# Error turbFoam

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

 June 21, 2007, 06:22 Hi, i have modified the turbf #1 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Hi, i have modified the turbfoam solver in a way that i can calculate forces in selected patches. the problem is that the solver aborts and gives the following message: Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model kEpsilon Reading the patch force dictionary Reading force solver data Starting time loop Time = 0.01 Courant Number mean: 0 max: 0 DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 2.34397e-13, No Iterations 1 AMG: Solving for p, Initial residual = 1, Final residual = 0.0483882, No Iterations 1 time step continuity errors : sum local = 0.000553499, global = -8.75052e-07, cumulative = -8.75052e-07 AMG: Solving for p, Initial residual = 0.314146, Final residual = 0.0218164, No Iterations 1 time step continuity errors : sum local = 0.000303637, global = 4.96421e-05, cumulative = 4.8767e-05 Calculating Pressure Forces.... Area of patch cock = 820.124 Pressure force on patch cock = -1.02047e+08 N Total Pressure Force in cock moving direction = -1.02047e+08 N Calculating Wall Shear Forces.... Shear Force on patch cock = 0 N Total Shear Force in cock moving direction = 0N Total Force in cock moving direction = -1.02047e+08N #0 Foam::error::printStack(Foam:stream&) #1 Foam::sigFpe::sigFpeHandler(int) #2 Uninterpreted: [0xffffe420] #3 Foam::divide(Foam::Field&, Foam::UList const&, Foam::UList const&) #4 void Foam::divide(Foam::GeometricF ield&, Foam::GeometricField const&, Foam::GeometricField const&) #5 Foam::tmp > Foam::operator/(Foam::tmp > const&, Foam::GeometricField const&) #6 Foam::turbulenceModels::kEpsilon::correct() #7 main #8 __libc_start_main #9 Foam::regIOobject::readIfModified() Can someone tell me what i have done wrong, because the problem is the same when i use the normal tubfoam solver, too. Daniel

 June 21, 2007, 07:24 When i turn off turbulence or #2 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 When i turn off turbulence or choose the laminar turbulence model the problem is gone. What do i have to do, to get the turbulence run? Daniel

 June 21, 2007, 07:35 Check you initial and boundary #3 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,907 Rep Power: 27 Check you initial and boundary conditions for k and epsilon. Regards, Alberto __________________ Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

 June 21, 2007, 07:42 Thanks for you answer! He #4 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Thanks for you answer! Here are my conditions: object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { dummyPatch3 { type zeroGradient; } dummyPatch4 { type zeroGradient; } dummyPatch5 { type zeroGradient; } in { type fixedValue; value uniform 0.00375; } out { type zeroGradient; } cock { type zeroGradient; object epsilon; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -3 0 0 0 0]; internalField uniform 0; boundaryField { dummyPatch3 { type zeroGradient; } dummyPatch4 { type zeroGradient; } dummyPatch5 { type zeroGradient; } in { type fixedValue; value uniform 0.00377; } out { type zeroGradient; } cock { type zeroGradient; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ( dummyPatch3 { type wall; physicalType wallFunctions; startFace 445651; nFaces 3898; } dummyPatch4 { type wall; physicalType wallFunctions; startFace 449549; nFaces 768; } dummyPatch5 { type wall; physicalType wallFunctions; startFace 450317; nFaces 9312; } in { type patch; physicalType pressureInlet; startFace 459629; nFaces 1154; } out { type patch; physicalType pressureOutlet; startFace 460783; nFaces 414; } cock { type wall; physicalType wallFunctions; startFace 461197; nFaces 508; I can't see anything wrong with them... Daniel

 June 21, 2007, 07:59 The initialization of the inte #5 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,907 Rep Power: 27 The initialization of the internal fields is wrong. With internalField uniform 0; you're setting the initial values of k and eps to zero in you whole domain. Regards, Alberto __________________ Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

