
[Sponsors] 
September 23, 2008, 11:12 
Musa:
(1) Pick up patch lik

#81 
Member
vof_user
Join Date: Mar 2009
Posts: 67
Rep Power: 9 
Musa:
(1) Pick up patch like wall  not internal mesh (2) If your are using paraview 3.3 you get the plot over line with some default coordinates which you can change (3) You may not get gamma=0.5 if you are at time step 0, so take some higher time step or you may remove the available entry of gamma and add a new value of gamma=0.5 (4) When you apply the integrate variables from filters menu you will see some data displayed in a spreadsheet which may not be useful so keep the Contour1 flag visible by making the data visible (eye)  just above IntegrateAttributes1. When you make this you will observe change in the data in spreadsheet which is the one required. (5) Select a row in the spreadsheet with mouse to highlight and then plot selection over time from filter menu. But before you apply you must copy the active selection which you can see below the apply button. Then apply to get the displacement with time. 

September 25, 2008, 10:26 
Gentlemen:
Can someone dire

#82 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 10 
Gentlemen:
Can someone direct me to where mesh refinement is performed. For example if I want mesh refinement at say evey 5th timestep,then where in the documentation is this discussed or where do I need to put this info? Also where is cell expansion discussed? Does cell expansion mean the originial cells are being increased in size or is it implying mesh refinement, ie, more cells are being added? Comments appreciated! Thanks Musa 

October 28, 2008, 14:49 
Replace
functionObjectLibs(

#83 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9 
Replace
functionObjectLibs("libsampling.so"); by functionObjectLibs ("libsampling.so"); Please note the blank space. If you were also interested in indicating the number of iterations between one probe and the next one, add this line: // E.g. write probes each 10 iterations interval 10; Cheers Patricio 

October 28, 2008, 16:22 
Hi
just read musaddeque's po

#84 
Senior Member
Hua Zen
Join Date: Mar 2009
Posts: 114
Rep Power: 9 
Hi
just read musaddeque's post.I have one question.In his post: // Name of the directory for the probe data name probes; I could find these lines in the interDyMFoam tutorial case.From the comment it seems that it is related to the output. while from the source code,it seems that it is exclusively used by sampledSurface,not related to output. could somebody make me clear? 

October 28, 2008, 21:38 
patrico:
Many thanks for po

#85 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 10 
patrico:
Many thanks for pointing out the error!. The block mesh and set fields now run without a problem. However, when I execute interFoam, the following error is sent to the screen: 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 deltaT = 0.00119048 > FOAM Warning : From function probes::read() in file probes/probes.C at line 72 Did not find location (0.035 0.01 0.05) in any cell. Skipping location. Time = 0.00119048 The analysis continues and the probe file records the same gamma value for each time step. This should not be the case since the gamma will be a 1 or 0 depending if there is "water" on the probe or "air" as the water sloshes over the probe. However, the probe point is right at the phase interface  between the water and air (I am running the damBreak problem). How am I supposed to figure out whether this point is in a cell or not? Any suggestions? Musa 

October 29, 2008, 05:41 
checkMesh case damBreak =>

#86 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9 
checkMesh case damBreak =>
Checking geometry... Domain bounding box: (0 0 0) (0.584 0.584 0.0146) Your error: Did not find location (0.035 0.01 0.05) in any cell. I would say that 0.05 > 0.0146, i.e. your probe is out of the computational domain. 

October 29, 2008, 16:10 
Patrico:
Sorry  I hade mad

#87 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 10 
Patrico:
Sorry  I hade made modifictions to the box geometry as follows: convertToMeters 0.01; vertices ( (0 0 0) // 0 (14 0 0) // 1 (14 10 0) // 2 (0 10 0) // 3 (0 10 0.1) // 4 (0 0 0.1) // 5 (14 0 0.1) // 6 (14 10 0.1) // 7 ); Based on above the probe location of 0.035, 0.01 and 0.05 should be within the box. let me know what you think. Thanks, Musa 

October 29, 2008, 17:12 
I wonder if you have already r

#88 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9 
I wonder if you have already read the User Guide?
5.3.1 Writing a blockMeshDict file The blockMeshDict file is a dictionary using keywords described in Table 5.5. The convertToMeters keyword specifies a scaling factor by which all vertex coordinates in the mesh description are multiplied. For example, convertToMeters 0.001; means that all coordinates are multiplied by 0.001, i.e. the values quoted in the blockMesh Dict file are in mm. In your case, 0.01*0.1=0.001 < 0.05. 

