Error: Problem solving matrix p

Help
pajofego
2009-11-23
2013-04-25
  • pajofego

    pajofego - 2009-11-23

    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
    pajofego

     
  • x-flow

    x-flow - 2009-11-23

    Hi,

    Can you send me the files to see what is happening?

    x-flow@users.sourceforge.net

    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.

     
  • pajofego

    pajofego - 2009-11-26

    Hi,

    I've send you the desired files. May be you can find out what is my mistake.

    Thanks in advance,
    pajofego

     
  • x-flow

    x-flow - 2009-11-26

    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.

     
  • pajofego

    pajofego - 2009-11-29

    Hi,

    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?

    Thanks in advance,
    pajofego

     
  • x-flow

    x-flow - 2009-11-30

    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.

     
  • pajofego

    pajofego - 2009-12-02

    Hi,

    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:
    $Title OpenFVM

    $File Parameter file

    $Parameter 1 30 Description of $Code

    30005 1 Convection interpolation scheme

    0 0 0 0 0 0

    30020 1 Binary output

    1

    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)

    0 0 0 0 0 0

    30040 1 Calculate variable (u v w p T s)

    1 1 1 1 0 0

    30090 1 Stability factor

    1

    30100 1 Steady state

    1

    30105 1 Convergence for steady state solutions

    1E1 1E1 1E1 1E1 1E1 1E1 

    30200 1 Adjust time interval

    1

    30201 1 Maxmimum Courant number

    0.9

    30400 1 Number of saves

    1

    30450 1 Write face scalars (u v w p T s)

    0 0 0 0 0 0

    30455 1 Write face vectors (uvw)

    0

    30460 1 Write element scalars (u v w p T s)

    0 0 0 0 0 0

    30465 1 Write element vectors (uvw)

    0

    30470 1 Write vorticity (x y z)

    0 0 0

    30475 1 Write stream function (xy)

    0

    30485 1 Probe (u v w p T s)

    1 1 1 1 0 0

    30500 1 Smooth values

    0

    30550 1 Maximum number of non-othorgonal corrections

    0

    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

    1.0

    30900 1 Maximum number of CICSAM corrections

    2

    32000 1 Start time

    0.0

    32001 1 End time

    55.5

    32002 1 Time interval

    0.01

    34000 1 Gravity vector

    0.0 0.0 0.0

    $EndFile

     
  • x-flow

    x-flow - 2009-12-02

    Hi,

    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.

     
  • pajofego

    pajofego - 2009-12-03

    Hi,

    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?

     
  • x-flow

    x-flow - 2009-12-07

    Hi,

    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.

     
  • x-flow

    x-flow - 2009-12-07

    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.

     
  • pajofego

    pajofego - 2009-12-07

    Hi

    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,
    pajofego

     

Log in to post a comment.

Get latest updates about Open Source Projects, Conferences and News.

Sign up for the SourceForge newsletter:

JavaScript is required for this form.





No, thanks