 June 21, 2007, 08:05 Thanks a lot Alberto, I've #6 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Thanks a lot Alberto, I've choosen the same values like for the inlet now and it works, how can i calculate that values for the internal field for different complex parts? Daniel

 June 21, 2007, 08:21 If you haven't detailed inform #7 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,907 Rep Power: 27 If you haven't detailed information, just use an average value of what you expect k and epsilon to be or the inlet value, as you're doing. Assuming you simulate for a time long enough, the final result is not influenced by the choice of your initial condition. With kind regards, A. __________________ Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

 June 21, 2007, 08:25 Thanks for your fast reply. No #8 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Thanks for your fast reply. Now it is working and i can go on with my tests, Regards, Daniel

 June 25, 2007, 16:57 Hello Daniel, A Good day to #9 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 531 Rep Power: 17 Hello Daniel, A Good day to you! I just happened to be looking through these messages, when I realised that you seem to be using a version of the solver "turbForceFoam", which incorporates rigid body motion (as of now in 1-D). It would be great if you could give me feedback regarding this modified solver.... have you made any interesting additions to the solver? Since I am currently making changes to it, it would be nice if you could let me know if there are any specific problems, or improvements which you have come up with while using it. Awaiting a reply! Enjoy! Philippose

 June 26, 2007, 05:11 Hi Philippose, yes i am using #10 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Hi Philippose, yes i am using the turbforcefoam solver. I have modified it because i don't need the body motion. I am only interested in the forces calculated by the solver. I am simulating hydraulic manifold valves for a automatic gear box and want to have the forces in the direction of the cock motion. Now a little question: How long has the case to be run to get god values for k and epsilon? I am trying with 100 steps from time 0 to 1e-5 with deltaT = 1e.7. Regards, Daniel

 June 27, 2007, 05:35 Another question: the force #11 New Member   Join Date: Mar 2009 Posts: 20 Rep Power: 9 Another question: the forces are only written as single values in a file, how can i write them as a field like p or u, so that i can view them in paraView? Daniel

 June 27, 2007, 14:22 Hello Daniel, A Good day to #12 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 531 Rep Power: 17 Hello Daniel, A Good day to you! Its interesting that you are from Baden Wuerttemberg :-)! I guess your town cant be too far from where I am :-)! Anyway.... as for your questions: a. Regarding convergence of k and epsilon.... this is dependent on many factors.... for example.... how accurate a solution are you expecting.... how complex the geometry is.... what kind of meshes you are using.... the boundary conditions, etc...etc.... :-)! I run cases between around 300,000 to around 1.5 Million pure tetrahedral cells, and I have found that "k" is the slowest of all the variables to converge. Epsilon and the velocity variables are more or less the same, and pressure converges the fastest. My simulations are normally run till an initial residual of around 1e-06, and this normally takes upto around 0.001 seconds, with a variable deltaT which hovers around 4e-07. b. Since turbForceFoam was written to incorporate the capability of rigid body motion into the fluid solver, I do not calculate the force as a field. Rather, I take a sum of the pressure at each boundary cell, multiplied by the area of the face of that cell which is on the boundary. This results in a single vector, which is the total force on a given patch. In order to save the force as a field, you will have to create a vector field similar to the velocity ("U") field, and instead of calculating the sum, you need to calculate the force on each patch cell face. I have not tried this yet, so I cannot give you the exact code to write... but I dont foresee it as being too difficult. Have a nice day! Philippose

 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 sivakumar OpenFOAM Pre-Processing 7 August 28, 2008 04:45 danie OpenFOAM Running, Solving & CFD 2 July 30, 2008 07:45 hsieh OpenFOAM Running, Solving & CFD 12 July 23, 2008 07:40 sippycup OpenFOAM Running, Solving & CFD 14 May 18, 2008 23:45 giampippetto OpenFOAM Running, Solving & CFD 0 March 9, 2006 03:21

All times are GMT -4. The time now is 00:53.