CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

How to initialise simulation with solution from previous simulation?

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 18, 2024, 09:08
Default How to initialise simulation with solution from previous simulation?
  #1
New Member
 
Tommy Nee
Join Date: Sep 2023
Posts: 11
Rep Power: 2
tnee3 is on a distinguished road
Hi!

I'm relatively new to OpenFOAM and I'm looking to initialise a simpleFoam simulation around an aerofoil using the kOmegaSST model with the solution I obtained from running the same simulation with the Spalart-Allmaras model, as was recommended on this blog post here to overcome some of the issues with the kOmegaSST model.

My question is simply how do I go about this. I know to change the startFrom in the controlDict to latestTime, then I'm guessing I copy in the k and omega fields to the latest time folder as these values are not calculated by the Spalart-Allmaras model. However when I tried all of this, the model's residuals just continued on a straight line and nothing seemed to change. I think I need to change something with the convergence criteria but I'm not sure what to change.

Any help on this would be greatly appreciated! I understand this is probably a fairly simple question but I can't seem to find any steps on exactly what to change to perform this.

Thanks!
tnee3 is offline   Reply With Quote

Old   February 19, 2024, 13:37
Default
  #2
Member
 
Shravan
Join Date: Mar 2017
Posts: 63
Rep Power: 9
Severus is on a distinguished road
Hello,
If you would like to continue with calculated values of k and omega fields, then you can use the following functionObject.
https://www.openfoam.com/documentati...8H_source.html
You can output the fields and then start your simulation (with start from latestTime) but with kOmegaSST. This may help

Thanks
Severus is offline   Reply With Quote

Old   February 20, 2024, 05:41
Default
  #3
New Member
 
Tommy Nee
Join Date: Sep 2023
Posts: 11
Rep Power: 2
tnee3 is on a distinguished road
Hi, thanks for replying! It's more for me that I don't really know how to set up the new case with the kOmegaSST model implemented. By this i mean do I create a new case folder and use mapFields to transfer the U,p and nut fields so that they can be used as the new initial conditions for the kOmegaSST run, or do I just replace the turbulence model, alter the convergence criteria (in some way, I wouldn't be sure how) and change the strartFrom to latestTime within the same case folder. I'm sorry, I know this is probably quite a basic question but I'm struggling with it at the moment.
Thanks!
tnee3 is offline   Reply With Quote

Old   February 20, 2024, 14:09
Default
  #4
Member
 
Shravan
Join Date: Mar 2017
Posts: 63
Rep Power: 9
Severus is on a distinguished road
Hi,
I think you can do either ways.
Make sure you have made the following changes:
1) Have the necessary fields in the latestTime folder (for instance in your case additionally k and omega). Note – you should use the correct (physical) values. For example as I mentioned you can try to calculate the other needed turbulent quantities using the turbulenceFields functionObject. Also, use appropriate/correct BC so that the simulation doesn’t crash

2) Add the required linear solver properties and schemes to new variables (k and omega) in fvSolutions file and fvSchemes files respectively

3) An easy way to check if your case is okay is to take a tutorial where kOmegaSST is used and try to be consistent in all your case files with that tutorial

4) startFrom latestTime with the new turbulence model (changed)

Regarding using turbulenceFields
In case you use OpenFOAM foundation versions, the turbulenceFields cannot give you omega (because turbulenceFields needs k and epsilon to calculate omega).
(See from line 76)
https://cpp.openfoam.org/v9/turbulen...8C_source.html

Also see this post: Issue about values of omega, k using SpalarAllmaras
You have it in the ESI version of OpenFOAM (v2106). So one way will be to move to using the ESI version. If you don’t want to move from Foundation to ESI, you can try to use k epsilon model instead of SpalartAllmaras first and then change to kOmegaSST (but I do not know if you prefer that)

Regarding residuals and convergence after changing your turbulence model
If you have problems with convergence if you change the turbulence model, I would suggest start with 1st order schemes (e.g. Euler for time and upwind schemes), play with outer/inner correctors, play with underrelaxation factors (for steady cases) and after the residuals stabilize you can slowly change them to the original ones desired. Also, try reducing your time step size or reduce maximum Courant number (with "adjustTimeStep on;")

Note if you want to change any of the files when the solver is running and if you want to OpenFOAM to read it immediately (while running), choose
HTML Code:
runTimeModifiable yes;
Good luck!
Severus is offline   Reply With Quote

Old   February 21, 2024, 13:12
Default
  #5
New Member
 
Tommy Nee
Join Date: Sep 2023
Posts: 11
Rep Power: 2
tnee3 is on a distinguished road
Hi!

Thanks very much for your very in depth reply, I will be sure to try all the above methods. I have a kOmegaSST model running okay-ish now but I'd imagine some of these will definitely improve it.

Thanks again!
tnee3 is offline   Reply With Quote

Reply

Tags
initialization, komegasst, simplefoam, turbulence models

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Unsteady Simulation from steady Solution hussein93 Main CFD Forum 2 February 8, 2024 07:49
Simulation beginning from initialized solution rather than restart file eskimmel SU2 2 June 19, 2023 10:03
Time-accurate solution restart from steady state solution jyotir SU2 6 December 8, 2021 08:34
Not getting converged solution in transient simulation Julian121 CFX 6 April 27, 2019 02:00
How can I use solution from one simulation as initial condition on a remote solver? Dano62 CFX 0 October 21, 2015 17:45


All times are GMT -4. The time now is 07:10.