Hello at all,
I'm looking here to get some help with openfvm. I trying to calc the flow properties (velocities and the pressure) of a complex 3 dim. Geometry. I used gmsh to produce the mesh. Starting from the files of the tutorial I defined the boundary conditions and etc. After a few calculation steps of my problem case I got following error message:
“Problem solving matrix p” (or sometimes u or v)
I made some changes in the par file but without success
Did anyone can give a little advise what could be the problem. If necessary it would be possible to provide the files of my case study.
Thanks in advance
Can you send me the files to see what is happening?
This problem is related to the solver reaching the maximum number of iterations. You can try increasing the number of iterations but usually it has to do with error due to oscillation of the calculations. It might be necessary to reduce time step or improve mesh quality.
I've send you the desired files. May be you can find out what is my mistake.
Thanks in advance,
Sorry I didn't respond sooner. Some how your email got in my spam folder.
I haven't seen yet the wdb case. Although, to get the cube example working consider setting "convection interpolation scheme" for u,v,w to 0 (upwind). In some cases I found that it is also useful to set "adjust time step" to 0 (disabled). This feature is mostly used for free surface calculations. If you are using windows set "binary output" to 0 because there is a bug when saving binary format in windows.
thanks for your. In fact, changing the convection interpolation scheme to 0 the cube example works. The second case with the complex 3D geometry is more difficult to keep them working. I try to modify the unstructed grid, but a steady state solution cannot be achieved, maximum solution time, 20 seconds. I'm not sure if with a improved mesh it would be possible to get a steady state solution. Did you have any more advises for me?
Try removing all non-orthogonal corrections, i.e. set to zero sometimes gmsh doesn't create to good tetrahedral meshes. The best would be to use a hexahedral mesher. It's a pitty gmsh doesn't have one.
the cube sample works fine with and without structed meshes. The residiuum will be reduced each iteration and the steady state solution will be achieved.
The residuum of the complex geometry from the sample wbd with unstructed grids decreases during the first iterations < 200, but for longer iteration times the residuum will be still constant on a higher level, e.g. for the pressure value > 1E4 (iteration # >2500). I've done a plot, but it is not possible to post this here. So my question is, how could I done to stabilize the solution for the steady state case?
Here my par file:
$File Parameter file
$Parameter 1 30 Description of $Code
30005 1 Convection interpolation scheme
0 0 0 0 0 0
30020 1 Binary output
30030 1 Time advancement method (u v w p T s)
2 2 2 2 0 0
30031 1 Explicit factor (u v w p T s)
30040 1 Calculate variable (u v w p T s)
1 1 1 1 0 0
30090 1 Stability factor
30100 1 Steady state
30105 1 Convergence for steady state solutions
1E1 1E1 1E1 1E1 1E1 1E1
30200 1 Adjust time interval
30201 1 Maxmimum Courant number
30400 1 Number of saves
30450 1 Write face scalars (u v w p T s)
30455 1 Write face vectors (uvw)
30460 1 Write element scalars (u v w p T s)
30465 1 Write element vectors (uvw)
30470 1 Write vorticity (x y z)
0 0 0
30475 1 Write stream function (xy)
30485 1 Probe (u v w p T s)
1 1 1 1 0 0
30500 1 Smooth values
30550 1 Maximum number of non-othorgonal corrections
30600 1 Convergence criterion (matrix solution)
1E-12 1E-12 1E-12 1E-12 1E-12 1E-12
30601 1 Maximum number of iterations (matrix solution)
100000 100000 100000 100000 100000 100000
30650 1 Matrix solver (u v w p T s) (0-Jacobi, 1-SOR, 2-CGN, 3-GMRES, 4-BiCG, 5-QMR, 6-CGS, 7-BiCGStab, 8-BiCGStabM)
8 8 8 7 8 8
30651 1 Matrix preconditioner (0-Null, 1-Jacobi, 2-SOR, 3-ILU)
3 3 3 3 3 3
30800 1 Interface scheme factor - CICSAM
30900 1 Maximum number of CICSAM corrections
32000 1 Start time
32001 1 End time
32002 1 Time interval
34000 1 Gravity vector
0.0 0.0 0.0
What type of mesh are you using? Can you send me the geo file?
Remember that if flow is turbulent it may never reach steady-state since OpenFVM does not calculate variables averged in time.
I send you a mail with the geo file. I used tetrahedral meshes out of gmsh. In my opinion a steady state vortex flow should be achieved. But I'm not sure. So at first I started to simulate the unsteady behavior, but without success. This means that I got for different time steps and calculation duration the same vector plot of the velocity. May be you can find out what kind of error I'm doing?
It looks like an interesting case. I think the problem is related with mesh quality. Gmsh uses MesAdpat+Delauny as default. The frontal method seems to produce better mesh quality for this case. The best would be to have a hexahedral mesh. For this you need to divide your geometry into smaller sections and use structured meshing.
Also don't enable adjust time step option. It is only for multiphase flows.
I have tried with Frontal method and removed the adjust time step and got much better results. Eventhough mesh is still tetrahedral.
thanks very much for your effort. I will try a last run with structured hexa meshes. It seem to be the last possible chance to produce a stable solution. I'll report here my experience if could achieve a nice solution.
Thanks and best regards,
Log in to post a comment.
Sign up for the SourceForge newsletter:
You seem to have CSS turned off.
Please don't fill out this field.