CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   bulk temperature about a Area (http://www.cfd-online.com/Forums/openfoam-programming-development/66084-bulk-temperature-about-area.html)

splif July 5, 2009 12:05

bulk temperature about a Area
 
Hello

I new in OpenFoam user and I try to get the bulk temperautre about a area.

the theory: my problem

tbulk = integration(U*T*dA) / integration(U*dA)

the nummerical:

I'm not really sure how to sovle this problem.
Postprocessing or ?
I think that you need a summation about the area,like:
sum = sum + T(n)*U(n)*dy (Fortran 2D)
How can i fixed this problem?
Have somebody a idea?

Thanks
valentin

henrik July 6, 2009 04:32

Dear Valentin,

There are two issues. How to define the area and how to parallelise.

I would also advise you to use the flux rather than the velocity since it is guaranteed to be conservative.

Neglecting parallelisation issues and assuming that you want to work with patch (iP) the following will the job:

Code:

heatFlux =
    sum(T.boundaryField()[iP]*phi.boundaryField()[iP])/sum(phi.boundaryField()[iP]);

Henrik

splif July 6, 2009 12:30

Hi Henrik,

sorry for this Question. But i'm not in used to work with openFoam.
what means [ip] ? It is for direction, like [x].

I'm not sure if i get you wrong:
Your equation mean:

q=sum(t*flux)/sum(flux)=sum(t*rho*U)/sum((rho*U)) ?
Is there no multiply wirh dy and dx?

Thanks
Valentin

gschaider July 6, 2009 14:51

Quote:

Originally Posted by splif (Post 221633)
sorry for this Question. But i'm not in used to work with openFoam.
what means [ip] ? It is for direction, like [x].
Quote:

Originally Posted by splif (Post 221633)

No. It is the index of the patch. For an example on how to get the index if you got the name of the patch have a look at the sources of $FOAM_UTILITIES/postProcessing/patch/patchIntegrate

I'm not sure if i get you wrong:
Your equation mean:

q=sum(t*flux)/sum(flux)=sum(t*rho*U)/sum((rho*U)) ?
Is there no multiply wirh dy and dx?

No. The is all included in phi (that is the flux Henrik was talking about). For the definition of phi look elsewhere (it's been discussed zillions of times)

Bernhard

henrik July 7, 2009 08:34

Dear Valentin,

thanks for your private message (in German). I hope you don't mind if I repeat what I understand is what you are trying to do.

Valentin is seeking to evaluate the local Nusselt number and needs the bulk temperature to do so. The local Nusselt number would be per wall face (additional averaging may apply) and the bulk temperature is a function of the axial position in the pipe (x-coordinate in his case).

The problem is now to evaluate the bulk temperature for a given axial position.

Is this correct?

Henrik

splif July 7, 2009 10:23

Hello Hendriks,

that's right. I search for a summation (lilke (sum(sum( T.yz*U.yz*dy)dz)each Cells) about an area (yz).And every summation should go every cells in x-> direction.
Perhaps somebody has an idea.

Thanks
Valentin

henrik July 7, 2009 11:22

Dear Valentin,

Okay. I would try the following. Create a lookup table for T_bulk as a function of x. To do so, you need a function that maps x into an index.

Code:

scalarField vol(nCellsx, 0.0);
scalarField Tbulk(nCellsx, 0.0);
forAll(T, cellI)
{
    if ( inBulkRegion(mesh.C()[cellI]) )
    {
        label index = floor(mesh.C()[cellI].x()/length*nCellsx);
        vol[index] += mesh.V()[cellI];
        Tbulkl[index] += T[cellI]*mesh.V()[cellI];
    }
}

Tbulk /= vol;

Then walk over the wall patch to calculate the local Nusselt number and use the same index function to look up Tbulk (but calculated with the face center's x-coordinate).

This is by no means elegant, it will not parallelise easily and there are better ways of doing this. However, this will get you a long way.

Henrik

splif July 7, 2009 12:19

Hello Hendrik,

thanks a lot.Have a nice evening (in German).

