|
[Sponsors] |
Convergence problem using simpleFoam steady state |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 17, 2006, 10:34 |
dear all,
I am now caculati
|
#1 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
dear all,
I am now caculating a model(small mesh: 20000 cells, big: 1000000 cells) created in ICEM CFD(converting to OpenFoam by fluentMeshToFoam) with simpleFoam, but whichever mesh i use, I cant get the convergent solution. also tried reducing the timestep from 1s to 0.01s, but wouldn't help. time step continuity errors increase fast. but i got satisfying solution solving the same finer meshed model with ANSYS-CFX. anyone could be so kind to give any suggestion? PS: parameters in the transportation file were same as in the simpleFoam tutorial case. And fvScheme are Gauss and upwind. If i should change a better scheme, which one would you recommend? Thank you. |
|
January 17, 2006, 10:42 |
simpleFoam is a steady-state s
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
simpleFoam is a steady-state solver and changing the time-step size will do nothing at all (just change the names of output directories).
You should play around with the under-relaxation factors in the system/fvSolution file: relaxationFactors { p 0.2; U 0.7; k 0.5; epsilon 0.5; R 0.7; nuTilda 0.7; } change the default convergence on the pressure equation in the same file: solvers { p ICCG 1e-06 0.001; check if your k and epsilon are bounded (any warnings in the log file), adjust the spatial discretisation, play around with non-orthogonal correctors, try a limited laplacian scheme on k and epsilon (if appropriate, depending on the mesh) and similar. Good luck, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
January 31, 2006, 06:30 |
The mesh is hybrid, tet + pris
|
#3 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
The mesh is hybrid, tet + prism + hex, + few pyramids. The cells are around 300 000.
I did as you suggested above, and chose limited linear divScheme for k and epsilon, limitedLinearV divScheme for U, and tried some higher order schemes, but still time step continuity errors increase. Concerning the non-orthogonal correctors, I first used 10, slow, didn't help. each timestep more than 200s, and keeps increasing. Now am trying 20 as suggested in UserGuide U-114. it is extremely slow, I'm wondering should i stop the computation. |
|
January 31, 2006, 06:42 |
You can try the following:
|
#4 |
Senior Member
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 204
Rep Power: 18 |
You can try the following:
Initialize the flow as good as possible, set some relevant constant value for k and epsilon in the internal field. Use potentialFoam to initialize the velocity. Use upwind scheme initially for U,k,epsilon, and later change to a better scheme. Under-relax as proposed by Hrv. Decrease the Reynolds number by increasing the viscosity or lower the velocity, and later change back to the real Reynolds number. Use stabilizing boundary conditions. Typically a Dirichlet condition for the pressure at the outlet seems more stable than a Neumann bc. You can later try to switch back to the bc's you really want. Håkan. |
|
February 2, 2006, 11:09 |
Dear Vvqf,
I am also a CFX-Us
|
#5 |
New Member
Thomas Groensfelder
Join Date: Mar 2009
Posts: 6
Rep Power: 17 |
Dear Vvqf,
I am also a CFX-User and trying to do some comparison to OpenFOAM. Ho did you export your mesh from ICEM to Fluent? Everytime I when I convert the mesh I get error-messages from fluentMeshToFoam(see below). I am using a pure hexa mesh exporting as unstructured. So far I never had a problems with CFX. Thanks in advance Thomas Here is the beginning of the error messages: /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.2 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : fluentMeshToFoam . . fluent.msh Date : Feb 02 2006 Time : 16:03:10 Host : arianna PID : 10095 Root : /romeo_home/groens/OpenFOAM/groens-1.2/run/movingIcoSFD Case : . Nprocs : 1 Create time Dimension of grid: 3 Number of points: 12000 Reading points Number of cells: 9044 Reading uniform cells number of faces: 29945 Reading uniform faces Reading uniform faces Reading uniform faces Reading uniform faces Reading uniform faces Reading zone data Reading zone data Reading zone data Reading zone data Reading zone data Reading zone data FINISHED LEXING dimension of grid: 3 Creating shapes for 3-D cells Creating patch for zone: 15 start: 1 end: 24319 type: interior name: int_MDL_CRVS Patch 15 contains solid or internal faces. Not added to boundary Adding to internal boundaries Creating patch for zone: 16 start: 24320 end: 24471 type: wall name: MIRROR Creating patch for zone: 17 start: 24472 end: 24947 type: wall name: ROTOR_AUS Creating patch for zone: 18 start: 24948 end: 29469 type: wall name: VOLUMEN Creating patch for zone: 19 start: 29470 end: 29945 type: wall name: WAND Default patch type set to empty Checking mesh --> FOAM Serious Error : From function bool primitiveMesh::checkClosedCells(const bool report, labelHashSet*) const in file meshes/primitiveMesh/primitiveMeshCheck.C at line 289 9044 high aspect ratio cells found. Max aspect ratio: 2.63847e+199 --> FOAM Warning : From function primitiveMesh::checkFaceDotProduct(const bool report, labelHashSet* setPtr) const in file meshes/primitiveMesh/primitiveMeshCheck.C at line 534 Severe non-orthogonality detected for face 0 between cells 0 and 1: Angle = 180 deg. --> FOAM Warning : From function primitiveMesh::checkFaceDotProduct(const bool report, labelHashSet* setPtr) const in file meshes/primitiveMesh/primitiveMeshCheck.C at line 534 Severe non-orthogonality detected for face 1 between cells 0 and 4: Angle = 179.991 deg. |
|
February 2, 2006, 15:04 |
Sounds like your cells are def
|
#6 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
Sounds like your cells are defined inside out or rather the converter expects the numbering of the vertices of a hex to be in a certain order. See the User Guide (section 6 I believe) on what Foam expects.
