|
[Sponsors] |
July 15, 2014, 08:37 |
The IHFOAM Thread
|
#1 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Dear colleagues,
Now that IHFOAM has been released I open this thread to gather questions, comments, bug reports and mainly anything you can think about regarding IHFOAM. You can find a general wiki page, which will be growing day by day here: http://openfoamwiki.net/index.php/Contrib/IHFOAM The release thread can be found here: http://www.cfd-online.com/Forums/ope...m-release.html I look forward to having some feedback from you. Best, Pablo Last edited by Phicau; July 16, 2014 at 02:04. |
|
July 23, 2014, 13:02 |
Compilation problem on OpenFOAM 2.2.x
|
#2 |
Member
Join Date: Dec 2009
Posts: 49
Rep Power: 16 |
Hi Pablo,
This is really exciting. A new wave generation package for OpenFOAM. Thank you for your hard work and making the code open-source. I have compiled IHFOAM for OpenFOAM 2.2.1 on my personal computer and it works without a problem (successfully ran the example provided). However, I have problem compiling IHFOAM for OpenFOAM 2.2.x (i'm using this version on my university cluster). IHFOAM throw the following error. Code:
wmakeLnInclude: linking include files to ./lnInclude Making dependency list for source file IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C Making dependency list for source file IH_Waves_InletVelocity/IH_Waves_InletVelocityFvPatchVectorField.C SOURCE=IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -DOFVERSION=22x -I/home/ehk112/OpenFOAM/OpenFOAM-2.2.x/src/finiteVolume/lnInclude -I./IH_Waves_InletVelocity/velProfiles -I../common -I../common/checks -I../common/calculateWaterLevel -IlnInclude -I. -I/home/ehk112/OpenFOAM/OpenFOAM-2.2.x/src/OpenFOAM/lnInclude -I/home/ehk112/OpenFOAM/OpenFOAM-2.2.x/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/IH_Waves_InletAlphaFvPatchScalarField.o In file included from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.H:277:0, from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:47: ../common/memberFun.H:4:17: error: invalid suffix "x" on integer constant ../common/memberFun.H:15:17: error: invalid suffix "x" on integer constant In file included from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.H:277:0, from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:47: ../common/memberFun.H: In member function ‘Foam::scalar Foam::IH_Waves_InletAlphaFvPatchScalarField::PI()’: ../common/memberFun.H:7:35: error: ‘mathematicalConstant’ has not been declared IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C: In member function ‘virtual void Foam::IH_Waves_InletAlphaFvPatchScalarField::updateCoeffs()’: IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:316:12: warning: unused variable ‘auxiliarSolit’ [-Wunused-variable] IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:319:12: warning: unused variable ‘Csolitary’ [-Wunused-variable] IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:320:12: warning: unused variable ‘ts’ [-Wunused-variable] IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:321:12: warning: unused variable ‘Xa’ [-Wunused-variable] IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:361:18: warning: unused variable ‘g’ [-Wunused-variable] In file included from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.H:277:0, from IH_Waves_InletAlpha/IH_Waves_InletAlphaFvPatchScalarField.C:47: ../common/memberFun.H: In member function ‘Foam::scalar Foam::IH_Waves_InletAlphaFvPatchScalarField::PI()’: ../common/memberFun.H:10:9: warning: control reaches end of non-void function [-Wreturn-type] make: *** [Make/linux64GccDPOpt/IH_Waves_InletAlphaFvPatchScalarField.o] Error 1 \n\nWave generation boundary conditions compilation failed Kind regards, katakgoreng |
|
July 23, 2014, 15:32 |
|
#3 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi katakgoreng,
thanks for your words. I see the problem, DOFVERSION gets exported in the wrong way: Code:
-DOFVERSION=22x Thanks for reporting this, I will update the allMake scripts soon to avoid problems (especially with 2.3.x). In the mean time I suggest that you change these two lines: Code:
ofversion=`echo $WM_PROJECT_VERSION | sed -e 's/\./\n/g' -e 's/-/\n/' | grep "[0-9]" | tr -d '\n'` export OF_VERSION=$ofversion Code:
export OF_VERSION=220 Code:
ofversion=`echo $WM_PROJECT_VERSION | sed -e 's/\./\n/g' -e 's/-/\n/' | sed -e 's/x/9/g' | grep "[0-9]" | tr -d '\n'` Best, Pablo EDIT: I am not able to reproduce the error, in my installation of 2.2.x DOFVERSION=22, no x is found. However, I will push the change today Last edited by Phicau; July 24, 2014 at 03:07. Reason: Minor correction |
|
July 25, 2014, 09:58 |
|
#4 |
Member
Join Date: Dec 2009
Posts: 49
Rep Power: 16 |
Hi Pablo,
I managed to compile the library after following your suggestion. I applied the following in the allMake script. Code:
ofversion=`echo $WM_PROJECT_VERSION | sed -e 's/\./\n/g' -e 's/-/\n/' | sed -e 's/x/9/g' | grep "[0-9]" | tr -d '\n'` Kind regards, katakgoreng |
|
July 29, 2014, 11:31 |
baseWaveFlume error
|
#5 |
New Member
Dmitrijs Gavrilovs-Stepanovs
Join Date: Jun 2014
Posts: 15
Rep Power: 12 |
Hi Pablo,
Thank you very much for a new toolbox for waves, it looks amazing. I was just trying to check out a tutorial case named baseWaveFlume by running runCase, and it gave me the following error in the terminal: Code:
Running... #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 Uninterpreted: #3 Elliptic::ellipticIntegralsKE(double, double*, double*) at ??:? #4 cnoidalFun::calculations(double, double, double, double*, double*) at ??:? #5 Foam::IH_Waves_InletAlphaFvPatchScalarField::updateCoeffs() at ??:? #6 Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) at ??:? #7 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() at ??:? #8 at ??:? #9 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6" #10 at ??:? ./runCase: line 16: 10397 Floating point exception(core dumped) ihFoam > ihFoam.log Simulation complete. I am also attaching log files: BlockMesh: https://www.dropbox.com/s/onlb1p42tcda8gv/blockMesh.log ihFoam: https://www.dropbox.com/s/ltpdgv7btjbsi0s/ihFoam.log setFields: https://www.dropbox.com/s/5nbu2xzgy7v3zup/setFields.log The openFoam version I am using is 2.1.1. Thank you very much in advance, Dmitrijs |
|
July 29, 2014, 11:36 |
|
#6 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi Dmitrjs,
apparently there is a floating point error when evaluating the elliptic integrals for the cnoidal wave theory. Can I see your IHwavesDict? Best, Pablo |
|
July 29, 2014, 12:21 |
|
#7 |
New Member
Dmitrijs Gavrilovs-Stepanovs
Join Date: Jun 2014
Posts: 15
Rep Power: 12 |
Hi Pablo,
Thank you for a super quick reply! Here is the file: https://www.dropbox.com/s/cfui3ucupz4ekeg/IHWavesDict Regards, Dmitrijs |
|
July 29, 2014, 15:01 |
|
#8 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi Dmitrijs,
I see, you are running the case with no modifications. Unfortunately I am not able to reproduce your error. From the logs I can confirm that we are using the same build (2.1.1-221db2718bbb) and the case runs flawlessly for me: Code:
IH Wave Generation BC Wave theory: cnoidal H: 0.1 T: 3 h: 0.4 L: 3.73668 m parameter: 0.8011 Direction: 0º Which OS are you running? Version? 32 or 64 bits? Can run the case with other wave theories? Best, Pablo |
|
July 30, 2014, 06:50 |
Water depth
|
#9 |
New Member
Dmitrijs Gavrilovs-Stepanovs
Join Date: Jun 2014
Posts: 15
Rep Power: 12 |
Hi Pablo,
Thank you for your suggestions, I tried other wave theories and everything else runs fine. It's OK because I do not need to use cnoidal wave theory in my research, so I can continue with other ones. Another question I want to ask is how do you specify the water depth, I looked in the user guide, but couldn't find it. Sorry about this noob question Dmitrijs |
|
July 30, 2014, 06:55 |
|
#10 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi Dmitrjs,
no water depth needs to be specified, it is measured automatically by the BCs depending on the water (alpha1 field) that is set in setFieldsDict. Best, Pablo |
|
August 1, 2014, 04:15 |
|
#11 |
New Member
Join Date: Aug 2014
Posts: 9
Rep Power: 12 |
Dear Pablo,
