[sahmed]

Dear all
I have a question, which might be helpful for others as well. Could anyone please tell me how can I restart a simulation in a solver using the results from a different solver. I know I can do that using latestTime option of the controlDict, but that is if I want to restart using the same solver. But if I want to use the restarting criteria (results) from another solver, how can I do that.

For example, suppose pisoFoam gives me a simulation results and I want to use those results as my starting criteria for simulation using another solver- icoFoam (I am just making up solver names).

Any of your helpful suggestion or comment will be highly appreciated and helpful for the community.
Thanks

~Sheikh Ahmed

[Flowkersma]

Dear Sheikh Ahmed,

If you are using the same mesh with the new simulation, you can simply copy the latest time step folder to the new case folder where you are using the new solver. You may also rename the folder to 0. If you are not using the same mesh, then you can use mapFields utility to interpolate the solution from the old case to the new case.

Best,
Mikko

[HenningW]

Hi,

you can work with flowkersma's solution. But -latestTime should work as well, I use it all the time.

I know I can do that using latestTime option of the controlDict, but that is if I want to restart using the same solver.

Do you get an error, when you try a different solver? Probably you need to add additional boundary conditions? But that would apply for the copied files as well.

As a third option you could also run

mapFields -parallelSource -parallelTarget -sourceTime latestTime  /folder/of/your/old/simulation

(Dont forget to create a mapDieldsDict)

[sahmed]

Thank you very much Flowkersma and Mikko for your prompt replies. According to your suggestions, I copied the U file of the latest time to the new solver's time folder and could run without error. I couldnt copy the whole 'time folder' since my older solver solves only P and U, whereas my new solver solves P, T, U etc. Also, the units of P were different (P/rho in pisoFoam and P in laminarSMOKE) and thats why I couldnt copy P as well.
Any idea or suggestion regarding the process I am using?

I dont need the mapFieldsDict right now since I am using identical mesh sizes, but I have to use that for my future runs for sure.

Thanks once again and please share if you have any new thoughts.

~SFA

[sahmed]

I am sorry, thanks to Mikko and HenningW

[Flowkersma]

I think that is fine what you are doing but note that the meshes have to be exactly same between the two cases. Probably, that is the case for you because you did not get any errors regarding that. If you want to use the P from incompressible case, you can change the unit and calculate the absolute pressure for compressible solver with foamCalc.

[sahmed]

Thanks Mikko. Could you tell me the foamCalc command to convert phi to p as you mentioned.

[Flowkersma]

You probably mean how to convert the pressure (p/rho) from the incompressible solver to the compressible solver. If that's the case, the syntax for foamCalc should be something like

foamCalc scalarMult p -value 1.2 -resultName p
foamCalc addSubtract p add -value 100000 -resultName p

where 1.2 is the density and 100000 is the atmospheric pressure (i.e. if you were using pressure=0 at the outlet for incompressible solver). Finally, you'll have to modify the dimension line in p file from

dimensions      [0 2 -2 0 0 0 0];

to

dimensions      [1 -1 -2 0 0 0 0];

In OF4 you should use postProcess utility but I don't know how it works.

[Carlo_P]

Hey Flowkersma,
now seems that the foamCalco doen't work, with OpenFOAM 6.


Now one should use postProcess utilities.
Do you have any idea how to convert your string?


Thanks a lot,
Carlo