Try creating a 1 hex mesh and put some print statements in the converter where it creates a the cellShape. E.g. Pout<< cellShapes[cellI] << endl; and see if you can figure out what needs to be changed. |
|
February 2, 2006, 16:44 |
Hello Mattjis,
thanks for you
|
#7 |
New Member
Thomas Groensfelder
Join Date: Mar 2009
Posts: 6
Rep Power: 17 |
Hello Mattjis,
thanks for your quick answer. You put me on the right way. I just built up my grid from scratch and found out that it is working when I create my mesh with another block orientation. I think the problem is in the vertice-numbering. I didn't expect this problem as the export function of icem is explicitely for an unstuctured mesh type. Found a check-mesh function in icem which I never had to use during the last 4 years. Anyway, thanks a lot one more time. Thomas |
|
February 3, 2006, 09:18 |
BTW, OpenFoam also offers the
|
#8 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
BTW, OpenFoam also offers the Checkmesh utility.
The turbulence model I chose for simpleFoam is k-epsilon model. I want to use SST model, but it is not available in OpenFoam. Do you think RNGkEpsilon might be a better choice? |
|
February 3, 2006, 09:54 |
As Håkan suggested, I did firs
|
#9 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
As Håkan suggested, I did first a potentialFoam calculation. And it seems now to be convergent, the time step continuity errors is decreasing slightly.
But the computing time increase, and from 5th timestep, it needs over 20 minutes(1200+s). non-orthogonal correctors is set to 6. any way to improve? ps: 2-cpu machine, 3G mem. |
|
February 3, 2006, 10:07 |
Have you tried upwind? Also, c
|
#10 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
Have you tried upwind? Also, check if you are getting inflow at the outlet. That is the most common source of instability.
For simpleFoam, non-orthogonal correctors do not always improve convergence (at least in my experience), more than 1 is probably overkill. I would try with different values and see how the simulation reacts. |
|
February 3, 2006, 10:34 |
Yes, the outlet. I just have p
|
#11 |
Member
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 17 |
Yes, the outlet. I just have problem there.
I tried upwind, and the outlet pressureOutlet, but without initializing U with potentialFoam. The boundary condition I want for the outlet is openning. Later I swithed to pressureInletOutlet. Under inletOutlet, there are 3 other options. But i dont know what are they for, like freeStream and atmosphere. dont know which to choose. Thank you! |
|
April 9, 2008, 08:56 |
Hello!
I am calculating a m
|
#12 |
New Member
Gabriela Bracho
Join Date: Mar 2009
Location: Valencia, Valencia, Spain
Posts: 14
Rep Power: 17 |
Hello!
I am calculating a model created in OpenFOAM (using blockMesh), with simpleFoam, but I can't get the convergent solution (incompresible flow). The geometry is similar to the nozzle2D case used in cavitatingFoam BC==> back and front: wedge, inlet and outlet pressure: positive values normalized by density, inlet and outlet velocities: zeroGradient, Wall velocity: fixedvalue (0 m/s) The problem is that Ux, Uy, k and epsilion converged, but Uz never converged.... I've played with all relaxation factors, solvers, fvSchemes.... and it didn't get better Anyone could be so kind to give any suggestion? or explain why this Uz never converged Thank you! Gaby |
|
May 18, 2011, 08:51 |
|
#13 | |
New Member
Daniel Plucenio
Join Date: May 2011
Posts: 7
Rep Power: 15 |
Hello Gaby, I am using OpenFOAM to simulate flow in a duct, using the wedge geometry and axisymmetric condition. I am having the same problem with Uz that you had years ago. Did you find out how to manage tha problem with Uz convergence?
Thanks in advance, Regards Quote:
|
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
convergence for transient/steady state simulation | Gab | CFX | 36 | August 20, 2012 13:55 |
SimpleFoam unable to reach steady state | francois | OpenFOAM Running, Solving & CFD | 8 | November 19, 2009 14:33 |
Steady state DPM - Convergence and particle tracks | Sandilya Garimella | FLUENT | 2 | March 28, 2008 16:53 |
transient problem run in steady state | luigi | FLUENT | 4 | March 13, 2008 07:54 |
steady state PISO problem | denizen | Siemens | 0 | December 20, 2006 03:55 |