CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   chtMultiRegionFoam and Ychar and Ypmma fields (http://www.cfd-online.com/Forums/openfoam-pre-processing/93643-chtmultiregionfoam-ychar-ypmma-fields.html)

Lada October 21, 2011 13:20

chtMultiRegionFoam and Ychar and Ypmma fields
 
I am playing around with the chtMultiRegionFoam solver and struggling with undersdanding what Ychar and Ypmma fields are for. They seem to apply to solids only.

Could anyone clarify meaning of those for me, please?

Having grepped the entire foam directory I found them in the multiregion tutorials only.
Do I need those fields when modeling a multiple solid case?

Thanks,
Lada

Linse October 24, 2011 10:13

I do not know if that is the same case for this tutorial case, but I know from combustion simulation that "char" is most of the time used for kind of inert fractions, while "pmma" could be used for poly-methyl-met-acrylat or some other strange substance that is not inert to chemical processes...
In general in combustion (and in chemistry-simulation as well, to my knowledge), "Y" is used as a letter defining a fraction within a mixture.

My guess would be these values are used to calculate any mixture-average-values containing pmma and char...

Lada October 24, 2011 13:05

Although it sounds convincing, I am now puzzled even more :) .

The thing is there is no chemistry or species present in those tutorials. They are just simple buoyant air flow around a solid (iron or so) material cases.

Based on what you wrote, it might be something that the author of all multiRegion tutorials forgot to remove because it is present only in time directories that relate to the solids (the changeDictionaryDict files that are used to modify boundary conditions for the particular model region (solid material), contain the Ychar and Ypmma as well).
It does not seem to be calculated as it appears in '0' directory only.

It is rather confusing.

Thank you for your response.

nandiganavishal February 23, 2013 12:58

Hi Vladimir,

I would like to know if you were able to solve the multiregion Problem. I am trying to solve a heat conductive equation between 2 solids of different thermal conductivities k1 and k2. I am using the chtMultiRegionFoam to solve this problem. I would like to enforce the following heat flux boundary condition

k1 grad(T) (region 1) = k2 grad(T) (region 2).

Kindly let me know what predefined boundary condition in OpenFoam corresponds to this BC.

Thanks

Regards
Vishal

Lada February 23, 2013 13:18

1 Attachment(s)
Hi Vishal,
if you are asking whether I have found out what those Ychar and Ypmma are for, I must tell you: no, I haven't. But for solids only calculation, they don't seem to have any meaning.
Regarding your problem. I am not clear what you want to do. Help me if I am wrong.
My understanding is that you want to solve conduction problem across two layers different in their conductivity. I would suggest that you just modify one of the tutorials accordingly.
I am not sure if what I imposed as a boundary condition between the two materials was correct but it worked (I used compressible::turbulentTemperatureCoupledBaffleMix ed for the boundary type, as it is what is in the chtMulti... tutorials).
This is exactly what is in the relevant part of changeDictionaryDict file:
boundaryField
{
".*"
{
type zeroGradient;
}
"interface_to_.*"
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
neighbourFieldName T;
K solidThermo;
KName none;
value uniform 275;
}
}


Hope this helps.
Lada

ps. please see the attached file. there is a 3 layer wall model in it which works just fine.

Linse February 23, 2013 13:28

Sorry for not answering earlier!

@Lada: If I remember correctly, sometime ago I was looking into the business with Ychar, Ypmma and so forth again. And I found that somewhere a mixed conductivity had been calculated, based on these two parameters. I think it was somewhere in the thermophysicalproperties that one had to define the different materials concerning their conductivity, mass, and so forth...

