[mariashva]

That's very kind of you. I will prepare the geometry file and send to you later, maybe you can give me some ideas about mesh and interface/contact.
I tried to using fine mesh with inflation, and hex dominant with only tet mesh in some region. I got good converged results. The residuals go down to the limits without going up in the middle. So I guess this result is better than my previous cases. I will do a parametric study on mesh size.
For the interface and contact. I have a case, like a flat surface half contact with a chip surface, another half contact with fluid domain. But Fluent doesn't cut the surface properly for interface settings. Do you mean I need to cut the face manually in design modeller, and then the faces will be automatically shown as in a pair in Setup? Is there any other automatical way to do it? Because in my Fluent setup, some faces can be automatically cut for a right contact but some are not. Not sure if it is because of the mesh quality in different regions or because the software is not that clever to do all the faces right...

[Lucas_Gasparino]

Ummmmm... Face splitting for interfaces generally is a manual procedure. What I do is generate the cut on SolidWorks, since it allows to project a sketch on the face without breaking the body. It may be more troublesome, but guarantees that you have all correct interfaces positioned and defined. Yes, models with contact/interface are a pain...
In general, if you're sure about the Cfd numerics used, but the results look sketchy, try different meshes and refinements and see what you get. In general, refined meshes give more accurate results in less iterations, but require processing power. Linear tets are standard in industry, but be aware that they only work well with node centered methods. In general, you want to introduce small perturbations to your model: if you're using structures mesh, introduce a but of asymmetry in the domain, otherwise you'll not set physical instabilities. Ansys meshing really isn't the best for unstructured hexa, but you can use cut cell methods, which will resemble more like traditional FV meshes. To be fair, I'd rather Ansys convert fluent to a FE approach: it's more robust and deals better with tets, as well as it's easier to implement higher order elements that eliminate the LBB condition. About inflation, it's only useful for turbulence or if you know generally where strong shocks will form on compressibilidade high speed flow. Elongated elements on complex geometries can result in meshes with high skewness, and that's something you want to keep low. Finally, laminar problems do achieve mesh independence: so run at least 2 levels of refinement and see if it converges to your validation. I'd just recommend that you get used to Paraview for post processing: CFD post is... limited. Finally, when you feel comfortable with fluent, start learning ICEM mesher, or TGrid: they're far superior to the standard workbench stuff. ICEM now has a lot of YouTube tutorials, so give it a try!

Sent from my XT1635-02 using CFD Online Forum mobile app

[mariashva]

Thank you for your great explanation. A quick question, 2 levels of refinement meaning?

[Lucas_Gasparino]

Originally Posted by mariashva

Thank you for your great explanation. A quick question, 2 levels of refinement meaning?

Mean refine the mesh twice, to be sure of your results. Preferably, each time by 1/2 of the original size. Since it's unstructured, set the global controls to half their values

Sent from my XT1635-02 using CFD Online Forum mobile app

[Rajaero]

Hi,
if i dont know the solid temperature and heat flux and heat transfer coefficient value but i have inlet air velocity and pressure and air temperature. if it is the case then how can i set a boundary condition for my simulation to find out the convection heat flux and heat transfer coefficient by forced convection.
i tried alot, i will appreciate if someone help me...
thanks in advance...

[Lucas_Gasparino]

Hi there!
First, you need at least some form of heat coming from the solid: you can set an initial body temperature and let it cool, for example, or you can infuse some heat through a surface on said solid.
That said, fluid/thermal simulations require no definition of Nu or h whatsoever: that comes from the thermal boundary later formed during fluid flow. However, your solid surface still must have an initial temperature, that will be diffused after the flow passes through it.
I'd suggest that you take a look at Incropera book, it's the best I know. Then, in the cfd, you have to set a solid/fluid interface on the touching walls, and turn on the energy equation. Don't forget to model the fluid as non isothermal! Finally, the solid needs only the conduction property, as Fourier equation in the solid requires it when you have convection (becomes a Poisson eqn.)

Sent from my XT1635-02 using CFD Online Forum mobile app

[Lucas_Gasparino]

Can you give more details?

Sent from my XT1635-02 using CFD Online Forum mobile app

[Rajaero]

thanks for your suggestion. my case is solid fluid interaction problem as you said. its aforced convection so ineed to use velocity inlet and pressure outlet boundary condition. as per your suggestion i will set the initial temperature for solid body.
non isothermal condition for the fluid model means i should not give a constant temperature right. if it is the case what boundary i should use for the fluid domain.
thanks in advance...

[Lucas_Gasparino]

Yeah, that's it. Now, the only thermal fluid bcs should be inlet temperature and adiabatic external walls, so there's no heat loss to outside ambient. If it's flow inside a pipe, you could set radiation in the external walls, or heat flux per m2, or a convective coefficient.

Sent from my XT1635-02 using CFD Online Forum mobile app

[Rajaero]

thanks for your reply,
i have done everything correct. but i set a wall temperature for the fluid domain wall (isothermal). now i understood the problem. i will try as per youer suggestion. if i get the solution i will let you know.

thanks alot man, i really appreciated your help.

[Lucas_Gasparino]

No worries! Glad to help. Did you check the reference I told you about?

Sent from my XT1635-02 using CFD Online Forum mobile app

[Rajaero]

not yet. i will check it

[Lucas_Gasparino]

Just a tip: try your case without turbulence first, then check the effects of higher Re and the impact of different turbulence models... If you have a metric load of storage, run a SAS case (must be transient), so as to have a realistic simulation

Sent from my XT1635-02 using CFD Online Forum mobile app

[Rajaero]

ok bro i will do that

thanks...

[Rajaero]

Hello,
i am doing fluid and solid coupled interface problem to find out the heat transfer coefficient. i have solved the case and got h value.
But,
There are two interface was created by fluent. so if want to calculate h value then which i need to choose?
for example,
Area-Weighted Average
Surface Heat Transfer Coef. (w/m2-k)
-------------------------------- --------------------
all-solid-contact_region-trg -14.667882
contact_region-src 41.948711
in this which interface value i should consider? or i need to calculate the net value?


is reverse flow becuse of following reasons?
1.mesh quality
2.outlet domain is too short.
3.chage pressure outlet to out flow condition (can i set outflow condition if ideal gas was used?)

Reverse flow will affect the solution or it only affect the convergence rate?

thanks in advance..