Boundary condition with velocity profile
I have to model a rotor in a large tank. What my approach is, is that I first model the rotor in small rotating frame, and than I want to use the velocity obtained at a surface around the rotor as boundary condition for further analysis.
For this I make the assumption that the behavior in the tank does not influence the velocity field just around the rotor, which assumption is met 'good enough'.
How can I use the velocity field obtained from a certain simulation as bc in another one? And is it also possible to do this when the mesh doesn't correspond between the two analyses? And is it also possible to apply also turbulence intensity, pressure and whatever more together with a velocity field?
This is pretty easy in Fluent (as long as your simulation is steady state):
You need to export a "profile" in your first simulation and import it to the other one.
After simulting go to: file->write->profile
You can select the desired surface and values to export. Normally, I just export all values of my outlet.
In you second simulation go to file->read->profile.
Bear in mind that fluent interpolates the values from the absolute coordinates. Thus, if your outlet from simulation 1) lies at position y=1m and your inlet from simulation 2) lies at position y=0m you need to tell that fluent. I think the form is self-explanatory. Just ask, if you have questions.
Thank you for the answer.
The only problem is that I don't get any form when I read the profile. I need to rotate and translate my results, but I can't find how to do this. Can you explain a little bit more about this procedure?
Additionally: I read the profile to a mesh where the surface of the profile is not available. Does that matter? Or does it just force all quantities, even without the surface?
Thanks in advance,
You need to go to Boundary Conditions->Profiles->Orient...
Here you can use a translational ("Direction Vector") and rotational ("Rotation Matrix [RM]") transformation. I think I found help in the fluent manual. If I recall corectly, this is a bit cumbersome. You need to translate every single value you want to use.
"...Additionally...". I don't think I understand what you mean. You can only set these profiles value as boundary conditions to an existing surface, as far as I know.
Thank you Rodriguez, that was helpful! I managed to define the RM and TM correctly now.
Forget the second point. Now I used the velocity profiles as boundary condition at a surface.
My idea behind the question was to avoid the use of boundaries, because fluent uses a lower order scheme at boundaries. I thought it would maybe be possible to force velocities at a certain location in a fluid domain using profiles, even when at that specific location no surface is present. But this is not possible, since the profiles are interpolated based
I still try to do so, but now though defining a new fluid domain at the location of the rotor, and in that domain I want to apply a source of momentum.
|All times are GMT -4. The time now is 01:41.|