first of all I would like to thank you a lot for having released IHFoam; it seems extremely useful and powerful, since it allows to reduce the computational domain extension significantly handling appropriately the boundary conditions for both wave generation and absorption. My main interest is focused on the evaluation of wave loads induced on semi and fully-submerged body. After having successfully installed IHFoam on OpenFOAM 2.2.2 version, I run the tutorial case "baseWaveFlume" and all seemed ok. Afterwards, I created a new case. I took as reference a case described in a MSc thesis freely available at the following URL: http://publications.lib.chalmers.se/...ext/151295.pdf The case is constituted by a 2D domain; there is an horizontal circular cylinder placed in the middle, whose axis is put exactly on the sea free surface at rest. At the inlet I generate a StokesV type wave. Since I would like to evaluate loads induced on the cylinder by the wave motion, I set in the controlDict file the forces function object structured as follows: forces { type forces; functionObjectLibs ("libforces.so"); log yes; patches (cylinder); pName p_rgh; UName U; rhoName rho; rhoInf 1; outputControl timeStep; outputInterval 1; } Unfortunately I get results that are completely different from those shown in the thesis. My first question is: is it correct to integrate the p_rgh term on the cylinder surface? I looked at the source code, and it seems almost identical to that of the openfoam distribution except for the porosity treatment, so I thought that integrating the p_rgh term was correct; but looking at the results I am not so sure. If you need more information before answering I can send you the case by email. I thank you a lot for your attention and for your help. Bye |
|
August 1, 2014, 04:38 |
|
#12 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi,
thanks for your feedback. The ihFoam solver solves the same equations as interFoam when no porosity is present. You can check it by running the same case, first with ihFoam and then with interFoam (loading the BCs dyanmically), you will obtain the same results. Regarding the force calculation, I would not integrate dynamic pressure (p_rgh) but total pressure (p). You should also check out if libforces.so is suitable for a two-phase case, as I remember doing some modifications long time ago, but now I am not quite sure what they were about. Best, Pablo |
|
August 1, 2014, 05:06 |
|
#13 |
New Member
Join Date: Aug 2014
Posts: 9
Rep Power: 12 |
Dear Pablo,
I thank you a lot for your quick answer. Concerning the libforces library, I have already checked if it works appropriately: I have read in other threads about the problems concerning the use of it with interFoam, but I think that they are solved in the version 2.2.2 I am using: in particular I am referring to the density value that is taken into account. The reason why I have integrated p_rgh and not p is that I would like to neglect the loads due to hydrostatic pressure and to consider only the dynamic ones; this because the work I took as reference explicitly tells that "...the initial force in still water are subtracted..." and I interpreted them as the hydrostatic forces. Unfortunately at the present I have no more idea where the problem is. I thank you a lot again for your help. Bye Gabriele |
|
August 1, 2014, 08:21 |
|
#14 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi Gabriele,
p_rgh is not generally the dynamic pressure, but a pseudo-dynamic pressure (p - rho g z). This is, the pseudo-dynamic pressure is dependent on the location of the fluid and its density. It is easy to see that a case at rest should have dynamic pressure equals zero, but that is only the case if the free surface lies at Z = 0. Moreover, two bodies of water at rest with different free surface elevation have different pseudo-dynamic pressure values. That is why I don't work with p_rgh, but with p, with which you can calculate the overpressure with respect to the initial state. Best, Pablo |
|
August 1, 2014, 11:07 |
|
#15 |
New Member
Join Date: Aug 2014
Posts: 9
Rep Power: 12 |
Dear Paul,