Lada February 23, 2013 14:39

Thanks Linse. I appreciate your help.
Now I know it is in solidThermophysicalProperties file of every solid region. But still have no clue what is it for. I copied coefficients for char 'variable' from chtMultiRegionFoam/multiRegionHeater/constant/heater tutorial here:

----------------------------------------------------------------------------------------------------------------------
charCoeffs
{
transport
{
K0 0.4;
n0 1.3;
Tref 300; //K0*pow(T/Tref_, n0))
}

radiation
{
sigmaS 0.0;
kappa 0.0;
emissivity 0.0;
}

thermodynamics
{
Hf 0;
C0 611.0;; // Cp = C0*(T/Tref)^n0
Tref 300;
n0 1.31;
}

density
{
rho 11.5;
}
}
----------------------------------------------------------------------------------------------------------------------
Unfortunately, I can't find much of a connection to what is defined at the beginning of the file within the constSolidThermoCoeffs section. This section was relevant to my simulations and when I modified it, it did the job I expected. I'll tinker with the char and pmma coeffs and see whether they have any effect on what I simulate.

nandiganavishal February 23, 2013 20:00

Hi Lada,

Thanks for the reply. I looked at your simulation set up files and have the following questions in the ChangeDictionaryDict file for concrete2.
"concrete_2_to_.*"
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
neighbourFieldName T;
K solidThermo;
KName none;
value uniform 261;
}

right
{
type mixed;
refValue uniform 258;
refGradient uniform 0;
valueFraction uniform 0.017871;

1. How did you know the temperature value ("261") at the boundary "concrete_2_to_.*"? What and where does this temperature value correspond ?

2. How did you calculate the valueFraction for the "right" patch boundary ?
3. What does the temperature value "258" here refer to?
4. Why did you use a mixed boundary condition ?

Please provide your reply.

Thanks

Regards
Vishal

Lada February 24, 2013 08:18

Hi Vishal,

ad 1) the temperature appears in all changeDictionaryDict files and it is an initial guess of the temperature at the interface. You can put any number there or delete the whole line and not much will happen. Maybe a few extra iterations will be needed to converge the case.
ad 2) I calculated the valueFraction according to the following formula:
valueFraction= 1 / (1 + conductivity/delta/HTC)
conductivity (W/m/K) stands for the conductivity of the material layer (concrete_1 or concrete_2) which is defined in respective solidThermophysicalProperties file of the layers (regions)
delta (m) is the half thickness of the first cell layer adjacent to the boundary
HTC (W/m2/K) is the heat transfer coefficient at the wall
ad 3) 258 is the temperature of the fluid that is at the outer side of the boundary
ad 4) as I could not find better boundary type to define the Robin's boundary condition, I had to choose the mixed one. Imagine a wall that stands between you and outdoors. You don't want to solve the flow in the room or outdoors, but you know the temperatures indoors and outdoors as well as the heat transfer coefficients at both sides of the wall. The mixed boundary condition allows you to solve such a case. The only drawback of it is that when the solved domain mesh is refined, the valueFraction must be recalculated manually, unless you are skilled enough and rewrite the boundary condition code so it does it for you automatically.

nandiganavishal February 25, 2013 13:06

Quote:

Originally Posted by Lada (Post 409774)
Hi Vishal,

ad 1) the temperature appears in all changeDictionaryDict files and it is an initial guess of the temperature at the interface. You can put any number there or delete the whole line and not much will happen. Maybe a few extra iterations will be needed to converge the case.
ad 2) I calculated the valueFraction according to the following formula:
valueFraction= 1 / (1 + conductivity/delta/HTC)
conductivity (W/m/K) stands for the conductivity of the material layer (concrete_1 or concrete_2) which is defined in respective solidThermophysicalProperties file of the layers (regions)
delta (m) is the half thickness of the first cell layer adjacent to the boundary
HTC (W/m2/K) is the heat transfer coefficient at the wall
ad 3) 258 is the temperature of the fluid that is at the outer side of the boundary
ad 4) as I could not find better boundary type to define the Robin's boundary condition, I had to choose the mixed one. Imagine a wall that stands between you and outdoors. You don't want to solve the flow in the room or outdoors, but you know the temperatures indoors and outdoors as well as the heat transfer coefficients at both sides of the wall. The mixed boundary condition allows you to solve such a case. The only drawback of it is that when the solved domain mesh is refined, the valueFraction must be recalculated manually, unless you are skilled enough and rewrite the boundary condition code so it does it for you automatically.

