[achuneka]

My case is Flow through a Venturi and I am using lesCavitatingFoam. BC - Velocity inlet and uniform pressure outlet.

I would like to run the case for a higher value of outlet pressure to get initial set of field values.

I then want to reduce the outflow pressure and continue running it further. I am running the job in parallel.

The problem is the modification of boundary conditions in the time files formed.

Please let me know

[mattijs]

- Stop the simulation and edit the last time dump (in all the processor directories). Set startTime to latestTime and restart

- Or use one of timeVaryingUniformFixedValue or timeVaryingMappedFixedValue to automatically vary a fixedValue b.c. (search this forum - see simpleFoam/pitzDailyExptInlet tutorial)

[achuneka]

Thanks Mattijs.

The problem in doing that is this.

The BC for pressure in a "non-decomposed" file looks like this.

outflow
{
type fixedValue;
value uniform 2e5;
}

When I decompose the file into n number of processors, on each processor the file looks like

outflow
{
type fixedValue;
value nonuniform 0();
}

Followed by a list of faces which actually have the same value 2e5.

Same thing applies in the boundary section of dumped time files.

So now if I have to modify these files, I have to
change each of them. Is there any other way to do that ?

[olesen]

Did you try with 'reconstructPar', edit the boundary files, 'decomposePar -fields' and then restart?

Or else, if you use the time-varying boundary condition like Mattijs mentioned, you can do a restart without needing to edit the field values themselves. The new value will get taken from the file.

[achuneka]

Thanks Mark... reconstructPar works ..

[miotto]

I posted a possible way to do this here:
Restarting simulations in openfoam with updated boundary conditions