hi all, i have problems in finding the right timestep for my simulation. i am trying to get the temperature on an enclosure that comes from a rotating coupling (10500 rpm). i have a fluid domain and a solid subdomain. when i´m using the auto timescale for both, i get the wrong temperature, only with physical timescale and a solid timescale of 100 i get the right temperature but the imbalance for H-Energy-Fluid is always at about 100%. Can someone help me with this?

Florian

Hi Florian,

Is your simulation properly converged? It doesn't sound like it. If it is not converged your results can show anything. Check the RMS and max residuals are OK, and the imbalances are OK.

Also, I think you are doing a CHT simulation. Getting convergence is always a bit tricky with these types of problems due to the different timescales present in the solid and liquid domains. If you are getting 100% imbalance for your energy equation in the fluid domain then you are definitely not converged. I would continue running to a much tighter tolerance then what you currently have, and maybe increase the solid timescale factor.

I would use either physical timescale or local timescale factor for your timestepping too. Auto timescale is often too small.

Glenn

Be careful when interpreting 100% imbalance in your CHT region. If there is only one boundary condition, i.e., your fluid solid interface, then this number is meaningless.

Neale.

what are you meaning with "meaningless"? I should not care about this? can you explain to me the reason for this? thanks Florian

Hi Neale,

I don't understand what you mean. You always need to get the energy equation to balance. The only time when the energy equation will not balance is when you have a steady state simulation with a heat flux on one wall and adiabatic walls everywhere else, and this is set-up is badly posed and not physical - so this will not converge anyway.

regards, Glenn

Guys,

Say for example you have a single CHT solid block completely surrounded by fluid and you have defined a single fluid solid interface between that CHT solid and your fluid domain. The flow is going around the single CHT block, cube, whatever, the geometry does not matter.

In this case there is only *one* non-zero flow through the interface into the CHT solid and the flow into solid = - flow out of fluid.

The percentage imbalance = sum of all flows through domain boundaries divided by the maximum flow through the domain boundaries.

In the case that you only have 1 flow the percentage imbalance is 100% because you you only have one flow to normalise by. In an ideal world the net flow through the single fluid solid interface would be zero, but this is not an ideal world. The net flow is going to depend on convergence level. I suspect that even if you converged your answer to roundoff residuals the net flow would still not be quite zero and you would still get 100% imbalance.

Is that clear.

Neale

Hi Neale,

I see what you are getting at, but I think you are wrong. The heat flux which would be going through the solid/fluid boundary is balanced by the temperature change in the fluid and solid. A fully converged solution would have this balanced, leaving an imbalance of zero.

Glenn

I think Neale will be right, because i used a monitor point on the surface of the solid, and now i can see that the temperature doesn't change anymore and my residuls reached a value of 10^-8 (RMS). The temperature is the same as it had been measured on the surface and the imbalance (H-Energy-Fluid)has reached 100%. Florian

Hi Florian,

I still remain to be convinced. Make sure the solid time scale factor is high enough. Last time I did a CHT simulation by far the slowest thing to converge was the T-Energy balance in the solid object, so it is possible it is not moving enough to be seen each iteration.

Regards, Glenn

For the solid I took physical timescale with a solid timescale of 500. My T-Energy balance reaches 0% only the H-Energy of the Fluid remains at 100%. Florian

Hi Florian,

Sounds strange that the fluid H energy equation did not balance. Are you sure your simulation is well posed (that is, actually physically possible)? I think you already said you converged to RMS 1E-8, so convergence should be OK.

Regards, Glenn

Hi Glenn

OK, I can accept that you don't agree. Try it sometime you will see.

You are right when you say that the heat flow (flux, whatever) through the CHT interface from the fluid to the solid should be balanced by the temperature gradient. If the world were ideal the "net flow", in my rudimentary example, through the entire interface will be exactly zero, which then should give 0% normalised imbalance.

However, things are not ideal. There are round off errors for example, so the likelyhood of getting exactly zero net imbalance, even with max residuals converged to round off (say 1.0E-6 for a single precision run) is basically zero.

One other possible normalisation is to use the maximium energy flow (including the fluid domain) instead. In this case you should see a much smaller number for the normalised imbalance. i.e. instead of 100% you will see something much less, say < 1%.

Neale

Hello Florian,

I agree with Glenn on this. It is very odd that you have 100% H-Energy imbalance. How is your problem setup? Does it have an inlet/outlet or all walls or what? Do you have all heat flux boundary conditions in the fluid domain, or are some T_spec?

For sure you should be able to get much better imbalance that 100% for the fluid domain (i.e. h-energy).

Dan.

Hello Neale, my problem has no inlet/outlet. it is setup with an adiabatic rotating shaft (coupling), two adiabatic side walls and one wall (the enclosure) is setup with a heat transfer coefficient and the outside temperature. Florian

Hi Neale, maybe i´m wrong with my simulation. can you suggest to me a physical timescale and a solid timescale, when the coupling rotates with an omega of 1100 1/s? i tried to use auto timescale with a solid timescale of 1000s. Regards Florian

Hello Florian,

If you are doing this steady state then a timestep of something like 1/omega is about right. Could be that the auto timescale is a bit too conservative. I think it usually gets something like 0.1/omega. So, you could try a bit higher fluid timestep.

Timestep for solid domains can also be explicity set or set to auto timescale. The flow solver uses a L^2/alpha scale for your solid domain when you select auto timescale where L is the cube root of the solid domain volume. This may not necessarily be appropriate if you have thin regions in your solid domain. In that case you want L to be based on the thin region size.

Otherwise I would say your setup should be working. If you have an h,T_inf boundary condition you are setting the temperature level. I was just worried that you had all flux conditions or something like that.

Neale