# Restart slolution doesn't work

 Register Blogs Members List Search Today's Posts Mark Forums Read

August 29, 2013, 17:29
Restart slolution doesn't work
#1
Member

Jianming Liu
Join Date: Mar 2009
Location: China
Posts: 66
Rep Power: 9
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.
Attached Files
 naca0012.txt (12.9 KB, 6 views)

 September 2, 2013, 11:49 #2 Member   Jianming Liu Join Date: Mar 2009 Location: China Posts: 66 Rep Power: 9 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.

 September 2, 2013, 21:07 #3 Member   Eduardo Molina Join Date: Sep 2010 Location: Brazil Posts: 35 Rep Power: 7 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

September 7, 2013, 07:20
#4
Member

Jianming Liu
Join Date: Mar 2009
Location: China
Posts: 66
Rep Power: 9
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

HTML Code:
    if (dual_time) {
int Unst_RestartIter;
Unst_RestartIter = int(config->GetUnst_RestartIter())-1;
else
Unst_RestartIter = int(config->GetUnst_RestartIter())-2;
}

Quote:
 Originally Posted by EMolina 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

 September 12, 2013, 03:36 #5 Super Moderator   Thomas D. Economon Join Date: Jan 2013 Location: Stanford, CA Posts: 269 Rep Power: 6 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

 February 4, 2014, 00:45 #6 Member   Anant Diwakar Join Date: Jan 2013 Posts: 68 Rep Power: 5 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

 February 5, 2014, 18:19 #7 Super Moderator   Thomas D. Economon Join Date: Jan 2013 Location: Stanford, CA Posts: 269 Rep Power: 6 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Armen A. Ghirghidov FLOW-3D 5 December 10, 2008 10:24 V. Kumar CFX 3 July 20, 2006 13:23 Alumna Phoenics 6 June 22, 2004 12:08 green Phoenics 2 May 27, 2004 21:03 Dmitry CD-adapco 1 March 27, 2002 11:26

All times are GMT -4. The time now is 21:02.