of temperature is not correct at all. Following is the link to it.
https://imageshack.com/i/givfjbj

Please help as to what I should do to get convergence..

As always, we need much more information about the simulation to find out where you went wrong.

The second figure shows a temperature field which is practically homogeneous, isn't it?

Could you plot the initial temperature field and the field you get after one time step?

@flotus1 &@FMDenaro:
I don't think the pictures are that much conclusive... Still following are the images. I have included images at first two and last two time steps.

https://imageshack.com/i/mh5rv8p
https://imageshack.com/i/f24vhvp


https://imageshack.com/i/f3n7scp
https://imageshack.com/i/n8in9lp

Although I am usually in favor of pictures against lengthy descriptions of them, we need information that is not in the pictures here.

What are the boundary conditions in your simulation anyway? How do you introduce the heat to the system? Is the block in the centre a solid material? If so, do you have a proper interface between this solid and the adjacent fluid? If you have an interface, how did you apply the constant temperature in the steady simulation? Why is this constant temperature condition not obeyed in the transient case? If there is no interface , what are the boundary conditions for each side of the inner block? Is it really necessary to complicate the simulation by adding material to the inner block? Couldnt you use a temperature boundary condition until we found out what is going wrong? How do you initialize the solution in both cases?
What is the dimension (length) of the domain? What are the material properties of the two materials you are using?

@Flotus1:


I have done a 3D modeling. The block in the centre is actually a rectangular bar which generates heat. The bar is made of solid material, aluminum. Around that is a domain filled with air. I have extruded it as frozen and specified it as fluid in design modeler. Convective boundary condition is applied to those walls. I therefore get two parts which I combined to form a new part. This creates a shadow region at the faces of the bar. The shadow region is applied a coupled boundary condition.

In my cell-zone condition I get two regions one solid and other as fluid. To the solid region I have specified a source term with vol. heat generation of 3000W/m3. I have activated gravity as -9.81m/s2 in y-direction. My domain material is air whose boussinesq approx. for density is activated.

My dimensions for the bar are 50mmx27mmx1000mm. The domain is roughly of the dimension 350x435x1000mm.

For the temperature contour, I have taken a plane that is perpendicular to the length(1000mm) of the bar at its approximate centre.

I used standard initialisation in both cases with initial temperature as 303K. I actually wanted to see the effect of heat generating bar in a enclosed container, hence I directly gave a heat generation to the solid material. Shall I try for constant temperature at the walls of the bar?

That explains a lot. What we have is a conjugate heat transfer (CHT). I am not an expert for this in fluent, but anyway you should use the search function of the manual to see how this problem is usually dealt with.

The basic problem is that the time scale at which the temperature of the solid changes is orders of magnitude higher than the fluid time scale (both the momentum and the energy time scale)
So when you simulate with a time step size of 0.01 for 4 seconds, the bar has only heated for some mK but you need the small time step size for correct simulation of the fluid flow.

The problem is caused by the huge difference between the heat storage capacity of the solid and the fluid.
So running the simulation with a temperature boundary condition instead of the solid bar will help a lot.
But since you are really interested in the temperature distribution within the solid (which will be almost perfectly uniform for the simulation parameters you have right now) you will have to perform a proper CHT simulation.

@flotus1:

Well, I have already referred the manual for convective heat transfer. It says one has to create a double sided wall i.e. the shadow region which I have and apply coupled boundary condition to it. Or, one can use the shell conduction model where we have to specify wall thickness, while specifying heat generation value in boundary condition for the particular wall. I first tried with shell conduction model, the problem is what wall thickness should I specify? I did not get much satisfactory results when I put tried with arbitary values. Hence, I adopted this approach as covered in an Ansys tutorial ("printed circuit board + heat generating chip" tutorial).


Well, what you told about time scale is really valuable! I need to study that, as I have not paid much attention to it till now.

Also, I am actually interested in temperature distribution in the air domain, not in the bar. Earlier, i used to boolean subtract the bar from the domain, but that meant I had to use heat flux(W/m2) at the walls of the bar. In order to model more accurately (so as to match with practical situation) I tried CHT which enabled me to put heat generation in the bar.

I will try the simulation using constant temperature at the walls of the bar, and let you know the results.

For your case, you can convert the volumetric heat generation rate inside the bar [w/m³] to a surface heat generation rate [W/m²] if you dont want to use a temperature BC.
Just match absolute heat generation rate for both approaches.
The result will be the same: no problems caused by CHT.

I tried with steady simulation constant temperature boundary condition at the walls of the bar. I tried using boolean subtract approach and also tried the conjugate heat transfer approach. Both cases I did not get convergence. Though the nature of the temperature contour looks okay.

I was searching for reason behind flattening of residual's curves. I came across a post that asked to scale the units. The fluent manual mentions that by default fluent takes dimensions of model in SI unit. So, if our model is created in millimeter we need to scale it. I scaled my model accordingly, initialised the problem. The surprising part is that I get convergence in the first iteration. Now, I have the feeling that their is something seriously wrong in my modeling of the problem. Can any one shed some light on this...?

You can easily check if the scale of your mesh was interpreted correctly by fluent by clicking on "mesh" -> "check"
You will get some usefull information about the extent of the mesh.
This should be the first thing you do when you start a new simulation.