[kiddmax]

Dear all

I try to simulate an unsteady case with converged steady solution as initial value. So What I did is copy the steady case as a new unsteady case, and change corresponding parameters for unsteady calculations.
In the controlDict file, I set it like this:
------------------
startFrom latestTime;

startTime 0;

stopAt endTime;

endTime .5;

deltaT 1e-4;
-----------------------



When I run pimpleFoam, it says:


-----------------------
Create time

Create mesh for time = 10000

Reading field p

Reading field U

Reading/calculating face flux field phi

AMI: Creating addressing and weights between 3724 source faces and 3724 target faces
AMI: Patch source weights min/max/average = 1.00025, 1.00025, 1.00025
AMI: Patch target weights min/max/average = 1.00025, 1.00025, 1.00025
Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

No finite volume options present


PIMPLE: no residual control data found. Calculations will employ 2 corrector loops


Starting time loop

End
-------------

No time loop happens, any guys have an idea???

Best regards,
Ye

[alexeym]

Hi,

startFrom latestTime;

startTime 0;

stopAt endTime;

endTime .5;

your endTime is 0.5 s, but

Create time

Create mesh for time = 10000

your start time is 10000.

Why don't you use mapFields -sourceTime 10000 <steady-state-case-directory> for mapping steady state solution onto your transient simulation initial time?

[kiddmax]

I forgot to mention, that mapField does not work for me. It gives a lot warning and get stopped. I also have a thread about that.

[kiddmax]

Dear Alexey

Thank you for you reply. I got my steady state solution for 10000 iterative steps. And I both tried to set 'startTime 10000 or startTime 0', 'endTime 10000.5 or 0.5', since I want to have 0.5s transient simulation, but they do give the same output as I list.

The time loop just does not start. I do not know why...

Best regards,
Ye

[alexeym]

Hi,

by default mapFields uses

meshToMesh::interpolationMethod mapMethod =
    meshToMesh::imCellVolumeWeight;

maybe you can try other methods: direct or mapNearest and they will work? I.e. add -method option to mapFields invocation.

Also if you just copy results from steady state solution, there should be uniform subfolder (i.e. 10000/uniform) where OF stores information on time and time step. Maybe if you delete this subfolder it will do the loop?

[Bernhard]

Originally Posted by alexeym

Why don't you use mapFields -sourceTime 10000 <steady-state-case-directory> for mapping steady state solution onto your transient simulation initial time?

Because this is quite redundant if the mesh and the boundary conditions are the same. Just do something like

$ mv 0 0.org
$ cp -r ../steadyStateCase/0 .
$ rm -r 0/uniform

[kiddmax]

Dear all,

After deleting the file 10000/unform, it works well.

Thank you !

Ye

[kiddmax]

Dear Alexey,

I tried other mapping methods: mapNearest, interpolate and cellPointInterpolate. I always got the same warning. I did not find the direct method you mentioned. Probably this problem comes from the interface I have (Which I use cyclicAMI boudary condition)??

Best regards
Ye

[eaxyd1]

Hi Ye and all,
I tried to the method you mentioned, and it works for serial running, but I can't run in parallel, the error:

[dang-SVE14A2SGC:17212] [12] /opt/openfoam231/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZNK4Foam16cyclicAMIFvPatch11ma keWeightsERNS_5FieldIdEE+0x1d5) [0x7ff2692f1085]
[dang-SVE14A2SGC:17212] [13] /opt/openfoam231/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZNK4Foam20surfaceInterpolation 11makeWeightsEv+0x27e) [0x7ff2697889ce]
[dang-SVE14A2SGC:17212] [14] /opt/openfoam231/platforms/linux64GccDPOpt/lib/libfiniteVolume.so(_ZNK4Foam20surfaceInterpolation 7weightsEv+0x19) [0x7ff269788be9]
[dang-SVE14A2SGC:17212] [15] pisoFoam() [0x41a35b]
[dang-SVE14A2SGC:17212] [16] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf0) [0x7ff266f28a40]
[dang-SVE14A2SGC:17212] [17] pisoFoam() [0x41c82b]
[dang-SVE14A2SGC:17212] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 1 with PID 17210 on node dang-SVE14A2SGC exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------

How do you solve in parallel?
Thanks a lot!
Sophie