Bye
Valentin

nimasam August 11, 2011 17:26

hi
could you calculate bulk temperature along pipe axis ? i search for it too

nimasam August 13, 2011 15:46

bulk Temperature + cell selection
 
Code:

    label patchii = mesh.boundaryMesh().findPatchID("fixedWall");
    const Foam::fvsPatchField<Foam::Vector<double> > Cpatches = mesh.Cf().boundaryField()[patchii];

    scalar nCellsx = Cpatches.size();
    labelListList inBulkRegionList (nCellsx);
   
    forAll(Cpatches, cellj)
    {
      label nSelectedCell = 1;
      forAll(mesh.C(), celli)
      {
        if ( (Cpatches[cellj]).z() == (mesh.C()[celli]).z())
          {
      inBulkRegionList[cellj].setSize(nSelectedCell,celli);
      nSelectedCell ++;
          }
      }
    }


hi dear foamer
i have a pipe! its axismyetric and it is 40*160! i want to have the cells in each cross section means the cells with the same highth!
so i should have a list, this list has 160 sublist, each sublist contains the cell IDs of in each highth! so it should be 40!
i wrote above code to make a list of list!!! it compiles well but the result is some how strange and it dose not return all cell selections in each height i expected it returns 40 cells in each height but you can see the results.can anybody tell me why?

labelListList:
160
(

19 // it should be 40 cells!
(
2
6
7
9
10
11
13
14
16
18
19
20
21
23
24
27
33
35
37
)


18
(
43
47
50
51
52
53
57
58
59
63
64
66
68
69
70
73
74
79
)

5(84 85 87 117 119)

11
(
123
125
129
130
136
139
140
141
143
149
152
)


20
(
160
161
166
167
169
170
172
173
176
177
178
180
181
182
185
190
195
196
197
199
)


13
(
200
201
205
209
210
217
221
222
224
229
232
235
238
)

8(244 246 247 262 265 266 275 278)
....
)

Bana December 4, 2015 14:51

Bulk temperature
 
Hi nima sam and Bruno
I need the answer to this question, my case is an axisymetric heated pipe too, I need to calculate bulk temperature at each cross section ,tbulk = integration(U*T*dA) / integration(U*dA) to compute nusselt number.additionally it is needed for fully developed condition of T at the outlet of pipe!!
any help or hint would be appreciated!
Thanks in advance

nimasam December 7, 2015 03:59

you should write some pieces of code to gather cells in each section and then return the value of them for calculation, above structure give you hints how to go forward.

Bana December 7, 2015 14:18

Dear Nima Sam
Thanks for your reply, your code was very inspiring for me but why it didn't get anticipated 2d array?
maybe "size()" member function returns the number of neighbour cells for a cell but in this case we need to access patches which are normal to each wall patch.Is it the problem or anything else?
bests,
MohammadReza

milad653279 July 30, 2016 16:59

Quote:

Originally Posted by nimasam (Post 320003)
Code:

    label patchii = mesh.boundaryMesh().findPatchID("fixedWall");
    const Foam::fvsPatchField<Foam::Vector<double> > Cpatches = mesh.Cf().boundaryField()[patchii];

    scalar nCellsx = Cpatches.size();
    labelListList inBulkRegionList (nCellsx);
   
    forAll(Cpatches, cellj)
    {
      label nSelectedCell = 1;
      forAll(mesh.C(), celli)
      {
        if ( (Cpatches[cellj]).z() == (mesh.C()[celli]).z())
          {
      inBulkRegionList[cellj].setSize(nSelectedCell,celli);
      nSelectedCell ++;
          }
      }
    }

hi dear foamer
i have a pipe! its axismyetric and it is 40*160! i want to have the cells in each cross section means the cells with the same highth!
so i should have a list, this list has 160 sublist, each sublist contains the cell IDs of in each highth! so it should be 40!
i wrote above code to make a list of list!!! it compiles well but the result is some how strange and it dose not return all cell selections in each height i expected it returns 40 cells in each height but you can see the results.can anybody tell me why?

labelListList:
160
(

19 // it should be 40 cells!
(
2
6
7
9
10
11
13
14
16
18
19
20
21
23
24
27
33
35
37
)


18
(
43
47
50
51
52
53
57
58
59
63
64
66
68
69
70
73
74
79
)

5(84 85 87 117 119)

11
(
123
125
129
130
136
139
140
141
143
149
152
)


20
(
160
161
166
167
169
170
172
173
176
177
178
180
181
182
185
190
195
196
197
199
)


13
(
200
201
205
209
210
217
221
222
224
229
232
235
238
)

8(244 246 247 262 265 266 275 278)
....
)

Dear foamer
the above code have been written by nimasam is very good but must be corrected till it works well. for reformation, if clause must be written as following:

Quote:

if ( float Cpatches[cellj].z() == float mesh.C()[celli].z() )
as you see, the float type must be added.

