|
[Sponsors] |
September 13, 2011, 12:30 |
|
#21 |
Member
andres
Join Date: Jul 2011
Posts: 31
Rep Power: 15 |
readSIMPLEcontrols.H doesn´t exist !
|
|
September 13, 2011, 12:41 |
|
#22 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
Ah, of course not! You are trying to compile a solver made for OpenFoam 1.6! In version 2.0, readSIMPLEcontrols.H has been replaced by simpleControl.H. Try replacing the include in my_simpleFoam.C. I can't guarantee you it will work, but it's worth a try. If it doesn't work, take simpleFoam from version 2.0 and add the modifications from this thread to it.
|
|
September 13, 2011, 13:47 |
|
#23 | |
Member
andres
Join Date: Jul 2011
Posts: 31
Rep Power: 15 |
I have change the line, re-compile but a new error appear.
I will try to rewrite the new "solver" from 0, because this is for an older version of foam. thanks for all! Quote:
|
||
September 13, 2011, 14:49 |
|
#24 | ||
Member
andres
Join Date: Jul 2011
Posts: 31
Rep Power: 15 |
I have copied the simpleFoam from /opt/openfoam200/applications/solvers/incompressible, to /home/usuarioubuntu/myfoam directory, then I rename the simpleFoam.C to mysimpleFoam.C, also I have changed the "files" in the Make subdirectory.
Quote:
Quote:
|
|||
September 14, 2011, 02:51 |
|
#25 |
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 22 |
Try to replace FOAM_APPBIN in Make/files with FOAM_USER_APPBIN
The error message says that you don't have write permission in the default appbin. |
|
September 14, 2011, 14:19 |
|
#26 |
Member
andres
Join Date: Jul 2011
Posts: 31
Rep Power: 15 |
amazing!! I was able to compile and run a test case of the icofoam+temperature solver.
Thanks Anton!!! |
|
September 22, 2011, 06:37 |
|
#27 | |
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 15 |
Quote:
--> FOAM FATAL IO ERROR: keyword div((nuEff*dev(T(grad(U))))) is undefined in dictionary "/home/.../incompressible/my_simpleFoam/case/system/fvSchemes::divSchemes" file: /home/.../incompressible/my_simpleFoam/case/system/fvSchemes::divSchemes from line 32 to line 40. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 400. FOAM exiting Any suggestions? |
||
September 22, 2011, 10:39 |
|
#28 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi Rob,
as the error message says you must add an entry for div((nuEff*dev(T(grad(U))))) in the fvSchemes file. Attached is a fvSchemes file for OpenFOAM 2.0.x. Good luck Martin |
|
September 22, 2011, 12:31 |
|
#29 |
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 15 |
Wow, that was quite simple. Sometimes you won't see the wood for trees.
The case is running now. Thank you very much. I have yet another question. Is it possible to add two internalField scalars for the temperature? I have 2 pipes connected to each other which swap heat directly. I need that kind of option, a nonuniform list of scalars did not work out. |
|
September 23, 2011, 04:28 |
Still won't work.
|
#30 |
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 15 |
Yeah, actually the solver was working ( I did not get an error message ).
