[riesotto]

Hi all,

how can I change the velocity at the inlet during a calculation. For better convergence I want to start up my simulation with a low velocity value and after some iterations change it to a higher value. Is there an easy way to do this????

kind regards
Florian

[nimasam]

yep there is,
look at groovyBC or swak4foam

[riesotto]

Hi nimasam,
thx for your reply. I will check this options...
kind regards
Florian

[philippose]

Hi,

I guess the easiest solution would be to use something like the "timeVaryingUniformFixedValue" boundary condition available in the native OpenFOAM distribution.

In your particular case, you can use this boundary condition to create a ramp of the inlet velocity to stabilize the initial part of the run.

Just search for the boundary condition in the forums for more details

Philippose

[riesotto]

Hi Philippose,

thx for your hint. It works fine with "timeVaryingUniformFixedValue".

Here for all who are intrested:
- first I wrote a file called rampe.dat, that is located in the main folder (the folder with /0, /constant, /system). This file contains:
(
(0.0 (-0.75 0.0 0.0))
(25.0 (-3.79 0.0 0.0))
(50.0 (-7.58 0.0 0.0))
(75.0 (-13.64 0.0 0.0))
)

here the first number (0.0 , 25.0 ...) is the time of the simulation and the following three numbers is the vector of the velocity (-0.75 0.0 0.0).

- Then I modified the boundary condition for the velocity (U):
...
inlet
{
type timeVaryingUniformFixedValue;
filename "rampe.dat"
value uniform (0 0 0);
outOfBounds clamp;
}

here outOfBounds means that after the endtime (75.0) the last value (-13.64 0.0 0.0) is retained.

- At the end I started the simulation and it works



Now I have a new Problem. Is it possible to change the value of omega in the MRFZones with this or any other method?????

kind regards,
Florian