yes, you are right! My error was exactly what you said! I erroneously thought that p_rgh was exactly the dynamic pressure and not a pseudo-dynamic pressure dependent on z since I put the origin of the coordinate system at z=0 and at the initial time p_rgh=0. I thank you a lot for your useful help. Bye Gabriele |
|
August 1, 2014, 12:48 |
tsmooth - arbitrary starting time
|
#16 |
Member
Join Date: Dec 2009
Posts: 49
Rep Power: 16 |
Hi Pablo,
From IHFOAM manual, it stated that the tapering function, "tsmooth" varies linearly from t=0 to t=tsmooth. Say I want to start my wave simulation at arbitrary time e.g t=-32s instead of t=0s, will the tapering function, "tsmooth" works in this case? Kind regards, katakgoreng |
|
August 2, 2014, 04:29 |
|
#17 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi katakgoreng,
no, it will not work in that case. It won't be difficult for you to change the implementation and make it start at a given tStart. Best, Pablo |
|
August 4, 2014, 08:53 |
Shifted water depth
|
#18 |
New Member
Dmitrijs Gavrilovs-Stepanovs
Join Date: Jun 2014
Posts: 15
Rep Power: 12 |
Hi Pablo,
I modified the baseWaveFlume tutorial to simulate the following waves: Type - Regular, Stokes 1 Period - 3.651s Wave height - 0.033m Wave Length - 10.862m Frequency - 1.72 Hz I also modified the tank: Length (x) - 17.965m Height (z) - 1.1 Width (y) - 0.1 In setFields directory I specified the water level to be 1m, however, by looking at the results it seems like the water level is shifted a bit. Below is the plot of the surface elevation against time at x=9.989m: 3.651_0.0128_0.006875.png The cell size in x direction is 0.0128, in y it is 0.006875. The water level is shifted by 0.003125m. This happens at any x location along the wave tank. The analytical solution of Stokes 1st waves is also included for comparison. I then refined the mesh to get the cell size of 0.00367 in y direction and got the following: 3.651_0.0128_0.00367.png The water level is shifted upwards now by 0.001m. My question is: would you say that this error is due to the mesh resolution or is there something I messed up in the set-up? Even if I force the solution to start at water depth of 1 (by adding/subtracting the differences), it is not quite stable compared to the analytical solution: Test.png I am also attaching my case: https://www.dropbox.com/s/ju3xfehxk4...eWaveFlume.zip Thank you very much in advance! Dmitrijs |
|
August 4, 2014, 14:56 |
|
#19 | |
Member
Join Date: Dec 2009
Posts: 49
Rep Power: 16 |
Quote:
Thank you for your reply. I will implement the changes as needed. Moving on to other problem. I managed to run IHFOAM for irregular waves (First Order) without any problem. However, when I turn the "secondOrder" switch as follows: Code:
waveType irregular; genAbs 1; absDir 0.0; nPaddles 1; secondOrder 1; tSmooth 0; waveHeights 151 ( 6.9996e-55 1.5088e-44 1.1786e-36 1.5102e-30 9.1404e-26 5.5529e-22 5.8462e-19 1.5943e-16 1.5204e-14 6.3620e-13 1.3881e-11 1.8014e-10 1.5382e-09 9.3393e-09 4.2838e-08 1.5571e-07 4.6602e-07 1.1848e-06 2.6248e-06 5.1752e-06 9.2422e-06 1.5170e-05 2.3170e-05 3.3274e-05 4.5330e-05 5.9042e-05 7.4054e-05 9.0062e-05 1.0697e-04 1.2504e-04 1.4505e-04 1.6836e-04 1.9685e-04 2.3259e-04 2.7701e-04 3.2946e-04 3.8535e-04 4.3530e-04 4.6719e-04 4.7362e-04 4.5762e-04 4.2614e-04 3.8523e-04 3.4121e-04 2.9907e-04 2.6179e-04 2.3055e-04 2.0527e-04 1.8521e-04 1.6938e-04 1.5682e-04 1.4667e-04 1.3823e-04 1.3099e-04 1.2457e-04 1.1871e-04 1.1325e-04 1.0808e-04 1.0316e-04 9.8455e-05 9.3941e-05 8.9614e-05 8.5468e-05 8.1500e-05 7.7706e-05 7.4081e-05 7.0623e-05 6.7325e-05 6.4182e-05 6.1189e-05 5.8340e-05 5.5630e-05 5.3052e-05 5.0601e-05 4.8271e-05 4.6056e-05 4.3951e-05 4.1951e-05 4.0051e-05 3.8245e-05 3.6529e-05 3.4898e-05 3.3349e-05 3.1876e-05 3.0476e-05 2.9145e-05 2.7880e-05 2.6677e-05 2.5532e-05 2.4443e-05 2.3407e-05 2.2422e-05 2.1483e-05 2.0590e-05 1.9739e-05 1.8928e-05 1.8156e-05 1.7420e-05 1.6718e-05 1.6049e-05 1.5411e-05 1.4802e-05 1.4222e-05 1.3667e-05 1.3138e-05 1.2632e-05 1.2150e-05 1.1688e-05 1.1247e-05 1.0826e-05 1.0423e-05 1.0037e-05 9.6681e-06 9.3150e-06 