CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

About interFoam solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 23, 2008, 11:12
Default Musa: (1) Pick up patch lik
  #81
Member
 
a a saha
Join Date: Mar 2009
Posts: 67
Rep Power: 8
asaha is on a distinguished road
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.
asaha is offline   Reply With Quote

Old   September 25, 2008, 10:26
Default Gentlemen: Can someone dire
  #82
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
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
musahossein is offline   Reply With Quote

Old   October 28, 2008, 14:49
Default Replace functionObjectLibs(
  #83
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 8
pbohorquez is on a distinguished road
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
pbohorquez is offline   Reply With Quote

Old   October 28, 2008, 16:22
Default Hi just read musaddeque's po
  #84
lin
Senior Member
 
Hua Zen
Join Date: Mar 2009
Posts: 114
Rep Power: 8
lin is on a distinguished road
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?
lin is offline   Reply With Quote

Old   October 28, 2008, 21:38
Default patrico: Many thanks for po
  #85
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
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
musahossein is offline   Reply With Quote

Old   October 29, 2008, 05:41
Default checkMesh -case damBreak =>
  #86
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 8
pbohorquez is on a distinguished road
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.
pbohorquez is offline   Reply With Quote

Old   October 29, 2008, 16:10
Default Patrico: Sorry - I hade mad
  #87
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
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
musahossein is offline   Reply With Quote

Old   October 29, 2008, 17:12
Default I wonder if you have already r
  #88
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 8
pbohorquez is on a distinguished road
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.
pbohorquez is offline   Reply With Quote

Old   October 30, 2008, 11:22
Default Patrico: You were right abo
  #89
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Patrico:

You were right about the error. Many thanks.

Musa
musahossein is offline   Reply With Quote

Old   November 12, 2008, 04:27
Default Time = 0.0038 Courant Numbe
  #90
emilianyassenov
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 = 1.67874e-06, No Iterations 37
DILUPBiCG: Solving for Uy, Initial residual = 0.901699, Final residual = 2.47234e-06, No Iterations 36
DILUPBiCG: Solving for Uz, Initial residual = 0.938489, Final residual = 4.1829e-06, 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 = 9.6956e-08, cumulative = 3.94409e-06
DICPCG: Solving for p, Initial residual = 0.666183, Final residual = 0.000557632, No Iterations 1001
time step continuity errors : sum local = 0.0113467, global = 8.28394e-06, cumulative = 1.2228e-05
DILUPBiCG: Solving for T, Initial residual = 0.64382, Final residual = 6.68318e-08, 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 = 7.52633e-06, No Iterations 52
DILUPBiCG: Solving for Uy, Initial residual = 0.990041, Final residual = 4.81015e-06, No Iterations 55
DILUPBiCG: Solving for Uz, Initial residual = 0.995945, Final residual = 7.08196e-06, 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 = 6.47856e-08, 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 = 5.29673e-06, No Iterations 199
DILUPBiCG: Solving for Uy, Initial residual = 0.995946, Final residual = 2.97571e-06, No Iterations 208
DILUPBiCG: Solving for Uz, Initial residual = 0.997078, Final residual = 7.97488e-06, 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 = 8.15618e-08, 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
  Reply With Quote

Old   November 12, 2008, 04:42
Default Hi Emo This is not an inter
  #91
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Emo

This is not an interFoam-related 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 Courant-limited 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 Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   November 12, 2008, 05:08
Default hi Niels, Sorry about that,
  #92
emilianyassenov
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
  Reply With Quote

Old   November 25, 2008, 13:49
Default Dear users I have a questio
  #93
New Member
 
Marc Wainwright
Join Date: Mar 2009
Posts: 3
Rep Power: 8
marc_w is on a distinguished road
Dear users

I have a question relating to the simulation of a 2-phase 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
marc_w is offline   Reply With Quote

Old   November 25, 2008, 17:16
Default Dear Marc are you simulatin
  #94
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 8
pbohorquez is on a distinguished road
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
pbohorquez is offline   Reply With Quote

Old   November 27, 2008, 14:12
Default Dear Patricio Thank you for
  #95
New Member
 
Marc Wainwright
Join Date: Mar 2009
Posts: 3
Rep Power: 8
marc_w is on a distinguished road
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
marc_w is offline   Reply With Quote

Old   December 2, 2008, 10:09
Default Hi, i'm also very intereste
  #96
ep4
Member
 
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 8
ep4 is on a distinguished road
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
ep4 is offline   Reply With Quote

Old   December 2, 2008, 11:46
Default You just need to re-write the
  #97
Member
 
Patricio Bohorquez
Join Date: Mar 2009
Location: Jaén, Spain
Posts: 94
Rep Power: 8
pbohorquez is on a distinguished road
You just need to re-write the PISO-Loop 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.
pbohorquez is offline   Reply With Quote

Old   December 3, 2008, 03:01
Default Hi, thank you for the answe
  #98
ep4
Member
 
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 8
ep4 is on a distinguished road
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/ep4-1.5/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/OpenFOAM-dev/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
ep4 is offline   Reply With Quote

Old   December 4, 2008, 03:09
Default Hi, Any comment on my previ
  #99
ep4
Member
 
Pattyn Eric
Join Date: Mar 2009
Posts: 61
Rep Power: 8
ep4 is on a distinguished road
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
ep4 is offline   Reply With Quote

Old   December 6, 2008, 18:58
Default Eric, I have pondered over
  #100
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 546
Rep Power: 18
chegdan will become famous soon enough
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 non-cyclic 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 non-cyclic 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
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 02:58.