But unfortunately the temperature was not solved with the p and U equation. It was not even read. When I performed the 'wmake' command in the console, I got this error message: Code:
SOURCE=my_simpleFoam.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam201/src/turbulenceModels -I/opt/openfoam201/src/turbulenceModels/incompressible/RAS/RASModel -I/opt/openfoam201/src/transportModels -I/opt/openfoam201/src/transportModels/incompressible/singlePhaseTransportModel -I/opt/openfoam201/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam201/src/OpenFOAM/lnInclude -I/opt/openfoam201/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linuxGccDPOpt/my_simpleFoam.o In file included from /opt/openfoam201/src/finiteVolume/lnInclude/simpleControl.H:36:0, from my_simpleFoam.C:54: /opt/openfoam201/src/finiteVolume/lnInclude/solutionControl.H: In function ‘int main(int, char**)’: /opt/openfoam201/src/finiteVolume/lnInclude/solutionControl.H:39:1: error: ‘namespace’ definition is not allowed here In file included from /opt/openfoam201/src/finiteVolume/lnInclude/solutionControl.H:149:0, from /opt/openfoam201/src/finiteVolume/lnInclude/simpleControl.H:36, from my_simpleFoam.C:54: /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:28:38: error: ‘Foam::solutionControl’ has not been declared /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:29:1: error: a function-definition is not allowed here before ‘{’ token /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:34:26: error: ‘Foam::solutionControl’ has not been declared /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:35:1: error: a function-definition is not allowed here before ‘{’ token /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:40:19: error: ‘Foam::solutionControl’ has not been declared /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:41:1: error: a function-definition is not allowed here before ‘{’ token /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:46:19: error: ‘Foam::solutionControl’ has not been declared /opt/openfoam201/src/finiteVolume/lnInclude/solutionControlI.H:47:1: error: a function-definition is not allowed here before ‘{’ token In file included from my_simpleFoam.C:54:0: /opt/openfoam201/src/finiteVolume/lnInclude/simpleControl.H:40:1: error: ‘namespace’ definition is not allowed here In file included from /opt/openfoam201/src/finiteVolume/lnInclude/simpleControl.H:109:0, from my_simpleFoam.C:54: /opt/openfoam201/src/finiteVolume/lnInclude/simpleControlI.H:30:19: error: ‘Foam::simpleControl’ has not been declared /opt/openfoam201/src/finiteVolume/lnInclude/simpleControlI.H:31:1: error: a function-definition is not allowed here before ‘{’ token my_simpleFoam.C:80:1: error: expected ‘}’ at end of input /opt/openfoam201/src/finiteVolume/lnInclude/initContinuityErrs.H:37:8: warning: unused variable ‘cumulativeContErr’ my_simpleFoam.C:80:1: error: expected ‘}’ at end of input make: *** [Make/linuxGccDPOpt/my_simpleFoam.o] Fehler 1 I tried to figure it out myself with no outcome. |
|
September 23, 2011, 05:52 |
|
#31 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi Rob,
here is the solver and a case for OpenFOAM 2.0.x. Please be aware, that the name of the solver is mySimpleFoam. Martin |
|
September 30, 2011, 06:34 |
|
#32 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Thank you Martin for sharing!
|
|
October 3, 2011, 09:21 |
|
#33 |
Member
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 17 |
Hi,
I have recently pegged away at simpleScalarFoam as well and came up with this: Code:
// --- Scalar Transport T.storePrevIter(); for (int nonOrth=0; nonOrth<=simple.nNonOrthCorr(); nonOrth++) { volScalarField DTEff = DT+turbulence->nut()/0.7; fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::laplacian(DTEff, T) ); TEqn.relax(); TEqn.solve(); } I use these schemes for the scalar transport: Code:
grad(T) Gauss linear; div(phi,T) Gauss Gamma 1.0; laplacian((DT+(nut|0.7)),T) Gauss linear limited 1.0; This is quite a basic implementation, so it would be nice to add some cool feature like residence time calculation, source terms, ... If I have any progress on this, I will post it as well. |
|
October 27, 2011, 12:16 |
Viscous Dissipation
|
#34 |
Member
Nickolas P
Join Date: Oct 2010
Location: Greece
Posts: 30
Rep Power: 16 |
Hello everybody,