8.9770e-06 8.6534e-06 8.3435e-06 8.0466e-06 7.7620e-06 7.4893e-06 7.2278e-06 6.9771e-06 6.7366e-06 6.5058e-06 6.2843e-06 6.0717e-06 5.8676e-06 5.6716e-06 5.4832e-06 5.3023e-06 5.1284e-06 4.9612e-06 4.8004e-06 4.6458e-06 4.4971e-06 4.3540e-06 4.2163e-06 4.0837e-06 3.9561e-06 3.8332e-06 3.7148e-06 3.6007e-06 3.4907e-06 3.3848e-06 3.2826e-06 3.1841e-06 3.0891e-06 2.9975e-06 2.9090e-06 2.8237e-06 2.7414e-06 ); wavePeriods 151 ( 3.884249368809477e+00 3.671732433514105e+00 3.481263838023756e+00 3.309592522968572e+00 3.154046799746415e+00 3.012465582580719e+00 2.883057424737786e+00 2.764301806471230e+00 2.654942440847882e+00 2.553913105660493e+00 2.460284851780139e+00 2.373278779565120e+00 2.292221575306356e+00 2.216513468644092e+00 2.145646483285414e+00 2.079174983366600e+00 2.016694194542422e+00 1.957859041980413e+00 1.902363115462027e+00 1.849923135693712e+00 1.800296688894330e+00 1.753266335182445e+00 1.708627715650175e+00 1.666205683094344e+00 1.625841779581378e+00 1.587384736025855e+00 1.550704950470484e+00 1.515684301148282e+00 1.482208312520658e+00 1.450179097118494e+00 1.419506863315684e+00 1.390103298576117e+00 1.361893140416630e+00 1.334806960217414e+00 1.308775470406623e+00 1.283739893757686e+00 1.259645737232861e+00 1.236437822632994e+00 1.214071083861960e+00 1.192497758104215e+00 1.171677737068486e+00 1.151573567701586e+00 1.132146391056949e+00 1.113363817234649e+00 1.095195486918437e+00 1.077609431237742e+00 1.060579224737798e+00 1.044080014115962e+00 1.028085232378105e+00 1.012573120436460e+00 9.975261351847418e-01 9.829169042049186e-01 9.687294144999418e-01 9.549365444666201e-01 9.415397941794010e-01 9.285137280754697e-01 9.158431710153953e-01 9.035137650322104e-01 8.915119150567447e-01 8.798247389120087e-01 8.684400211899366e-01 8.573461706633287e-01 8.465321809208577e-01 8.359875939441058e-01 8.257024663732671e-01 8.156673382327752e-01 8.058732039100968e-01 7.963114852005511e-01 7.869678130164477e-01 7.778469197261978e-01 7.689350249903883e-01 7.602250266078759e-01 7.517101405697962e-01 7.433838834374071e-01 7.352400558782441e-01 7.272727272727273e-01 7.194762213108857e-01 7.118451025056948e-01 7.043741635556808e-01 6.970584134950508e-01 6.898930665746810e-01 6.828735318219066e-01 6.759954032312580e-01 6.692499715568762e-01 6.626422195863787e-01 6.561636734667095e-01 6.498105802158671e-01 6.435793308062119e-01 6.374664533278936e-01 6.314686065382260e-01 6.255825737718250e-01 6.198052571881915e-01 6.141336723351205e-01 6.085649430078931e-01 6.030962963856439e-01 5.977250584276245e-01 5.924486495133034e-01 5.872645803113677e-01 5.821670586591529e-01 5.771606007087532e-01 5.722395165720564e-01 5.674016409255456e-01 5.626448810568722e-01 5.579672138465144e-01 5.533666828987560e-01 5.488413958134378e-01 5.443895215904884e-01 5.400092881597564e-01 5.356989800291421e-01 5.314569360444723e-01 5.272815472549722e-01 5.231712548785720e-01 5.191245483616429e-01 5.151373098499406e-01 5.112134674075854e-01 5.073489495340000e-01 5.035424209312513e-01 4.997925860767781e-01 4.960981877533202e-01 4.924580056435688e-01 4.888708549862383e-01 4.853355852904490e-01 4.818510791054916e-01 4.784162508432087e-01 4.750300456503874e-01 4.716914383287029e-01 4.683994322998880e-01 4.651530586139369e-01 4.619492410173970e-01 4.587913600411077e-01 4.556763604217741e-01 4.526033746107611e-01 4.495715583049353e-01 4.465800896732820e-01 4.436281686141943e-01 4.407150160420266e-01 4.378398732015727e-01 4.350020010092046e-01 4.322006794194680e-01 4.294352068159956e-01 4.267048994256552e-01 4.240090907549058e-01 4.213471310473847e-01 4.187166335182665e-01 4.161205084992614e-01 4.135563780732408e-01 4.110236544113114e-01 4.085217639969770e-01 4.060501471931783e-01 4.036082578249551e-01 4.011955627770757e-01 ); wavePhases 151 { 0 }; waveDirs 151 { 0 }; Code:
