Solid Solid heat flux-Interface
 

Hi every one.

I am simulating a basic solid solid interface problem (see figure)


http://imageshack.com/a/img746/5492/n7BIUk.png

It is composed by two materials. One is Aluminum (50x0.1x5 mm) and the other is polyurethane (50x0.1x3 mm). This 0.1 mm is to convert a 3d simulation in a 2d simulation using one element thick. It is a steasy state problem in which I have applid 290 K in the 5 mm side (aluminum) and 285 K in the 3 mm side. Hence, I have a gradient of 5 degree.

The problem is:

- I am getting a 31 % imbalance energy in aluminum domain. On the other hand my balance is perfectly in my Polyurethane. I don't know why. It should be very simple and energy must conserve because I am using a conservative interface. I am getting this imbalance in my solver results and also in my cfd post using ccl comand.

I evaluate my heat flux in the 290 K side using: AreaInt( Heat Flux)@location290

In the interface in both side I am using:AreaInt( Heat Flux)@Interface290 side 1 and AreaInt( Heat Flux)@Interface290 side 2

I tryid everything: Refine mesh, use more interations, diminish residuals, change geometries and I always get imbalance in my aluminium or any other material in which I have high conductivity compared with the other material.

I have solved turbulent flow, radiation and many difficult problems in the last year, I am frustrated for my failure in this simple task.

Thank you in advanced

How much is the imbalance compared to the "radiative heat flux" at the interface ?

In this case I am only simulation heat conduction in two material with 5 degree temperature difference.
The next step would be add a radiation model to this simulation. But for now I am just trying to verify this conduction case, hovewer, this 31 % imbalance in the aluminium is freaking me out.
I simulated many different combinations of thickness sizes and temperature difference, but I am always getting a huge imbalance in the aluminium side.

Large imbalances which are slow to diminish are common in solid heat transfer simulations. The reason is because the time scales associated with heat transfer in many materials are much slower then the time scales associated with fluid flow for a similar geometry. This means that you frequently need to use much larger physical time steps than normal. So modify the simulation (I do it while the simulation is progressing) to have much larger time steps in the solid domain - 100x or 1000x the default timestep is often used.

Also I recommend adding imbalances to your convergence criteria for solid heat transfer simulations to make sure this imbalance is OK. It is not included in the convergence criteria by default and that can let major errors slip through.

How can I modify my time scale while the simulation is progressing? And how can I set differente time scales for two different domain?

Thank you

Assuming you have a steady state case, you can enable beta features and edit the domain of interest. You should now see a new Solver Control tab in the domain, and you should be able to select a Timescale for such domain.

Thank you guys, it worked out!

Just one more question. I would like to see my temperature in each cell with as much algarisms possible. When I define a point isome cells in cfd post, the temperature has only 2 ou 3 algarismos (e.g. 289.236K) However, How can I find the final temperature with more algarisms? It is not very important for my results, but my professor want to see them to compare with the analytical solution

Edit Default Legend View, or whichever Legend you are using for the specific plot. See Appearance Tab/Text Parameters/Precision.