[Lukas Zollner]

Hey Everyone,

I am currently conducting Heat Transfer Simulations in FLUENT. I have a general question about the timestep selection for my setup. To asume a simple case, one could think of a heated cube where one face has a convective boundary condition with a high temperature while the rest is adiabatic. I know that it is possible to estimate the minimal timestep according to the mesh size with dt=rho*cp*dx^2/k as a nondimensional result of the diffusion equation. Unfortunately my material parameters (density, specific heat capacity and thermal conductivity) estimate very low meshsize for small timesteps. although for my specific problem the physicale time scales need to be small e.g. 0.01s. My estimated mesh sizes would be 5E-5m. This is far too fine considering the total elements in my domain. My current approach works->convergence and reasonable temperature development. Therefore I am interested in what effect my assumption (timestep smaller than estimated by the temperature propagation speed) has. Is it common practice to work like this? I do not see a way to meet the formal requirements without using millions of elements on my domain.

Thanks in Advance
Lukas

[LuckyTran]

You kind of have your needs backwards. You want to model a certain physical time, say 0.01s.

You generate a mesh of some spatial resolution dx.
Then you calculate the largest allowable time-step size based on stability criteria. I'm not sure you have the right stability criteria.
If the time-step size is too small, then you generate a mesh with bigger cells until you can afford it.
If you have already predetermined a mesh size, then you are stuck with a certain time-step. But the way you describe your situation sounds strange.

You are trying to time-resolve a diffusion process, which is like saying you're doing DNS. The time-steps will be small and you will need a lot of them!

Either way, you should do a time-step size sensitivity study and run it using several time-step sizes and compare the results. Heat conduction is parabolic and is quite stable and you should be able to use large time-steps if you're using Fluent since it's an implicit solver.

[Lukas Zollner]

Hey LuckyTran,

thanks for the immediate reply.
Maybe I got it wrong. let me rephrase the question.

For a given mesh in a solid heat Transfer Problem. Is there a a Problem if timesteps are getting too small. Thats not a question of computational cost now. Example: Say my mesh size is 1mm with that i calculate a timestep as 3s or so. If i now go below that timestep in my configuration, is it good practice?
Check out this COMSOL link. They explain the Problem.
https://www.comsol.com/forum/thread/...0-21T13:43:33Z

P.S: I know COMSOL is a FEM Solver but I think the Problem stays the same

[LuckyTran]

Using a smaller time-step than the maximum allowable is a very good idea. You should always do this.

The stability criteria often limits the maximum time-step, not the minimum. It's unlikely you'll be able to run a small enough time-step that's still physically meaningful where the truncation errors become significant. You should always be able to go smaller.

I don't see the relevance of the COMSOL discussion you posted or which part of the discussion you are even referring to. There is no problem except the one that you made up. Just run it....

[Lukas Zollner]

I think this effect might realy just be realeted to FEM approach. I did check if different time stepping has effect on the solution and it is very Little effect. decreasing timesteps for various meshs showed the same effect.
However, when I compare different meshes I obtain different temperatures at randomly distributed points and planes. Therefore, the Problem seems to be sensitive to the grid.
Any idea where this effect can come from? I only have solid heat tranfer and tried various meshes

[LuckyTran]

Originally Posted by Lukas Zollner

However, when I compare different meshes I obtain different temperatures at randomly distributed points and planes. Therefore, the Problem seems to be sensitive to the grid.
Any idea where this effect can come from? I only have solid heat tranfer and tried various meshes

That's very typical. The solution will depend on the grid an also depend on the time-step size etc. A lot of people spend a lot of time to figure out the right grid and time-step size to make their solution insensitive to these parameters (so-called mesh sensitivity studies and time-step sensitivity studies).

What does your mesh look like? Is it smooth? Is it all tets? If you use a tet based grid the topology can easily change even with a tiny change in cell count and you can easily get wildly different results. If you use a more regular smooth grid, like all cubes, then the grid topology does not change much and it is more robust but still you should expect some sensitivity.


Of course I assumed you already know how to run enough iterations per timestep to achieved inter-timestep convergence...

[Lukas Zollner]

In order to check grid sensitivity and sensitivity to temporal discratization I tried various grids and timesteps.
Mostly I am using a grid containing hex and tet elements (But I also tried only tet and even conversion to polyhedral and Inflation at boundary). I am checking average, minimum and maximum values for temperature in the cell zones as well as specific randomly distributes Points.
Now, looking at one mesh I observe little effect by varyiing the timestep. So far that was what I expected.
However when just refining a mesh via element face size I get different results. Average, min and max temperatures usually show small Variation and seem to converge to a steady state with finer mesh. But comparing the specific Points I get different results. Example: Some Points show higher temperature with finer mesh. When refining more the temperature at this Point can be lower again. Depending on the Observation Point the effect can be the other way round. I dont know if that is to be expected, considering a decreasing numerical error when refining the mesh. So the solution should "converge". Is there a chance, that FLUENT interpolates the area weighted average for specific Points wrong, when changing the mesh?
I simulate conduction between two solid bodies (coupled wall). one material has low conductivity 0.7 W/mK. When I increase the value, Errors become smaller.

Best Lukas