Thanks Lada,

That clarifies my question !! I would like to know if it is possible to use this BC if there is a source of heat flux (q) at the interface of region 1 and region 2. Now the temperature at the wall (Tw) would be something like this

Tw=(k1/DeltaY1)/(k1/DeltaY1+k2/DeltaY2)*T1+(k2/DeltaY2)/(k1/DeltaY1+k2/DeltaY2)*T2 - q/(k1/DeltaY1+k2/DeltaY2)

where k1 - conductivity of region 1
k2 - conductivity of region 2
DeltaY1 - spatial discretization in region 1
DeltaY2 - spatial discretization in region 2
T1 - temperature near the surface of region 1
T2 - temperature near the surface of region 2

Please let me know.

Thanks
Regards
Vishal

Lada February 25, 2013 14:20

Hi Vishal,

I guess you need thermal baffle boundary condition for that. I am not familiar with that though so not much of a use. See http://www.openfoam.org/version2.0.0/thermophysical.php
and the respective tutorial.

nandiganavishal February 25, 2013 17:15

Quote:

Originally Posted by Lada (Post 410010)
Hi Vishal,

I guess you need thermal baffle boundary condition for that. I am not familiar with that though so not much of a use. See http://www.openfoam.org/version2.0.0/thermophysical.php
and the respective tutorial.

Thanks Lada for the tip !!

Ahmed Khattab February 26, 2013 02:53

Ypmma, Ychar
 
Quote:

Originally Posted by Lada (Post 329221)
Although it sounds convincing, I am now puzzled even more :) .

The thing is there is no chemistry or species present in those tutorials. They are just simple buoyant air flow around a solid (iron or so) material cases.

Based on what you wrote, it might be something that the author of all multiRegion tutorials forgot to remove because it is present only in time directories that relate to the solids (the changeDictionaryDict files that are used to modify boundary conditions for the particular model region (solid material), contain the Ychar and Ypmma as well).
It does not seem to be calculated as it appears in '0' directory only.

It is rather confusing.

Thank you for your response.

Hi vladimir,

i think that these are contribution ration of two species making the solid. the factor is modified from 0 in 0 folder to 0.5 for each in changeDictionaryDict file as every other variable. but i tried to change these factors to be 0.7and 0.5 so the summation of it will be greater than 1 which is wrong but the solver ran. another thing these Ychar, and Ypmma have characteristic (rho, cp, ...)that could be changed which recommend that it species of the solid. to solve this situation i suggest to set there properties as your material (make them have same properties) so you can make them as one material.

that what i think, i hope it will be useful. :)

Ahmed Khattab February 26, 2013 08:27

BC discription
 
Quote:

Originally Posted by nandiganavishal (Post 409694)
Hi Vladimir,

I would like to know if you were able to solve the multiregion Problem. I am trying to solve a heat conductive equation between 2 solids of different thermal conductivities k1 and k2. I am using the chtMultiRegionFoam to solve this problem. I would like to enforce the following heat flux boundary condition

k1 grad(T) (region 1) = k2 grad(T) (region 2).

Kindly let me know what predefined boundary condition in OpenFoam corresponds to this BC.

Thanks
Regards
Vishal

Hi Vishal,

please find below the description of BC compressible::turbulentTemperatureCoupledBaffleMix ed copied from .h file of this BC, i hope it will be helpful for you.

Code:

Description
    Mixed boundary condition for temperature, to be used for heat-transfer
    on back-to-back baffles.

