Question about solid part of CHT (conjugate heat transfer) in CFX
 

Hi,

The tetra grids are generated for the solid part of CHT. Hexa grids are generated for the fluid part.

Then when we run the CHT simulation in CFX, will CFX use FVM or FEM to calculate the heat transfer behavior in the solid part?

Why do you have a tetra grid for the CHT part in the solid? Having separate grid types may lead to errors if it's not done properly.

The energy equation is used to calculate heat transfer flow, using the finite volume method.

Because of the geometry complexity. Why would it introduce additional errors? I anyway can't avoid GGI for this case. How to treat the separate grid types properly?

I said it might introduce errors if it's not done properly. This might be due to stuff like orthogonality, or sudden inflation etc. This obviously depends on your mesh. I've found it's a little bit tricky to control those parameters when you have tet and hex cells in one mesh.

Please read the CFX solver modelling guide, the chapter on advice on flow modeling.

Thanks. I understand there would be a problem at the fluid-solid grids interface.

Another question: tetra grids usually doesn't perform well for the cfd, does it usually work well with FVM for the solid part?

I assume the mesh laws which apply to fluids also apply to solids.

As long as you have good mesh statistics I don't see why tet region will not work well on a solid domain.

In solid regions the requirements on mesh are quite different to fluid regions. The equations to solve are well behaved numerically (no non-linear bits) which means that mesh quality is much less of an issue in solid regions. You still need a fine enough mesh to resolve any gradients (spatial or temporal), but mesh quality is not too important. So a tet grid will be fine for most applications.

The numerics do not change between tet and hex grids. CFX is a finite volume solver (regardless of the mesh type) with FEM-like integration points and flux calculations.

What is the usual mesh quality criteria for the solid part?

Do a mesh sensitivity study to determine it.

The most important parameter is to have sufficient resolution to resolve the spatial and temporal transients you expect.

Do I need to do some special treatment for the fluid-solid connection part? Like take care of the expansion ratio (if expansion ratio is still defined at the connection between hexa and tetra)?

On the fluid side you need to do the normal mesh density checks, and check the y+ is right. On the solid side just check the mesh is fine enough to resolve the gradients. You will be able to use a big jump in mesh sizes across the interface - but best check to be sure.

I generate both the hexa grids for the fluid domain and tetra grids for the solid domain by ICEM. So I suppose the grid quality button is only for fluid. Then we totally don't care about the grid quality for the solid domain at all and the solid grids quality can be very bad. And there is no need to smooth it. Right?

Do we still need to care about grid quality?

Yes in my opinion. Especially so if you want to extract heat fluxes and heat transfer coefficients.

Heat fluxes and heat transfer coefficients are determined using the temperature difference between the node at Twall and the next node adjacent to Twall.

No, I do not agree with Mr CFD. Mesh quality in solid regions is not too important. You have to have a really terrible mesh before it causes problems.

The reason for this is in the maths - in solid regions the only equation being solved is the heat equation and that is entirely linear. Linear equations are easy to solve and pretty robust numerically. So you can be rough with them and they still converge to an accurate solution. It is the non-linear terms in the NS equations (u du/dx etc) which makes them tricky to solve and sensitive to poor mesh.

The heat fluxes and HTC require good mesh quality in the fluid side, but the solid side just needs a fine enough mesh to resolve the gradients. If you do not believe me then try it out :)

in my opinion ghorrocks is right ... i made a study two weeks before and i got the following results:

i checked the heat transfer from a solid to a fluid:

the gradient on the fluid side (Tw-Tnw) is about factor 400 (!) higher than the gradient on the solid side (Tw-Tw1)

.......Solid..........Fluid
|_____|_____||_____|
|_____|_____||_____|
|_____|_____||_____|
|_____|_____||_____|
..................Tw
..Tw2....Tw1......Tnw

so u need good elements on fluid side to approximate the gradient as good as possible ...

for sure this result is what every literature about heat transfer is telling .... :)

Hi ...
I am modeling transienrt CHT with ANSYS CFX.
I did 2 simulations one without modeling solid and in the CFD wall i set isothermal B.C and i validated results with experiments. then i did another simulations with adding structure to the geometry and defing fluid-solid interface, and in the interface Conservative heat flux has been set. the temperature gradient obtaioned in the Solid looks Ok . however the pressure is strange, compare to the case without the structure pressure drops 10 times with is defenetliy wrong. so i am wondering what could be the problem. I expected the decrease in the pressure but not that much.
it seems that in my simulation solid is damping pressure oscilations in the fluid. and i don't know why.
i tried changing the solid mesh in the way that it matches with the fluid in the interface but no change was observed.
i also tried to set different B.C condition in the external layer of solid which is in contact with the ambient air: adiabatic , isothermal , heat transfer coefficient ...but at the end it just changed the pressure few pascal and the still too far from experiment.
i would appreciate any help.

Can you post the pressure you are seeing, what your geometry looks like and what you expect to see?

Attachment 24017 Geometry without solid part

Attachment 24019 pressure signal


Attachment 24018 geometry including solid
Attachment 24020 pressure signal

What effect do you expect the solid region to have on the pressure waves? Is this an FSI simulation?