[bienxanh1901]

Hi everyone!
I am developing the IBM (immerse boundary method) for incompressible flow with heat transfer model, and i have a problem when simulate a validation case as shown in the picture of the cross section of domain:

https://goo.gl/photos/9iu3dR8ZWhAyTASX9
The temperature decreases lower than 20oC and may be negative if i run with coarse mesh. i have refined the mesh, and the temperature still lower than 20 at that area.

i know that is the instability area. but i do not know how to fix this problem, because i only have a little experience in heat transfer.
please help me!
many thanks.

[sbaffini]

Well... there might be an infinite number of causes for this, the specific IBM implementation being only one of these. You should give more details.

In general, a temperature out of bounds is generated by some non bounded interpolation (either in the scheme or in the ibm interpolations).

But there might be a bug anywhere.

I would exclude the instabilty as cause, unless it actually leads to the case blowup.

[FMDenaro]

Originally Posted by bienxanh1901

Hi everyone!
I am developing the IBM (immerse boundary method) for incompressible flow with heat transfer model, and i have a problem when simulate a validation case as shown in the picture of the cross section of domain:

https://goo.gl/photos/9iu3dR8ZWhAyTASX9
The temperature decreases lower than 20oC and may be negative if i run with coarse mesh. i have refined the mesh, and the temperature still lower than 20 at that area.

i know that is the instability area. but i do not know how to fix this problem, because i only have a little experience in heat transfer.
please help me!
many thanks.

Does your code works in a flow problem without any IB body?
How about the discretization of the internal energy equation?

[bienxanh1901]

Originally Posted by sbaffini

Well... there might be an infinite number of causes for this, the specific IBM implementation being only one of these. You should give more details.

In general, a temperature out of bounds is generated by some non bounded interpolation (either in the scheme or in the ibm interpolations).

But there might be a bug anywhere.

I would exclude the instabilty as cause, unless it actually leads to the case blowup.

Hi sbaffini!
Thank you for your supported.

These pictures are detail information of my case:

https://goo.gl/photos/FhZUDyz3zqgSLASp7
This is the domain in IBM method:
- Green field: fluid (only solve this field).
- Red field: solid.
- Blue line: Forcing points.
- Black line: immerse boundary.

The grid point size is about 0.13 mm.
I use LES Smagorinsky turbulence model.

My model use both forcing and ghostcell points. The interpolation and extrapolation are in first order (3 points).

And here is the solved temperature field:
https://goo.gl/photos/FzvCKzDDQfw9NNfQ7

I have rescaled from 19.5 to 20.5 oC to see the low temperature points.

Thanks!

[bienxanh1901]

Originally Posted by FMDenaro

Does your code works in a flow problem without any IB body?
How about the discretization of the internal energy equation?

Hi FMDenaro!
Thank you for your reply!

My code use FVM (finite volume method) for spatial discretization and Mac-Cormack predictor-corrector for temporal scheme.

My code had validated with many case, include none IBM and IBM, such as, Channel flow, Periodic hill, Wavy flow, Tube, Echangeur, ...vv.
This problem occur when i simulate a geometry that have a corrner like this case.

[FMDenaro]

Originally Posted by bienxanh1901

Hi FMDenaro!
Thank you for your reply!

My code use FVM (finite volume method) for spatial discretization and Mac-Cormack predictor-corrector for temporal scheme.

My code had validated with many case, include none IBM and IBM, such as, Channel flow, Periodic hill, Wavy flow, Tube, Echangeur, ...vv.
This problem occur when i simulate a geometry that have a corrner like this case.

From the temperature field it seems more a numerical instability, not a problem due to the corner.
The static Smagorinsky model add further viscosity and conducibility so that you need to consider the time step value based on the viscous stability constraint.
Reduce your time step but I suggest to run a case without SGS model.

[sbaffini]

I have to take back what I said before, this looks like a genuine instability to me too.

However, if you always have problems with sharp corners, that might be something to look at closely.

What do you mean by forcing AND ghost cells? Could you explain more? I am also confused by the fact that you use forcing in mesh points (the blue line) but you use a FV method.

One thing I can think of is that, as you actually have a field also within the body, in sharp corners (and in many other cases) you might end up having the same red cell which has to provide values for 2 really different neighbor green fluid cells. How do you handle that?

[bienxanh1901]

Hi FMDenaro and sbaffini.

I had refined the mesh resolution and decreased the time step before. the temperature result is improved but still lower than 20 at that zone.

I am intend to use UDS in the energy equation. Is that the good idea?

[FMDenaro]

Could you post the temperature field for this improved solution?

Consider that:

1) the static SGS Smagorinsky model require a constant as input. How about the value you fixed?
2) In no way you can perform a LES using a first order upwind discretization.

[arjun]

Originally Posted by bienxanh1901

Hi everyone!
I am developing the IBM (immerse boundary method) for incompressible flow with heat transfer model, and i have a problem when simulate a validation case as shown in the picture of the cross section of domain:

https://goo.gl/photos/9iu3dR8ZWhAyTASX9
The temperature decreases lower than 20oC and may be negative if i run with coarse mesh. i have refined the mesh, and the temperature still lower than 20 at that area.

i know that is the instability area. but i do not know how to fix this problem, because i only have a little experience in heat transfer.
please help me!
many thanks.

the symmetry BC is not possible here.

[bienxanh1901]

Originally Posted by FMDenaro

Could you post the temperature field for this improved solution?

Consider that:

1) the static SGS Smagorinsky model require a constant as input. How about the value you fixed?
2) In no way you can perform a LES using a first order upwind discretization.

Hi FMDenaro!

here are the Temperature fields of the case (DX = 0.13mm, DT = 2e-5 s)
https://goo.gl/photos/GCs6pxjvYUPNmLq9A

and case ((DX = 0.09mm, DT = 1e-5 s)
https://goo.gl/photos/fVzb8wapVSwyWRxF6


I use fixes value of Cs = 0.1 and Prt = 0.71.

Should I continue decrease the time step or increase the mesh resolution?

[bienxanh1901]

Originally Posted by arjun

the symmetry BC is not possible here.

Hi arjun!

Could you explain the reason why we can not use the symmetry condition here?

[arjun]

Originally Posted by bienxanh1901

Hi arjun!

Could you explain the reason why we can not use the symmetry condition here?

What you have is geometric symmetry and not flow symmetry. You can not have flux across the symmetry condition that is there shall be no flow across it. You have an inlet perpendicular to it on the right side. That is bound to cause flow crossing that symmetry BC.

So your problem is not well defined from CFD point of view.

[FMDenaro]

To be clear, using LES no 2D hypothesis, no symmetry conditions must be used!