[tH3f0rC3]

Hi,

I want to calculate the heat transfer from a fluid to a solid.
I have found a good mesh for the fluid region. But I can't find a good mesh for the solid region. Using the Courant number to find a good mesh also results in a bad calculation (see extention).
You can see a cut through the mesh.

Does someone have an idea?!
Maybe it is better to use the extrude option to generate the volume mesh?

I think I have to use a finer mesh in the solid region than in the fluid region. However I get bad results...

Mesh size:
solid: 5*10^-4m
fluid: 3*10^-3m


Best Regards,
tH3f0rC3

[fshak92]

Originally Posted by tH3f0rC3

Hi,

I want to calculate the heat transfer from a fluid to a solid.
I have found a good mesh for the fluid region. But I can't find a good mesh for the solid region. Using the Courant number to find a good mesh also results in a bad calculation (see extention).
You can see a cut through the mesh.

Does someone have an idea?!
Maybe it is better to use the extrude option to generate the volume mesh?

I think I have to use a finer mesh in the solid region than in the fluid region. However I get bad results...

Mesh size:
solid: 5*10^-4m
fluid: 3*10^-3m


Best Regards,
tH3f0rC3

Tell the details about your simulation,,about the meshes,,the models you activated, and pictures of your mesh.

[tH3f0rC3]

The upper block is defined as the solid region. The block below is defined as the fluid region.
The white region is set up as a mass-flow inlet and the face on the other side is set up as pressure outlet. The walls of the fluid channel are set as adiabatic. The heat is transfered between the solid and the fluid region on the interface.
The block is set as adiabatic except the top wall (not visible) (the face on the top of the solid region parallel to the blue face.

Hope you understand the simulation.

Best Regards,
tH3f0rC3

[fshak92]

Originally Posted by tH3f0rC3

The upper block is defined as the solid region. The block below is defined as the fluid region.
The white region is set up as a mass-flow inlet and the face on the other side is set up as pressure outlet. The walls of the fluid channel are set as adiabatic. The heat is transfered between the solid and the fluid region on the interface.
The block is set as adiabatic except the top wall (not visible) (the face on the top of the solid region parallel to the blue face.

Hope you understand the simulation.

Best Regards,
tH3f0rC3

I don't have enough experience in meshing,but it seems the density of mesh in right block is not so good,,But it can be easily fined by defining the mesh size of your right block,,go to solid'd region/to your surfaces/Mesh condition/checking the 'custom surface size' or ... and play with the sizes...
If you have problem again,,tell all the models(laminar,segregated...) you activated ,maybe the others can help you...

[tH3f0rC3]

That's exactly the problem. The mesh is not good.
But I can't find a good mesh. I have tried nearly every mesh size. Greater than the fluid and smaller than the solid region without success.

In the appendix you can find a result of an other mesh. The cells which are not colored are calculated with temperatur values greater than 285K or less than 282K.

The fluid inlet is set up with 363K. On the upper side of the solid the boundary "convection" is set up with an ambient temperature of 273K.

So the heat will be transfered from the streaming fluid through the solid to the upper side of the solid where the heat will be transfered as specified in the boundary. (alpha=5000W/m²K, T=273K).

fluid:
Water

solid:
density: 2000 kg/m³
specific heat: 800 J/kgK
thermal conductivity: 3 W/mK

The Courant-number for these two regions is very different.


Best regards,
tH3f0rC3

[siara817]

I think it is better to check the quality of the mesh using, Drived parts/Threshold.
check the cell quality. then see where does have the lowest quality. I would appreciate if you could give some information about the dimensions of your geometry, including fluid channel and solid box.

[Ladnam]

If the fluid region is the thin block and you have only two cells across the thickness then it is too few. You can use prism layer and polyhedral as meshing models. Check Y+ values if you use turbulence.

[tH3f0rC3]

Originally Posted by Ladnam

If the fluid region is the thin block and you have only two cells across the thickness then it is too few. You can use prism layer and polyhedral as meshing models. Check Y+ values if you use turbulence.

Ok, you're right.
I have used four cells. I hav uploaded the wrong picture. But the geometry is the same.
The solid block is 32mm wide, 180mm long and 15mm high. The fluid channel is 1,5mm high with the same width and length as the solid block.