October 30, 2008, 11:22 
Patrico:
You were right abo

#89 
Senior Member
musaddeque hossein
Join Date: Mar 2009
Posts: 309
Rep Power: 10 
Patrico:
You were right about the error. Many thanks. Musa 

November 12, 2008, 04:27 
Time = 0.0038
Courant Numbe

#90 
Guest
Posts: n/a

Time = 0.0038
Courant Number mean: 2.09671 max: 1060.3 DILUPBiCG: Solving for Ux, Initial residual = 0.919624, Final residual = 1.67874e06, No Iterations 37 DILUPBiCG: Solving for Uy, Initial residual = 0.901699, Final residual = 2.47234e06, No Iterations 36 DILUPBiCG: Solving for Uz, Initial residual = 0.938489, Final residual = 4.1829e06, No Iterations 36 DICPCG: Solving for p, Initial residual = 0.879601, Final residual = 0.00364827, No Iterations 1001 time step continuity errors : sum local = 0.0259577, global = 9.6956e08, cumulative = 3.94409e06 DICPCG: Solving for p, Initial residual = 0.666183, Final residual = 0.000557632, No Iterations 1001 time step continuity errors : sum local = 0.0113467, global = 8.28394e06, cumulative = 1.2228e05 DILUPBiCG: Solving for T, Initial residual = 0.64382, Final residual = 6.68318e08, No Iterations 59 ExecutionTime = 378.29 s ClockTime = 381 s Time = 0.0039 Courant Number mean: 9.857 max: 30723.2 DILUPBiCG: Solving for Ux, Initial residual = 0.992898, Final residual = 7.52633e06, No Iterations 52 DILUPBiCG: Solving for Uy, Initial residual = 0.990041, Final residual = 4.81015e06, No Iterations 55 DILUPBiCG: Solving for Uz, Initial residual = 0.995945, Final residual = 7.08196e06, No Iterations 51 DICPCG: Solving for p, Initial residual = 0.943505, Final residual = 0.00279098, No Iterations 1001 time step continuity errors : sum local = 0.133287, global = 0.000834918, cumulative = 0.000847146 DICPCG: Solving for p, Initial residual = 0.511564, Final residual = 0.000185419, No Iterations 1001 time step continuity errors : sum local = 0.0590576, global = 0.0111944, cumulative = 0.0103473 DILUPBiCG: Solving for T, Initial residual = 0.906877, Final residual = 6.47856e08, No Iterations 76 ExecutionTime = 392.06 s ClockTime = 395 s Time = 0.004 Courant Number mean: 114.419 max: 474556 DILUPBiCG: Solving for Ux, Initial residual = 0.997831, Final residual = 5.29673e06, No Iterations 199 DILUPBiCG: Solving for Uy, Initial residual = 0.995946, Final residual = 2.97571e06, No Iterations 208 DILUPBiCG: Solving for Uz, Initial residual = 0.997078, Final residual = 7.97488e06, No Iterations 198 DICPCG: Solving for p, Initial residual = 0.967972, Final residual = 0.244505, No Iterations 1001 time step continuity errors : sum local = 357.75, global = 0.0473633, cumulative = 0.0577106 DICPCG: Solving for p, Initial residual = 0.43629, Final residual = 0.000865386, No Iterations 1001 time step continuity errors : sum local = 78.2216, global = 0.0380752, cumulative = 0.0957858 DILUPBiCG: Solving for T, Initial residual = 0.96816, Final residual = 8.15618e08, No Iterations 88 ExecutionTime = 411.14 s ClockTime = 414 s Time = 0.0041 I have such a problem that courant number increasing after a while...I can t find out the problem...I have decrease time steps and it is working longer but again crash... can someone help me? best regards emo 

November 12, 2008, 04:42 
Hi Emo
This is not an inter

#91 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,698
Rep Power: 27 
Hi Emo
This is not an interFoamrelated question, as you are using a different solver. Thus please use approapriate threads in the future. Further, when you are not informing which solver you are using, you cannot expect qualified help. Your timestep must be too large, thus either adjust your solver to use a Courantlimited timestep or lower your time step. If that is not helping, there might be problems with your mesh and/or initial conditions/BC. Best regards, Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

November 12, 2008, 05:08 
hi Niels,
Sorry about that,

#92 
Guest
Posts: n/a

hi Niels,
Sorry about that,I see... I am using turbFoam and I have include transport equation but there is something wrong... I can t find out... regards Emo 

November 25, 2008, 13:49 
Dear users
I have a questio

#93 
New Member
Marc Wainwright
Join Date: Mar 2009
Posts: 3
Rep Power: 9 
Dear users
I have a question relating to the simulation of a 2phase flow using the interFoam solver. My problem consists of a gravity driven liquid film falling down a vertical wall in a quiescent gaseous atmosphere. Due to its instability the falling film develops surface waves which in their developed state cause the velocity and pressure distribution in the liquid phase to be periodic in streamwise direction (the periodicity of pressure is due to the fact that the film is driven by gravity and not by pressure). As I'm focusing on the developed state of the film I'm simulating only one surface wave using a cyclic boundary condition in streamwise direction. My computational domain has a length of one wavelength. I have previously simulated the full film with interFoam under the given conditions and have therefore a pretty good understanding of what the flow should look like. In the simulation with the cyclic boundary condition I have observed that the face values for pd on the cyclic boundary differ considerably for the cells on either side of it. Indeed, the data files for pd contain a list of values associated with the cyclic boundary with a length of two times the amount of faces on that boundary. As far as I can tell this list is not one of matching value pairs. The same is true for the values of the other variables U and gamma although the difference between values associated with different sides of the cyclic boundary is smaller. Further, I observe an abrupt pressure change between the last interior cell face and the corresponding face on the cyclic boundary for both "sides" of the domain. This erroneous pressure distribution is causing dynamics that do not correspond with the simulation of the full film. I assume that the cause of this problem is the use of a cyclic boundary condition. I would be grateful for any help in this matter. Yours faithfully Marc 