Best regards,
Milad

gurjeetpunia October 14, 2016 06:42

Hello all,
I am working on heat transfer analysis in rectangular duct using ANSYS-Fluent. for calculation of local nusselt number I need bulk fluid temperature. where,

Tbulk = integration(U*T*dA) / integration(U*dA)

I am able to get Tbulk. please help me to find that.

gschaider October 14, 2016 11:31

Quote:

Originally Posted by gurjeetpunia (Post 621509)
Hello all,
I am working on heat transfer analysis in rectangular duct using ANSYS-Fluent. for calculation of local nusselt number I need bulk fluid temperature. where,

Tbulk = integration(U*T*dA) / integration(U*dA)

I am able to get Tbulk. please help me to find that.

Phone your Fluent-support about it. The phone number should be on the contract you paid a lot of money for.

That is one of the reasons why one pays money for Fluent: you don't have to face sarcastic answers on the MessageBoard. Paid support people are polite

gurjeetpunia October 14, 2016 14:20

Dear Bernhard,
Thanks for your response. BUT need help to calculate integration of UTdA in Fluent. means how to calculate integral of product of more than one variable along the length.

gschaider October 17, 2016 11:32

Quote:

Originally Posted by gurjeetpunia (Post 621555)
Dear Bernhard,
Thanks for your response. BUT need help to calculate integration of UTdA in Fluent. means how to calculate integral of product of more than one variable along the length.

You're in an OpenFOAM-forum. People here usually don't know Fluent. And if they do they won't admit it. Ask in the Fluent-Forum

Mirage November 3, 2016 13:50

Quote:

Originally Posted by nimasam (Post 320003)
Code:

    label patchii = mesh.boundaryMesh().findPatchID("fixedWall");
    const Foam::fvsPatchField<Foam::Vector<double> > Cpatches = mesh.Cf().boundaryField()[patchii];

    scalar nCellsx = Cpatches.size();
    labelListList inBulkRegionList (nCellsx);
   
    forAll(Cpatches, cellj)
    {
      label nSelectedCell = 1;
      forAll(mesh.C(), celli)
      {
        if ( (Cpatches[cellj]).z() == (mesh.C()[celli]).z())
          {
      inBulkRegionList[cellj].setSize(nSelectedCell,celli);
      nSelectedCell ++;
          }
      }
    }

hi dear foamer
i have a pipe! its axismyetric and it is 40*160! i want to have the cells in each cross section means the cells with the same highth!
so i should have a list, this list has 160 sublist, each sublist contains the cell IDs of in each highth! so it should be 40!
i wrote above code to make a list of list!!! it compiles well but the result is some how strange and it dose not return all cell selections in each height i expected it returns 40 cells in each height but you can see the results.can anybody tell me why?

labelListList:
160
(

19 // it should be 40 cells!
(
2
6
7
9
10
11
13
14
16
18
19
20
21
23
24
27
33
35
37
)


18
(
43
47
50
51
52
53
57
58
59
63
64
66
68
69
70
73
74
79
)

5(84 85 87 117 119)

11
(
123
125
129
130
136
139
140
141
143
149
152
)


20
(
160
161
166
167
169
170
172
173
176
177
178
180
181
182
185
190
195
196
197
199
)


13
(
200
201
205
209
210
217
221
222
224
229
232
235
238
)

8(244 246 247 262 265 266 275 278)
....
)

Hi Guys :)

I would like to use the code to compute my Tbulk. But It is for me not clear, how does this code compute Tbulk and Where should I write the code?

Thanks for your help :)


All times are GMT -4. The time now is 14:21.