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

buoyantSimpleFoam and watertank

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

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 14, 2014, 15:28
Default
  #41
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 4
BernhardS is on a distinguished road
Unfortunately I do not get beyond 0.07 seconds before the pressure blows up. If have attached the new version with the modified Allrun script. Switching off the turbulence does not make any difference...
Attached Files
File Type: gz ts_v1.gz (38.2 KB, 2 views)
BernhardS is offline   Reply With Quote

Old   January 15, 2014, 11:32
Default
  #42
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 4
BernhardS is on a distinguished road
I am able to run that case if I change the BCs for p_rgh for bottom and wall to buoyantPressure and the one for top to fixedValue. Additionally I use funkySetField to initialize p. I have to use a lot of outerCorrectors (~30) at the beginning and underrelaxation, especially for p_rgh.

The velocity profile at the wall, due to the heat loss, is not as distinctive as before with buoyantBoussinesqPimpleFoam (see post #36). While the velocity profile is well developed in the lower region (after 360 sec), there are some disturbances in upper region probably caused by the BC for the top face.
UY.jpg T1.jpgThot.jpg Tcold.jpg
At least the temperature distribution is stable and quite uniform in radial direction (except at the outer wall with the heat flux) which was previously not the case.

Does anyone have an idea which BCs might be as well appropiate for a closed tank?
Even though the case is running with the current BCs, it is probably a wrong setup since there is still some velocity (see Fig. 2, UY) at the top face where it should actually be zero...
BernhardS is offline   Reply With Quote

Old   January 15, 2014, 16:07
Default
  #43
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg (Bavaria, Germany) Leoben (Styria, Austria)
Posts: 845
Rep Power: 17
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bernhard,

I tryed several options.

- changing 0/ files
- changing initialization
- changing thermodynamicProperties (with air its working)

- test case with cht
- test case with buoyant
- test case with boussinesq

- testings with diverent meshes
- testings with several fvSolution options

- changing pEqn.H in buoyantPressure

- checking with laminar and turbulent flow characteristics

Summary:

- most simulations have a continuity problem (U_x,y,z) blow up and p_rgh too
- re-coarse the mesh did not solve the problem
- thermodynamics changing to perfectGas with air is working
- changing p_rgh (top) to fixedValue is working but the results are bad.

At the moment I am out of ideas - sorry.
Tobi is offline   Reply With Quote

Old   January 16, 2014, 04:13
Default
  #44
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 4
BernhardS is on a distinguished road
Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...
BernhardS is offline   Reply With Quote

Old   January 17, 2014, 07:18
Default
  #45
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg (Bavaria, Germany) Leoben (Styria, Austria)
Posts: 845
Rep Power: 17
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by BernhardS View Post
Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...
Additionally you can set g to (0 0 0)^T - it should give the same possibilty to solve the case but you need gravitation.
Tobi is offline   Reply With Quote

Old   March 3, 2014, 15:00
Default
  #46
nsf
Member
 
Nicolas Edh
Join Date: Mar 2010
Location: Uppsala, Sweden
Posts: 71
Rep Power: 6
nsf is on a distinguished road
Quote:
Originally Posted by jherb View Post
Add the following line to your thermophysicalProperties:
Code:
dpdt no;
see:

[/code]
Hi all,

I might have an explanation of why the solution diverges when the density is non-constant and dpdt is on. I am hoping for your comments.

By using icoPolynomial we are setting the fluid as incompressible, i.e. \rho(p,T) = \rho(T). So we have, by definition:

\frac{\partial\rho}{\partial p} = 0

Which is what icoPolynomial returns when the function psi is called. For an ideal gas \frac{1}{RT} is returned. The compressibility can be expanded to

\frac{\partial\rho}{\partial t} \frac{\partial t}{\partial p} = 0

or

\frac{\partial\rho}{\partial t}\left[ \frac{\partial p}{\partial t}\right]^{-1} =0

So if we have non constant density, \frac{\partial\rho}{\partial t} \ne 0 and hence \frac{\partial p}{\partial t} must diverge?

Perhaps we would need and compressiblePolynomial class where the compressibility can be set even though it's really small for water?

Any thoughts?

Cheers
Nicolas
nsf 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



All times are GMT -4. The time now is 01:11.