CFD Online Discussion Forums - Restart slolution doesn't work

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- SU2 (https://www.cfd-online.com/Forums/su2/)

- - Restart slolution doesn't work (https://www.cfd-online.com/Forums/su2/122861-restart-slolution-doesnt-work.html)

Restart slolution doesn't work

Dear developer,
I use the newest version of SU2 on the github. But I find a problem, the restart solution process doesn't work, and show :

Requesting a negative iteration number for the restart file!!
Press any key to exit...

the configure file is attached.

Many thanks.

Dear,
I have found the problem, for unsteady computation, I should set the value of UNST_RESTART_ITER in the configure file. If set UNST_RESTART_ITER=1, and SOLUTION_FLOW_FILENAME= solution_flow.dat, then there should be a restart file: solution_flow_00000.dat in the work directory.

In my case, I want to simulation the oscillating airfoil with the specified moving (\alpha=\alpha_0+\delta\alpha\sin(\omega t)). I want to use the converged result at the mean AoA=\alpha_0 as the restart data, then perform the oscillating moving of the airfoil. Now the output restart file of the computation of the static airfoil do not include the date of "Grid_Velx", "Grid_Vely", in this case they should be zero. So I must add it to as the restart file of the unsteady computation. Could you please tell me if there is other method?

Thank you.

Hi all.

I am facing the same problem of liujmljm, I was doing a pure dual time step unsteady simulation with Su2, but after I pull the newest version of SU2 available on Github I cannot restart my simulations anymore. I tried put on the configure file the UNST_RESTART_ITER=1 option to read the solution_flow_00000.dat like liujmljm said but the 'Requesting a negative iteration number for the restart file!!' error persists.

Can someone clarify this new option on SU2?

Thanks in advance

Based on the definition of CEulerSolver::CEulerSolver(CGeometry *geometry, CConfig *config, unsigned short iMesh) in the file solver_direct_mean.cpp.

As the setting by above description, UNSTEADY_SIMULATION should be set as DUAL_TIME_STEPPING-1ST_ORDER. If it is DUAL_TIME_STEPPING-2ST_ORDER, I think
UNST_RESTART_ITER might be equal to 2, and su2 will
read the solution_flow_00000.dat

HTML Code:

    if (dual_time) {

      int Unst_RestartIter;

      if (config->GetUnsteady_Simulation() == DT_STEPPING_1ST)

        Unst_RestartIter = int(config->GetUnst_RestartIter())-1;

      else

        Unst_RestartIter = int(config->GetUnst_RestartIter())-2;

      filename = config->GetUnsteady_FileName(filename, Unst_RestartIter);

    }

Quote:

Originally Posted by EMolina (Post 449455)

Hi guys,

Thrilled to hear that you are using the most recent version of the code for unsteady flows with dynamic meshes! Good news: we are overhauling this section of the code to make it easier to use and more capable for the V3.0 release. Unfortunately, that means that some of the config options and capabilities are being modified slightly (and may change more in the near future while we get everything settled).

The current version of the code works as expressed above in the post by Jianming (as of 09.11.2013). Use the new option UNST_RESTART_ITER to choose the iteration number that you would like to restart a simulation from (this is the iteration number appended to the files). Note that for 1st-order dual time, a single restart file is required (iter-1), but for 2nd-order, two previous time levels are required for a proper restart.

Lastly, we will soon be adding a separate option for starting an unsteady flow from a converged, steady solution without needing to worry about the iteration numbers, etc. Stay tuned for this in the near future.

Hope this helps, and thanks for using SU2,
Tom

Hi

I am trying to restart an unsteady NACA0012 airfoil simulation
from a steady state restart file.

How can I run Dual time stepping (2nd order) as there is single restart file
obtained from steady state simulation ?

Thanks
Anant

Hi Anant,

An unsteady restart could be performed by copying the steady restart file to two files named solution_flow_00000.dat and solution_flow_00001.dat and then choosing the following options in the config file:

% Restart solution (NO, YES)
RESTART_SOL= YES

% Iteration from which to restart the unsteady calc
UNST_RESTART_ITER= 2

% Restart flow input file
SOLUTION_FLOW_FILENAME= solution_flow.dat

It should load in the two identical files as the solution at the two previous time levels and start the calculation on iteration 2.

Hope this helps,
Tom