[pythag0ra5]

Hi all,

I have a problem understanding the conjugated heat transfer mechanism present at my model. The geometry consists of a block of copper (Dimensions: 10 mm (width) x 10 mm (height) x 100 mm (length) with a circular cutout (diameter 5 mm). Air at a temperature of 200 K and an inlet velocity of 1 m/s flows through the circular cutout of the copper block. The copper block has an initial temperature of 300 K and has a convective heat transfer of 10 W/m²K to the ambient temeprature of 300 K. Due to symmetry, I only modelled 1/4 of the problem. I set up my simulation model following the official ANSYS Tutorial Heat Transfer from a Heating Coil and the advice given in this video tutorial.

After the simulation, I evaluated the average temperature of the with this expression:

volumeAve(Temperature)@Solid

The results look pretty much how I would expect them. I evaluated the temperature at both the solid and the fluid symmetry wall. You can see how the cold air stream gets heated up by the solid with increasing pipe length. The image below shows the results from a steady state simulation:

steadystate.png

I simulated 3 different cases and evaluated the average temperature of the solid accoroding to the formular stated above:

1. Steady state simulation: 279.0 K
2. Transient simulation (duration: 3.600s = 1h / timestep: 10s): 269.2 K
3. Transient simulation (duration: 18.000s = 5h / timestep: 10s): 269.2 K

I always thought that the steady state simulation represents the final solution after a certian (unknown) amount of time, whereas a transient simulation also provides information about the history of the solution. However, the results above tell a different story, do you have any explanation for that? It would make sense to me if both transient cases would predict higher temperatures compared to the steady state case. Just for the record: All cases use the same BC and the same mesh.

Many thanks in advance!

[ghorrocks]

Before you go reading too mush into the results, have you done the basic checks that your simulation is accurate? If your simulation is inaccurate your results are rubbish so trying to read anything into the results is going to end in confusion. Read the FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

So:
1) Check your convergence is OK. I bet this is where the problem with your steady state simulation is ..... For CHT simulations you should include imbalances as part of your convergence criteria as only the imbalances checks that you have global conservation - and conservation of heat usually takes a lot longer than conservation of momentum in CHT simulations.

So do another simulation with the residual tolerance 10x tighter and the imbalances 10x tighter. If it is the same as your previous simulation then you are OK. If not you have to tighten the tolerance by another 10x and keep going until you obtain convergence.

2) Check your mesh resolution. Repeat the simulation with half the mesh element edge length. Keep refining until you converge.

3) Check your time step size for the transient simulation. Halve the time step size and keep refining until you obtain convergence.

Only after you have shown your simulation is accurate can you start thinking about what the results mean.

[pythag0ra5]

Dear Glenn,

thanks a lot for the advice with the imbalance, that saved my day . I had to run the steady state simulation much longer to obtain convergence of the thermal energy. The (converged) temperature of the Solid is now 269.5 K, which is in accordance to the transient simulation.

Once again, thank you very much for helping me!

[ghorrocks]

OK, you found a big error. But don't forget the rest of the comments in case there is a smaller error - make sure the other key sources of error are under control.