CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

p_rgh with chtMultiRegionFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2014, 02:07
Default p_rgh with chtMultiRegionFoam
  #1
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Hello,

I want do simulate the cooling prozess of a hot sphere (500K) in a cylindrical air-flow.(pictures) ModellEinzelkugel.pdf

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
Attached Images
File Type: jpg p_rgh.jpg (18.8 KB, 17 views)
File Type: jpg p.jpg (19.3 KB, 16 views)
Attached Files
File Type: txt p.txt (1.4 KB, 11 views)
File Type: txt p_rgh.txt (1.4 KB, 11 views)
styx is offline   Reply With Quote

Old   March 4, 2014, 05:01
Default
  #2
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
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:
Originally Posted by styx View Post
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
jherb is offline   Reply With Quote

Old   March 4, 2014, 06:11
Default
  #3
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Quote:
Originally Posted by jherb View Post
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?

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:u.jpg
styx is offline   Reply With Quote

Old   March 4, 2014, 06:25
Default
  #4
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
The velocities at the outlet do not look physically correct. Just an idea: Try the mean value boundary condition for the pressure outlet:
Pressure outlet boundary condition
Or you have to extend the dimension of your cylinder much longer in the downstream direction so you get a homogeneous velocity distribution.
jherb is offline   Reply With Quote

Old   March 4, 2014, 06:50
Default
  #5
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Quote:
Originally Posted by jherb View Post
The velocities at the outlet do not look physically correct. Just an idea: Try the mean value boundary condition for the pressure outlet:
Pressure outlet boundary condition
Or you have to extend the dimension of your cylinder much longer in the downstream direction so you get a homogeneous velocity distribution.
I would prefer to try the "fixedMeanValue" boundary. I the thread from obove, the meanValue is 3.3. What does this Value say? Can I try a value of the same order?
styx is offline   Reply With Quote

Old   March 4, 2014, 07:11
Default
  #6
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
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).
jherb is offline   Reply With Quote

Old   March 4, 2014, 07:55
Default
  #7
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
The link in the thread about this topic does not open. Is there another source where I can get the library?
styx is offline   Reply With Quote

Old   March 4, 2014, 08:47
Default
  #8
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
You could use the version in this message:
Pressure outlet boundary condition
or try my modifications:
Pressure outlet boundary condition
jherb is offline   Reply With Quote

Old   March 5, 2014, 02:30
Default
  #9
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Quote:
Originally Posted by jherb View Post
You could use the version in this message:
Pressure outlet boundary condition
or try my modifications:
Pressure outlet boundary condition
Iam sorry to ask you again. Im trying to install the library described in the first link. Im not sure in which folder I have to copy the files. I is the first time I add any sources to my openfoam installation.

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?
styx is offline   Reply With Quote

Old   March 5, 2014, 07:22
Default
  #10
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
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
(actually starting with OpenFOAM 2.2.2 wmake alone is enough). This should install a shared library in your directory $FOAM_USER_LIBBIN. If you add the new library to your controlDict, like
Code:
libs ( "libfixedMeanValue.so");
OpenFOAM should find it automatically.

Quote:
Originally Posted by styx View Post
Iam sorry to ask you again. Im trying to install the library described in the first link. Im not sure in which folder I have to copy the files. I is the first time I add any sources to my openfoam installation.

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?
jherb is offline   Reply With Quote

Old   March 5, 2014, 08:15
Default
  #11
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Thank you very much for your reply. It was very helpful.
The simulation is no running with "fixedMeanValue".
Im looking forward for the results.
styx is offline   Reply With Quote

Old   March 5, 2014, 10:57
Default
  #12
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Quote:
Originally Posted by jherb View Post
The velocities at the outlet do not look physically correct. Just an idea: Try the mean value boundary condition for the pressure outlet:
Pressure outlet boundary condition
Or you have to extend the dimension of your cylinder much longer in the downstream direction so you get a homogeneous velocity distribution.

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: U-fixedMeanPressure.jpg

I also added the BC for the velocity. Maybe you can have a look at it. U.txt
styx is offline   Reply With Quote

Old   March 5, 2014, 11:14
Default
  #13
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
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).
jherb is offline   Reply With Quote

Old   March 5, 2014, 11:29
Default
  #14
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
Quote:
Originally Posted by jherb View Post
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).
Here is the rescaled velocity field. Gravity is not activated in both cases.
U-fixedMeanPressure2.jpg

The overall velocity in this second picture is lower than in the old picture (old simulation) because I have reduced the massflow.
styx is offline   Reply With Quote

Old   March 5, 2014, 16:53
Default
  #15
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 206
Rep Power: 9
jherb is on a distinguished road
The new picture looks ok. Do you have experimental data to compare with (e.g. the temperature distribution, heat transfer coefficients,...)?

Quote:
Originally Posted by styx View Post
Here is the rescaled velocity field. Gravity is not activated in both cases.
Attachment 29147

The overall velocity in this second picture is lower than in the old picture (old simulation) because I have reduced the massflow.
jherb is offline   Reply With Quote

Old   March 6, 2014, 01:28
Default
  #16
New Member
 
ande
Join Date: Oct 2013
Posts: 18
Rep Power: 3
styx is on a distinguished road
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.
styx is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Error in thermophysical properties (chtMultiRegionFoam) mukut OpenFOAM Pre-Processing 17 September 3, 2014 07:54
Custom boundary condition: unexpected behavior with chtMultiRegionFoam leroyv OpenFOAM Programming & Development 3 February 1, 2014 07:49
Error in chtMultiRegionFoam kirankarki OpenFOAM 5 October 24, 2012 17:20
Embed explicitSetValue in chtMultiRegionFoam samiam1000 OpenFOAM 2 April 18, 2012 05:14
chtmultiregionFoam alvora OpenFOAM 9 February 23, 2011 03:06


All times are GMT -4. The time now is 12:08.