    Specifies gradient and temperature such that the equations are the same
    on both sides:
    - refGradient = zero gradient
    - refValue = neighbour value
    - mixFraction = nbrKDelta / (nbrKDelta + myKDelta())

    where KDelta is heat-transfer coefficient K * deltaCoeffs

    Example usage:
        myInterfacePatchName
        {
            type        compressible::turbulentTemperatureCoupledBaffleMixed;
            neighbourFieldName  T;
            K                  lookup;
            KName              K;
            value              uniform 300;
        }

    Needs to be on underlying mapped(Wall)FvPatch.

    Note: K : heat conduction at patch. Gets supplied how to lookup/calculate K:
    - 'lookup' : lookup volScalarField (or volSymmTensorField) with name
    - 'basicThermo' : use basicThermo and compressible::RASmodel to calculate K
    - 'solidThermo' : use basicSolidThermo K()
    - 'directionalSolidThermo' directionalK()

    Note: runs in parallel with arbitrary decomposition. Uses mapped
    functionality to calculate exchange

Good Luck :)

Sasy September 25, 2013 01:14

Helping
 
Hi Foarmers
I want simulate evaporation in two phase.(gaz and liquid) with conjugate heat transfer.But i dont know i use two phase solver (such as interFoam or interPhasechangeFoam) and add solid Region or use chtMultiRegionFoam and modify for twophase??

klilla September 25, 2013 03:31

Now, you have to combine the 2 :). You need to change the fluid dictionary of the chtMultiRegionFoam solver with interFoam. I did something simular already. So if you have problem I might be able to help.

Let me have one question, however. I do not know phase change modelling, but I plan to do a simulation of water jet impingement on heated planar surface. Now, I planned to do it with compressible multiphase solver., since I suspact that water wapour is compressible. What do you think about this? Can you model evaporation with incompressible flow solver?

Sasy September 25, 2013 03:40

Quote:

Originally Posted by klilla (Post 453461)
Now, you have to combine the 2 :). You need to change the fluid dictionary of the chtMultiRegionFoam solver with interFoam. I did something simular already. So if you have problem I might be able to help.

Let me have one question, however. I do not know phase change modelling, but I plan to do a simulation of water jet impingement on heated planar surface. Now, I planned to do it with compressible multiphase solver., since I suspact that water wapour is compressible. What do you think about this? Can you model evaporation with incompressible flow solver?

Hi kapa
thank you For reply
yes,i use interPhasechange solver (that is for incompresible fluid) and modify this solver by adding Energy equation and source term.but i should implemented conjugate heat transfer for my case.and i dont have idae.in youre opinion can I implemented solid region for my solver or not,i should use chtMultiRegionFoam solver and modify this solver for two phase incompresible with phase change?

klilla September 25, 2013 03:51

If you go to the chtMultiRegionSimpleFoam solver source code, you can see a directory called (fluid). That is the directory, where you have to work in. At the release implementation it is derived from simpleFoam. First I suggest to compare simpleFoam and chtMultiRegionSimpleFoam/fluid files in order to understand the way of implementation. Than you can start to change it for your need.

Good luck,
Lilla

Sasy September 25, 2013 03:59

Quote:

Originally Posted by klilla (Post 453471)
If you go to the chtMultiRegionSimpleFoam solver source code, you can see a directory called (fluid). That is the directory, where you have to work in. At the release implementation it is derived from simpleFoam. First I suggest to compare simpleFoam and chtMultiRegionSimpleFoam/fluid files in order to understand the way of implementation. Than you can start to change it for your need.

Good luck,
Lilla

thank you for reply
But i have a question..
why chtMultiRegionSimpleFoam? what is differnce with chtMultiRegionFoam? az i said,my fluid is incompresible,but i think this solver for compressible Fluid,am I right?
Regards,

klilla September 25, 2013 04:11

Indeed, I have forgotten that. You need to compare it with rhoSimpleFoam than. It is a nice excersice.
Lilla


All times are GMT -4. The time now is 07:04.