p_rgh with chtMultiRegionFoam
5 Attachment(s)
Hello,
I want do simulate the cooling prozess of a hot sphere (500K) in a cylindrical air-flow.(pictures) Attachment 29065 Iam not sure which boundary conditions for p and p_rgh I should choose. I added the files for p and p_rgh. The pressure p at the inlet is lower than at the outlet. Can anyone explain this pressure distribution? (pictures) Thanks in advance Andreas |
A few questions:
What is the boundary "fluidwall" and why is the type empty? Normally this means that you are doing a 2D simulation. What is the temperature and density of the fluid behind (downstream of) the sphere? It's probably lower so the velocity becomes higher. Now I am not really sure what kind of pressure (total/static/...) OpenFOAM is saving. Perhaps the higher pressure is a result of the increased velocity at the outlet compared to the inlet? Quote:
|
1 Attachment(s)
Quote:
Thanks for the quick reply. fluidwall is not the wall of the cylindrical channel. This is just an empty boundary which comes from snappyHexMesh. It is a real 3D Simulation. The wall of the channel has the name fluidWall_region0. Here is a picture of the velocity:Attachment 29072 |
The velocities at the outlet do not look physically correct. Just an idea: Try the mean value boundary condition for the pressure outlet:
http://www.cfd-online.com/Forums/ope...condition.html Or you have to extend the dimension of your cylinder much longer in the downstream direction so you get a homogeneous velocity distribution. |
Quote:
|
Just replace the "fixedValue" boundary condition for outlet in p and p_rgh by fixedMeanValue. Add meanValue 100000 (and keep the value).
(Of course you have to add the compiled library for the new boundary condition to your controlDict as described in the above referenced thread). |
The link in the thread about this topic does not open. Is there another source where I can get the library?
|
You could use the version in this message:
http://www.cfd-online.com/Forums/ope...tml#post418371 or try my modifications: http://www.cfd-online.com/Forums/ope...tml#post477560 |
Quote:
In the thread it is said, that the files can be compiled in the personal foam directory. Is this the OpenFOAM/ubuntu-2.2.1/run directory or the opt/openfoam221 directory? |
Actually you can unpack the archive in any directory you have write permission. I would recommend something like $HOME/OpenFOAM/ubuntu-2.2.1/application. Then step into this directory and issue the command
Code:
wmake libso Code:
libs ( "libfixedMeanValue.so"); Quote:
|
Thank you very much for your reply. It was very helpful.
The simulation is no running with "fixedMeanValue". I´m looking forward for the results. |
2 Attachment(s)
Quote:
I have the first results of the simulation with fixedMeanValue BC for p and p_rgh. The pressure distribution is the same as you can see in the pictures from the first post. The velocity field looks much better now: Attachment 29145 I also added the BC for the velocity. Maybe you can have a look at it. Attachment 29146 |
I think the U boundary conditions are ok. Could you scale the velocities on the two pictures (of the old and new simulation) with the same range. Especially in the second image it looks like the velocity next to the sphere is the same as up- and downstream (which does not make sense).
|
1 Attachment(s)
Quote:
Attachment 29147 The overall velocity in this second picture is lower than in the old picture (old simulation) because I have reduced the massflow. |
The new picture looks ok. Do you have experimental data to compare with (e.g. the temperature distribution, heat transfer coefficients,...)?
Quote:
|
For this model I have no experimental data to compare with. I want to compare the results with ansys cfx. Maybe there will be a experiment with a real pebble bed to compare with in a few months.
|
All times are GMT -4. The time now is 23:48. |