November 25, 2008, 17:16 
Dear Marc
are you simulatin

#94 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9 
Dear Marc
are you simulating Kapitza instabilities? For sake of simplicity, we must first think in the uniform stream falling down the vertical wall. The momentum equation along the direction of the gravity (z) establishes that the vertical gradient of the reduced pressure (pd) is balanced with the viscous forces, where the reduced pressure is related with the absolute pressure (P) by pd = P  rho g z. I mean, the reduced pressure is not periodic, but the absolute pressure. interFoam solves pd, not P! Good luck P 

November 27, 2008, 14:12 
Dear Patricio
Thank you for

#95 
New Member
Marc Wainwright
Join Date: Mar 2009
Posts: 3
Rep Power: 9 
Dear Patricio
Thank you for your swift reply. Yes I am simulating Kapitza instabilities. Your remark about the definition of pd was most helpful. I have checked the data files for pd and p and observed that the cyclic condition is applied to the variable pd which leads to a jump in p over the cyclic boundary. Is there a way to explicitly or implicitly achieve that the cyclic condition is applied to p and not to pd? Yours sincerely Marc 

December 2, 2008, 10:09 
Hi,
i'm also very intereste

#96 
Member
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 9 
Hi,
i'm also very interested in the question of Marc Wainwright: "Is there a way to explicitly or implicitly achieve that the cyclic condition is applied to p and not to pd?". Any idea? Thank you Eric 

December 2, 2008, 11:46 
You just need to rewrite the

#97 
Member
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 9 
You just need to rewrite the PISOLoop as a function of p instead of pd. This means that the flux prediction in pEqn.H is to be modified, as well as the momentum predictor in UEqn.H, replacing ghf*fvc::snGrad(rho) by the discretisation of rho*g.


December 3, 2008, 03:01 
Hi,
thank you for the answe

#98 
Member
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 9 
Hi,
thank you for the answer. If i have well understood what you said, as the PISO loop is now done (based on pd), i could impose a non cyclic boundary condition to the p field only. However, when trying it just as a test, i receive the following error, due to the fact, i think, that i declare not a patch but cyclic in my blockMeshDict file: inconsistent patch and patchField types for patch type cyclic and patchField type calculated file: /net/ric_home/ep4/OpenFOAM/ep41.5/run/free_convection_channel/Mesh_coarse/0/p:: inout1 from line 47 to line 48. From function fvPatchField<type>::New(const fvPatch&, const DimensionedField<type,>&, const dictionary&) in file /home/dm2/henry/OpenFOAM/OpenFOAMdev/src/finiteVolume/lnInclude/newFvPatchField .C at line 140. FOAM exiting Is there something else i should also do? If i want a steady solution, have you advices? How modify the SIMPLE alogorithm or something else? Thank you Eric 

December 4, 2008, 03:09 
Hi,
Any comment on my previ

#99 
Member
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 9 
Hi,
Any comment on my previous post ? It could be really interesting for to be able to impose a cyclic boundary condition for all fields, except for the pd field. Thank you Eric 

December 6, 2008, 18:58 
Eric,
I have pondered over

#100 
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 579
Rep Power: 20 
Eric,
I have pondered over this before and there is a limitation in OF (in my humble opinion) that If you define a patch as cyclic then you cannot use a noncyclic patch type on another field. OF sees that you are trying to do this and spits out some errors, as it should. i have seen posts that discuss options to fix this, but they seem somewhat difficult. personally I see some utility in allowing a patch to be cyclic in some equations and noncyclic in others. For instance once might want cyclic flow (momentum only) and watch the evolution of heat in the system by no cyclic behavior. Solving this type of problem is of great importance to my thesis and I will pick this up after the hollidays and try to figure it out. Dan 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
InterFoam MULES solver  jaswi  OpenFOAM Running, Solving & CFD  4  November 21, 2012 09:56 
Wmake problem interFoam solver  feijooos  OpenFOAM Running, Solving & CFD  4  December 8, 2008 12:01 
DICPCG solver in interFoam  m9819348  OpenFOAM Running, Solving & CFD  1  September 20, 2007 13:10 
About interfoam solver  qiu  OpenFOAM Running, Solving & CFD  0  May 6, 2007 22:48 
Need documentation for interFOAM solver  mer  OpenFOAM Running, Solving & CFD  5  May 31, 2006 12:22 