|
[Sponsors] |
How do set a steady solution as an initial solution to an unsteady simulation? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 18, 2020, 06:39 |
How do set a steady solution as an initial solution to an unsteady simulation?
|
#1 |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
In the study of the aeroelastic Isogai Case A such as in this paper,
https://kiwi.oden.utexas.edu/papers/...es-Willcox.pdf It states that, using SU2, they first initialized a steady state solution for an unsteady simulation. How do i go about in doing this (in general)? Do i need to make 2 configuration files, one that is for the initial steady and the other for the unsteady? I have tried this, and set the unsteady config file to restart from the steady config but it gives me an error, where it can't find the restart file. So i assume I can do this all in one config file? I have checked the tutorial on Unsteady NACA 0012, where i assume they first initialized a steady state solution. But attached in the picture is where i dont understand how they did the following. Attached is an example of my config file |
|
April 18, 2020, 10:31 |
|
#2 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
I don't think you can do it in one config file.
I would just rename and duplicate the steady restart according to the time-domain naming convention, and then start the unsteady simulation. Note that the first time steps of such an unsteady simulation are not useful, you still need to wait for transients to clear and for the simulation to start showing some kind of periodic behavior (starting from steady state hopefully makes this quicker...). Regarding the passage you highlighted, I think it is not referring to this restart process, they are explaining the dual time-stepping strategy in simple terms (i.e. what goes on inside the solver, it is not something accessible from the user side). |
|
April 18, 2020, 10:53 |
|
#3 |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
Hi, I have renamed my steady state solutions (restart_flow) to solution_flow_00000. Running this would give me an error of 'negative iterator etc.' I mean i understand the DUAL_TIME stepping strategy would require 2 solution flows, I dont understand how i can create 2 steady state solutions (meaning i dont understand the logic behind this). So what i did was i copy pasted the solution_flow_00000.dat file and renamed it to solution_flow_00001.dat. I still get the error of a 'negative iterator'.
Ive attached my steady config file, hopefully you can help me out here. Moreover, on the topic of the typical section model, I would like to ask. Is there anyway i can define the x position of the elastic axis in SU2? Based on the template only the Xcg is written. Would the Elastic axis location be defined by the SU2 variable REF_ORIGIN_MOMENT_X? (for a typical section) % Distance in semichords by which the center of gravity lies behind % the elastic axis CG_LOCATION= -0.2 If i can verify, does the CG_LOCATION defined above coincide with the attached picture? |
|
April 18, 2020, 11:23 |
|
#4 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
You need to set RESTART_ITER=2 (1 more than your last restart)
I cannot help with the aeroelastic features, I never used them. |
|
April 20, 2020, 09:05 |
|
#5 | |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
Quote:
Referring to my attachment, would that mean removing the time history up to the blue line? |
||
April 20, 2020, 12:14 |
|
#6 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
A lot more than that, the characteristic time (period) seems to be around 0.08s, I would disregard around 10 periods, after which maybe you start seeing a clearly repeating cycle (same peak to peak amplitude, same average, etc.).
That is assuming what you are studying is periodic. If you want to study a short transient that is not periodic, e.g. a quick movement of a control surface, you still need an "unsteady initialization", the gist of it is, until the initial particles (from a steady state of freestream initialization) leave the domain the results are not good. |
|
April 26, 2020, 09:15 |
|
#7 | |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
Quote:
|
||
April 26, 2020, 19:23 |
|
#8 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
You have a moving grid problem, you are probably missing the grid velocities when you restart (similar to this problem Restart causes FGMRES orthogonalization failed).
Try using RESTART_STEADY_STATE= YES and be sure to use v7.0.3. |
|
April 27, 2020, 12:54 |
|
#9 | |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
Quote:
Ran the SAME steady state case TWICE and renamed each restart_flow file to solution_flow_00000 and solution_flow_00001, twice because my unsteady simulation is in DUAL_TIME. I wonder if this is actually a correct procedure? |
||
April 28, 2020, 16:24 |
|
#10 |
Senior Member
Pedro Gomes
Join Date: Dec 2017
Posts: 466
Rep Power: 13 |
I played around with your case and I think there is a bug somewhere preventing aeroelastic restarts from steady state. Likely because the grid velocities are not in steady restart files.
I'll investigate this a bit but for now the conclusion is there is a bug. On another note your case will run much faster if you use ILU as the preconditioner for deformation (for the reasons explained here https://su2code.github.io/docs_v7/Li...econditioners/) |
|
April 28, 2020, 18:05 |
|
#11 | |
New Member
pro
Join Date: Mar 2020
Posts: 25
Rep Power: 6 |
Quote:
|
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" | bigphil | OpenFOAM CC Toolkits for Fluid-Structure Interaction | 686 | December 22, 2022 10:10 |
pressure in incompressible solvers e.g. simpleFoam | chrizzl | OpenFOAM Running, Solving & CFD | 13 | March 28, 2017 06:49 |
Cannot run the code properly: very large time step continuity error | crst15 | OpenFOAM Running, Solving & CFD | 9 | December 14, 2014 19:17 |
Moving mesh | Niklas Wikstrom (Wikstrom) | OpenFOAM Running, Solving & CFD | 122 | June 15, 2014 07:20 |
pimpleFoam: turbulence->correct(); is not executed when using residualControl | hfs | OpenFOAM Running, Solving & CFD | 3 | October 29, 2013 09:35 |