[Seeth]

Hey everyone,

I am doing a simulation of the heating process of a water tank and trying to get a good mesh for this purpose. I read that a polyhedral mesh is best for heat transfer simulations but I get a much more conforming mesh with a trimmed mesh.
Still, i have some problems to get a clean mesh around the heating module and the temperature sensor (just some smaller irregularities). I have tried all kinds of things to fix it but didn't manage to.

I will add some pictures to show you my model and mesh.

Thanks in advance!

[me3840]

What makes it look unclean? The only problem I see here is your prism heights need adjustment to transition better to the core mesh.

[Seeth]

In Picture 1 and 3 you can see a thin line on the top side of the prism mesh, running through multiple of the layers. Why is it generated, it just seems wrong to me?
Also what would be a good transition ratio between thickest prism layer and core mesh?
Is it better to use this mesh compared to a polyhedral mesh (I read that polyhedral is better for heat transfer but as I mentioned, I get a more conforming result with this one)?

[tisa]

Originally Posted by Seeth

In Picture 1 and 3 you can see a thin line on the top side of the prism mesh, running through multiple of the layers. Why is it generated, it just seems wrong to me?

It is probably not really that way. Your plane just cuts through cells. Use the derive part "Cell Surface..." and as its Part use your plane from before. You will probably see that there are no extra cells.

[Seeth]

Thank you, I will try that out

[me3840]

Originally Posted by Seeth

Also what would be a good transition ratio between thickest prism layer and core mesh?
Is it better to use this mesh compared to a polyhedral mesh (I read that polyhedral is better for heat transfer but as I mentioned, I get a more conforming result with this one)?

The other comment on the lines in the prism layer is correct. Anyway, for these questions:

A good transition ratio is 1. Usually 1 to 0.5 is fine.

Poly meshes are not necessarily better for heat transfer. Poly meshes are nice because (in STAR-CCM+) they are conformal across multiple parts, which means you don't need possibly nonconservative interpolation across parts. However you don't have multiple parts, so this is not useful to you.

Poly meshes have lots of faces on every cell, which make them good at resolving flows with lots of curvature. But you have a domain which is mostly vertical under convection, so a lot of your flow is really not strongly curved. For flows that are mostly straight, hex-type meshes are superior, which happens to be what you're using. So I'd stick with the trimmer for this one.

[calim_cfd]

Poly meshes are usually superior because you have more faces, which means more flexibility with flow resolution. However, since you're solving a finite volume problem, the size of your problem scales with the number of faces as well as control volumes. So you may have a heavier case with the same number of control volumes because you simply have more faces per volume. Trimmed meshes usually work with hexaedrons (6 faces), however, there's an option in starccm for you to use regular 12-14faces polyhedrons mesh using the trimmed meshes. It is sort of a mid-term between hexa and full polyhedron I'd say.
Regarding the heat transfer, you usually need to resolve the Boundary layer with a low-Reynolds turbulence models, if your case is not laminar. Also, check how similar the thermal boundary layer is with the momentum one (Prandtl number) so you can judge whether your boundary layer height and density if fine enough to resolve the thermal boundary layer. If Pr <1 & if your resolution is ok for the momentum diffusivity*, it should be ok for the thermal diffusivity, otherwise you should refine accordingly.

[Seeth]

Thank you very much for the advice and insight on the mesh types. Since my heat transfer problem is relatively simple, I will be using a laminar flow type (the only flow happening here is by convection). For the thermal boundary layer I will check if my density is fine enough to resolve my problem.

One more question regarding time steps and convergence. I have experimented with different time steps and inner iterations, first on a more course mesh and also on the current mesh. However I am struggling to get good convergence in my residuals. Is there a rule of thumb for the choice of time step and inner iterations? Also, should I increase the under-relaxation factor for the fluid flow if I keep having convergence problems (right now it is at 0,9)?

[calim_cfd]

Hi.
Since you're working with laminar flows with buoyancy/convection mainly, careful. First, it seems from your comment that you're running an implicit transient solver, yes? If that's the case, (i'm not 100% sure on this, i'd have to see some dimensions and bc settings) but i'd guess that your residuals won't go down much (1-2 order) and will just oscillate. Else, if you're running a steady state solver, the results will also behave much like a transient solution. This is just the software computing a cigarette's smoke convection like flow, which just oscillates indefinitely. I guess that's the case. So don't expect your relative residuals to go down much. Maybe your absolute residuals? It all depends on your case.


As for the relaxation factors, assuming you're taking about the equations' factors, such as U, P, Rho, k, etc, the default values usually suffice, but you can start to sooth your solution by setting the velocity one as low as 0.3, maybe less, and see if it helps. Please notice that the lower the relaxation factor, the longer your simulation will take. Beware of that instability can also come from poor meshes and bcs and dealing with these factor will just waste your time. Increasing the relaxation factor it's kinda going the opposite direction of its purpose even though it can be done in very rare cases i guess.


As for the inner and outer iterations, default should again suffice. Only if you wanna control very tricky cases because you either can't remesh your case or need to change bcs, and the like. Or if you wanna speed things up because you know the time scales of your problem and you're confident in forcing different time increments and steps.



hope it helps

[Seeth]

Yes, I am using the implicit transient solver and my relative residuals dont go down much and oscillate as you described, good to know that this is kinda expected.

As for the relaxation factors, I have them on default and will probably leave it there for now after what you´ve told me.

The default time step in my case is 1s with a maximum of 5 inner iterations, I guess i will keep it like that for now and do some test runs. Since the heating of water is relatively slow anyway, 1s timestep should suffice.

Thank you very much for your detailed advice