Best Regards,
tH3f0rC3

[abdul099]

Not sure if I understood it the right way. The thinner region is the fluid region? What mass flow did you specify on your inlet boundary?

Regarding cell sizes: For CHT cases, it is recommended to have a conformal interface, a 1-1 connectivity of the cells on both sides of the interface. Therefore you should have the same size on both sides and also mesh them together.

[tH3f0rC3]

Originally Posted by abdul099

Not sure if I understood it the right way. The thinner region is the fluid region? What mass flow did you specify on your inlet boundary?

Regarding cell sizes: For CHT cases, it is recommended to have a conformal interface, a 1-1 connectivity of the cells on both sides of the interface. Therefore you should have the same size on both sides and also mesh them together.

That's clear. If the mesh wouldn't be like that the solution didn't work. But obviously it works although with obvious mistakes.

The mass flow on the inlet is 0.01 kg/s

[abdul099]

In fact, it works when you've got different cell sizes on both sides of the interface. But then one cell from the first side will be connected to several cells on the second side. That will smear your solution and clearly will have an impact on accuracy.
That can even happen when you have the same cell size on both sides, but mesh both regions independently.
This is NOT recommended, since it will reduce the accuracy.

Whenever you can mesh both sides at the same time with the same size, you should get a so called "conformal interface". When you initialise the interface, and it says "conformal match", you've won. In this case, every cell from the first size will have only one face connected to exactly one cell from the other side. That's one continuous mesh in the whole domain.

Maybe I will have a closer look on your model this weekend, but I can't promise that.

[tH3f0rC3]

Originally Posted by abdul099

In fact, it works when you've got different cell sizes on both sides of the interface. But then one cell from the first side will be connected to several cells on the second side. That will smear your solution and clearly will have an impact on accuracy.
That can even happen when you have the same cell size on both sides, but mesh both regions independently.
This is NOT recommended, since it will reduce the accuracy.

Whenever you can mesh both sides at the same time with the same size, you should get a so called "conformal interface". When you initialise the interface, and it says "conformal match", you've won. In this case, every cell from the first size will have only one face connected to exactly one cell from the other side. That's one continuous mesh in the whole domain.

Maybe I will have a closer look on your model this weekend, but I can't promise that.

Hey, thanks for your help!
Hope you will have a few minute time :-D

Best Regards

[tH3f0rC3]

Hi,


maybe someone else has an idea.
I can't be the first one who has this problem. There must exist a trivial solution. It is a typical CHT problem.


Best Regards,
tH3f0rC3

[tH3f0rC3]

Maybe the problem differs a little bit from the description above.

I havn't found a good mesh size for the solid region yet.
Because it is a steady-state simulation I can't use courant number to find a useful mesh. I have tried now several mesh studies without success.

Does anyone have an idea how to find a good mesh for the following material data:
density: 1380 kg/m³
thermal conductivity: 1300 J/kgK
specific heat: 5 W/mK
plastic material: PET

Best Regards,
tH3f0rC3

[tH3f0rC3]

Does someone has an idea how to mesh a continuum with a physik like this to calculate steady state heat conduction?

Best Regards,
tH3f0rC3

[abdul099]

I can't understand your issues. I tried to model your first geometry, the two blocks etc. according to your description. It has been working pretty nice. The results are reasonable, no issues found.

You're right regarding your second last post: It's a typical CHT case, and there's a trivial solution. But I don't now what your problem was. Maybe you can describe a little better which steps you did to get the model with you're experiencing issues.

Regarding your last post: A conduction problem shouldn't cause any trouble. Just try to mesh it, run for some hundred iterations and look at the results. When the gradients are too high, refine the mesh. There should be no huge temperature jumps from one cell to the next.

[tH3f0rC3]

I have still the same problem. I can't find a good mesh.
I will now describe exactly what I'm doing.

I want to calculate the heat conduction inside a PET block:
The solid block is 32mm wide, 180mm long and 15mm high
density: 1380 kg/m³
thermal conductivity: 1300 J/kgK
specific heat: 5 W/mK
plastic material: PET

The heat will be transfered from a streaming fluid (Water) so one side of the solid (PET).
T(in)=90°C
Thus the two interfaces between the solid and the fluid are set up for heat transfer. The other walls are set up as adiabatic with the exeption of the upper side of the solid block (across from the interface between solid/fluid) which is set up with a thermal specification: Convection (alpha=5000W/mK and ambient T=253K)
The fluid block has an inlet and an outlet in longitudinaldirection (length of the block). The massflow is 0.01kg/s.