PIMPLE: Operating solver in PISO mode Reading field porosityIndex Porosity NOT activated Reading field p_rgh Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting turbulence model type laminar Reading g Calculating field g.h No finite volume options present time step continuity errors : sum local = 0, global = 0, cumulative = 0 GAMG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 Starting time loop Courant Number mean: 0 max: 0 Interface Courant Number mean: 0 max: 0 deltaT = 0.00011999 Time = -31.9999 alpha1 BC on patch inlet #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 secondOrderFun::C(double, double, double, double) at ??:? #4 secondOrderFun::etaSO(double, double, double, double, double, double, double, double, double, double, double, double, double, double) at ??:? #5 Foam::IH_Waves_InletAlphaFvPatchScalarField::updateCoeffs() at ??:? #6 Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) at ??:? #7 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() at ??:? #8 at ??:? #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #10 at ??:? Really appreciate your help in this matter. Kind regards, katakgoreng |
||
August 5, 2014, 02:40 |
|
#20 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
Hi Dmitrijs, katakgoreng,
@Dmitrijs I don't see anything wrong, setFields does not magically set water at your desired level, it just fills up full cells whose centre is inside the box you define. If the top of the filled cells is not exactly at 1 m, then you are definitely not obtaining that water level. I would also not expect great results from your resolution, as the wave height is discretized by 2 cells only, which may not be enough. @katakgoreng I copied your IHWavesDict over to the default baseWaveFlume tutorial and it runs perfectly well for me: Code:
Create time Create mesh for time = -32 PIMPLE: Operating solver in PISO mode Reading field porosityIndex Porosity NOT activated Reading field p_rgh Reading field alpha1 Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Selecting turbulence model type laminar Reading g Calculating field g.h time step continuity errors : sum local = 0, global = 0, cumulative = 0 DICPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 Starting time loop Courant Number mean: 0 max: 0 Interface Courant Number mean: 0 max: 0 deltaT = 0.00119048 Time = -31.9988 alpha1 BC on patch inlet MULES: Solving for alpha1 alpha1 BC on patch inlet Phase-1 volume fraction = 0.571429 Phase-1 total volume = 0.08 Min(alpha1) = 0 Max(alpha1) = 1 alpha1 BC on patch inlet MULES: Solving for alpha1 alpha1 BC on patch inlet Phase-1 volume fraction = 0.571429 Phase-1 total volume = 0.08 Min(alpha1) = 0 Max(alpha1) = 1 Velocity BC on patch inlet 3D_2D Absorption BC on patch outlet "Initial water depths for absorption" 1( 0.4 ) "Correction Levels" 1( 0 ) DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00153011, No Iterations 1 time step continuity errors : sum local = 0.00120801, global = -9.77904e-10, cumulative = -9.77904e-10 DICPCG: Solving for p_rgh, Initial residual = 0.000715141, Final residual = 2.98766e-05, No Iterations 16 Velocity BC on patch inlet 3D_2D Absorption BC on patch outlet "Correction Levels" 1( 0 ) time step continuity errors : sum local = 5.04735e-05, global = -3.37527e-05, cumulative = -3.37537e-05 DICPCG: Solving for p_rgh, Initial residual = 1.47718e-05, Final residual = 9.43515e-08, No Iterations 32 Velocity BC on patch inlet 3D_2D Absorption BC on patch outlet "Correction Levels" 1( 0 ) time step continuity errors : sum local = 3.19798e-07, global = -7.17437e-09, cumulative = -3.37609e-05 ExecutionTime = 2.74 s ClockTime = 3 s Courant Number mean: 1.09895e-06 max: 8.59363e-06 Interface Courant Number mean: 0 max: 0 deltaT = 0.00139456 Time = -31.9974 The problem seem the same you were facing with the cnoidal function. Which OS and version are you using? 32/64 bits? Best, Pablo |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Divergence detected in AMG solver: k when udf loaded | google9002 | Fluent UDF and Scheme Programming | 3 | November 7, 2019 23:34 |
udf problem | jane | Fluent UDF and Scheme Programming | 37 | February 20, 2018 04:17 |
UDF velocity profile | willroca | Fluent UDF and Scheme Programming | 2 | January 10, 2016 03:13 |
Error messages | atg | enGrid | 7 | August 30, 2013 11:16 |
Phase locked average in run time | panara | OpenFOAM | 2 | February 20, 2008 14:37 |