I m studying polymer rheology under different types of geometry. To do that I work in simpleFoam switching off the turbulent part as the flow is creeping laminar with Re<<1. In the past I sucessfully added the temperature equation on simpleFoam by the help of Martin. However, this equation lacks of the viscous dissipation part that contributes for the frictional loss which at the moment I need to study. In the created file TEqn.H I declared the heat equation as below but I dont know how to insert the viscosity (I use a Newtonian fluid so this is actually the laminar viscosity). The file is: fvScalarMatrix TEqn ( fvm::div(phi, T) - fvm::laplacian(alpha, T) == (1/rho*Cp)*(2*(VISCOSITY??)*symm(fvc::grad(U)) && fvc::grad(U)) ); TEqn.relax(); eqnResidual = TEqn.solve().initialResidual(); maxResidual = max(eqnResidual, maxResidual); Hoping that I ve written the equation correctly....can anybody help me out on how to insert the viscosity??I have tried to insert it as: nu(), nuEff() but it didnt work out (in each case it was reported that....'nu'or 'nuEff' is not declared in this scope). Thanks in advance! Nickolas |
|
October 28, 2011, 20:22 |
|
#35 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi Nickolas,
you can try the attached solver (for OpenFOAM 2.0.x) and case. Comments are added to the code and the case. Increase of temperature is calculated via controlDict (4.585 K) and nearly matches to the appropriate formula for high viscous newtonian fluids (4.73 K). Ah, and you can access the viscosity for your formula with "laminarTransport.nu()". Martin |
|
January 1, 2012, 10:34 |
|
#36 |
Senior Member
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 200
Rep Power: 15 |
hey,
thanks for sharing the solver .. it works really fine, the only problem I'm having is I'm not getting any T on the paraView .. when i try to view it but I'm getting the results in the folder, any suggestions... to what i could do to get the T in the paraView along with P and U which I'm getting regards, hasan. |
|
January 1, 2012, 10:35 |
|
#37 |
Senior Member
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 200
Rep Power: 15 |
hey,
thanks for sharing the solver .. it works really fine, the only problem I'm having is I'm not getting any T on the paraView .. when i try to view it but I'm getting the results in the folder, any suggestions... to what i could do to get the T in the paraView along with P and U which I'm getting regards, hasan. |
|
January 1, 2012, 11:04 |
|
#38 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi Hasan,
have you selected T in the "Volume Fields" list of the Object Inspector? See attached image... Martin |
|
January 1, 2012, 11:06 |
|
#39 |
Senior Member
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 200
Rep Power: 15 |
Thank you .. I'm so sorry i found... it. another doubt abt boundry conditions, can i post it here..? coz there is no reply from the foundry condition forums..?
|
|
January 25, 2012, 09:39 |
|
#40 |
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 17 |
Hi All,
I started to use the solver buoyanSimpleFoam to simulate incompressible liquid water (or "incompressible" vapour water) with temperature field. For this I used the basicRhoThermo type in buoyanSimpleFoam where is possible to choose the incompressible thermo type. But I found some problems I posted here: http://www.cfd-online.com/Forums/ope...implefoam.html My model has also a porous medium. Surfing on the forum I found this post where TEqn is added for simpleFoam solver. I downloaded the last Martin's solvers (thanks to share it!). Hi have two question: 1) Is it correct to use this solver for my case (liquid water or vapour water), or is it better switch off the viscous dissipation? 2) I'd like to add a thermal prop. for the porous zones. I known in OF2.0.x there is a fixedTemperature thermo prop. that add a term in the hEqn. How can "fix" this for TEqn? Thanks for any help Andrea
__________________
Andrea Pasquali |
|
Tags |
simplefoam, temperature |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Calculation of the Governing Equations | Mihail | CFX | 7 | September 7, 2014 07:27 |
Adding a new temperature dependent viscositymodel? | dgadensg | OpenFOAM Programming & Development | 10 | May 22, 2010 06:47 |
Adding temperature equation in settlingFoam | sachin | OpenFOAM Running, Solving & CFD | 2 | March 31, 2010 04:21 |
Adding temperature field to InterFoam | yapalparvi | OpenFOAM Running, Solving & CFD | 8 | October 14, 2009 21:18 |
Adding coriolis forces in simplefoam | Xabi | OpenFOAM Running, Solving & CFD | 1 | April 24, 2009 05:43 |