Now the question is how to mesh. I can't find a useful mesh thus I can't give more specifications here. I have tried nearly evers mesh size from 0,01m to 0,0001m without success.
Maybe abdul can give me some details from his simulation so that I can compare it to the one I set up.

Best Regards,
tH3f0rC3

[abdul099]

Can try.

I've meshed the geometry you posted the last time: Solid block 32x180x15mm, water region 32x180x1.5mm.

I applied the following sizes / models, using version 7.02.008:

Base size 5mm
Min surface size 25% (default)
Target surface size 100% (default)
Nearly all other mesh values are default, except:

Embedded thin mesher activated
Customize thickness threshold activated
Thin mesher layers and thickness treshold: nearly arbitrary. To be set on region level, otherwise it might not work

On region level (water region only)l:
Thin mesher layers: 4
Thickness threshold: 2 mm (only needs to be bigger than the water region thickness to allow the thin mesher to detect the water region to be thin)

Make sure, per-region meshing is NOT ticked (mesh continuum). Also make sure, you've created the interface between solid and fluid region before meshing. Then you will get conformal interfaces, which gives the best accuracy.

The I hit the volume mesh button and got a mesh with 29520 cells, which is nearly nothing.

Specified the boundary conditions you've given here and run for some iterations. After about 50 iterations, the results looks pretty nice. See picture Pic1.png for details.

Of course, the mesh is very coarse. Refining the mesh (e.g. base size 2.5mm) and put more thin layers (e.g. 8) would rise accuracy of the solution (and of course, increases the mesh size. In this example, 140k cells).
The results will still look great after some iterations (see Pic2.png)

Both simulations run laminar. You didn't give any information whether you tried it laminar or turbulent, so I tried both.
After switching to turbulent (realizable ke two-layer model), it still looks fine. You can see a slight jump for the heat transfer through the top boundary since the water will transfer more heat to the solid (See Pic3.png). This is expected due to the higher mixing due to turbulence effects.

I could keep refining the mesh, but I've got only an old quad core Phenom II, so I'm not patient enough. I hope you'll belive me when I say, you can achieve good results when you put the right settings. I haven't done any comparison to theoretical results or experiments, but I assume, the solution will not change much when I keep refining the mesh.

I've got absolutely no clue why it didn't work for you. I hope this information will help you. Let us know when you still experience any issues, but when you do so, I would need the sim-file. I'm running out of ideas without seeing your setup.

[tH3f0rC3]

Many thanks for your help.


Could you please upload a screenshot of the temperature distribution in a x-y plane (in my simulation the y-z plane) in the solid block? In this plane you will probably see the temperature distribution as a chessboard. (see pic)
And this is the problem.

I've tried your set up and I'm have still the same problem.

Best Regards,
tH3f0rC3

[abdul099]

Sure, can do. See the attached pictures. Now I see what your issue is. For me it was just the expected behaviour, resulting from the mesh resolution and the position of the section.

Your mesh is just not fine enough. You can see that in my first picture. A coarse mesh will cause the plane section to cut through cells with different temperatures, resulting in that chessboard pattern. A little more explanation: The cell center of neighbored cells have different distances from the boundaries and therefore the cell needs to have a different temperature (due to the temperature gradients).
I didn't see this as an issue since it's the behaviour I'm expecting when my mesh is not fine enough.

You can see, the pattern improves a lot when you refine the mesh like I've done in the next two pictures. Don't forget, your domain is just a thin slice, heated from one side and cooled with a very high heat transfer coefficient from the other side. There is a high temperature gradient in your solid, and you need a lot of cells to resolve that properly.
What you always should do: Look at your results, and when there are too big jumps in the results, refine the mesh. I've already wrote that, see my post from 31 May:

"Just try to mesh it, run for some hundred iterations and look at the results. When the gradients are too high, refine the mesh. There should be no huge temperature jumps from one cell to the next."

What you see in your case is exactly what I've described. I'm sorry when it wasn't clear enough what I intended to say.