Register Blogs Members List Search Today's Posts Mark Forums Read

 July 5, 2009, 12:05 bulk temperature about a Area #1 New Member   Valentin Mayer Join Date: Jul 2009 Posts: 5 Rep Power: 8 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

 July 6, 2009, 04:32 #2 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 275 Rep Power: 9 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

 July 6, 2009, 12:30 #3 New Member   Valentin Mayer Join Date: Jul 2009 Posts: 5 Rep Power: 8 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

July 6, 2009, 14:51
#4
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
Quote:
Originally Posted by splif
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 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:

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

 July 7, 2009, 08:34 #5 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 275 Rep Power: 9 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

 July 7, 2009, 10:23 #6 New Member   Valentin Mayer Join Date: Jul 2009 Posts: 5 Rep Power: 8 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

 July 7, 2009, 11:22 #7 Senior Member   Henrik Rusche Join Date: Mar 2009 Location: Braunschweig, Niedersachsen, Germany Posts: 275 Rep Power: 9 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

 July 7, 2009, 12:19 #8 New Member   Valentin Mayer Join Date: Jul 2009 Posts: 5 Rep Power: 8 Hello Hendrik, thanks a lot.Have a nice evening (in German). Bye Valentin

 August 11, 2011, 17:26 #9 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,147 Blog Entries: 1 Rep Power: 15 hi could you calculate bulk temperature along pipe axis ? i search for it too

 August 13, 2011, 15:46 bulk Temperature + cell selection #10 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,147 Blog Entries: 1 Rep Power: 15 Code: ``` label patchii = mesh.boundaryMesh().findPatchID("fixedWall"); const Foam::fvsPatchField > 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) .... )

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post vemps FLUENT 0 May 1, 2009 01:09 cadcamvijay Main CFD Forum 2 March 21, 2009 01:36 mike CFX 1 March 19, 2008 08:22 Italy CFX 4 July 12, 2007 00:05 Yogesh FLUENT 0 February 18, 2005 16:37

All times are GMT -4. The time now is 10:40.