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

Forces for a sloshing case

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 8, 2007, 13:22
Default Dear all, I have the follow
  #1
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
Dear all,

I have the following problem which I would also like to present at the OpenFOAM conference in November:

A satellite tank is filled to about 50% and the liquid is all gathered at the bottom of the tank (spherical tank with a cylindrical section in the middle), although there is no acceleration acting on the liquid. At t=0s the system is accelerated downwards and hence the liquid will start to move upwards. At t=15s the acceleration stops and the whole system is left in a zero gravity condition again. I would like to extract the forces acting on the tank in order to compare them with actual flight data (Sloshsat FLEVO). Unfortunately I have no idea how to treat the pressure, since the pressure used in interFoam does not contain hydrostatic pressure, as far as I understood it. I have been scanning the forum forwards and backwards but haven't found anything. I'd be happy if someone could point me in the right direction.

Oliver
ogloth is offline   Reply With Quote

Old   October 10, 2007, 03:13
Default I guess my posts must be reall
  #2
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
I guess my posts must be really stupid, since they seem to never get answered. Well - I am fully aware that OpenFOAM is open-source and that all replies and support is voluntarily and that of course nobody has any right to his or her problems being answered. Still, I was hoping to get some support, especially since I am actually trying to validate OpenFOAM against some experimental data.

Anyway, I have implemented a dirty workaround: I simply take the highest point of liquid and set the hydrostatic pressure to zero at that level. All other cells (and boundary faces) get a hydrostatic pressure according to the y-difference to that highest cell. Obviously this will be wrong for isolated regions of liquid.

Somebody must have a similar problem I would assume!

Oliver
ogloth is offline   Reply With Quote

Old   October 10, 2007, 07:14
Default Hi Oliver! This might, or m
  #3
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,912
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Oliver!

This might, or might not help you. In Hrv's dev version there is an utility applications/utilities/postProcessing/stressField/interFoamPressure/ that calculates the static pressure from interFoam-results.

I just stumbled on it. I never tried it. I didn't have too close a look at it. You're on your own from here on, I'm afraid.

Bernhard

PS: Just get it with
svn checkout https://openfoam-extend.svn.sourceforge.net/svnroot/openfoam-extend/trunk/Core/O penFOAM-1.4.1-dev/applications/utilities/postProcessing/stressField/interFoamPre ssure/
It compiles with a standard-OpenFOAM-1.4.1-installation (just take care: the above URL usually gets mutilated by the MessageBoard-software)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   October 10, 2007, 07:45
Default Thanks a lot for the link! I h
  #4
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
Thanks a lot for the link! I have downloaded the sources and at a first glance it seems to work well. That was exactly what I was looking for; so far I have used a modified version of the liftDrag tool with the crude approximation, which I described above.

Thanks!!!
Oliver
ogloth is offline   Reply With Quote

Old   October 10, 2007, 07:54
Default Careful with the boundary cond
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Careful with the boundary conditions on p - if you are getting trouble (i.e. pressure distriution that does not look right), the tool now allows you to set the pressure b.c.-s rather than the code trying to guess it.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   October 10, 2007, 08:18
Default The pressure looks ok to me. H
  #6
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
The pressure looks ok to me. How does the tool guess the BCs? Basically that should be the same as those for pd - from my understanding at least ... Btw, how does it work? I assume you take the gravity and the velocity field and then you compute the pressure field that matches these, is this correct?

Another question: Do you recon it is possible to compute flow with a varying gravity field? By varying I mean spatially - a change in time I am already using in the simulation. I guess it could be done by modifying the ghf field in interFoam. This can be important for acceleration fields that are created by spinning.

Oliver
ogloth is offline   Reply With Quote

Old   October 10, 2007, 08:20
Default just found a flaw in my line o
  #7
Super Moderator
 
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 114
Rep Power: 8
ogloth is on a distinguished road
just found a flaw in my line of thinking - BC for pressure should be a gradient in y-direction ...
ogloth is offline   Reply With Quote

Old   October 22, 2007, 20:12
Default > Another question: Do you rec
  #8
New Member
 
Giro
Join Date: Mar 2009
Posts: 13
Rep Power: 8
girogirozakk is on a distinguished road
> Another question: Do you recon it is possible to compute flow with a varying gravity field?
> I guess it could be done by modifying the ghf field in interFoam. This can be important for acceleration fields that are created by spinning.

Hi,Oliver.
I tried that approach & code is opened at this URL.
http://members.jcom.home.ne.jp/issa_.../sloshing.html


May be , It's OK....I think(hope).
If I made mistakes, please teach me.


> compare them with actual flight data (Sloshsat FLEVO).

I want to try , too.
Where the URL I must check?
If no problem, please tell me.


thanks

Giro
girogirozakk is offline   Reply With Quote

Old   October 22, 2007, 22:15
Default I don't understand the followi
  #9
Senior Member
 
Join Date: Mar 2009
Posts: 225
Rep Power: 9
paka is on a distinguished road
I don't understand the following sentence by Dr. Jasak:
"Careful with the boundary conditions on p - if you are getting trouble (i.e. pressure distriution that does not look right), the tool now allows you to set the pressure b.c.-s rather than the code trying to guess it."

I figured out the only way to "set" the b.c. for interFoamPressure is to define the "p" dictionary in 0 sec. time directory. Is it right?

I obtained results for defined "p" b.c. and for undefined "p" b.c. Both results look exactly the same. So how to define those b.c.?

Initially, somehow I missed that topic, so if you would like to help me with verifying my results using interFoamPressure tool please follow the following conversation:
http://www.cfd-online.com/OpenFOAM_D...tml?1192152325

Regards,
Krystian
paka 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
UDF for sloshing Alamedda FLUENT 1 November 13, 2013 02:29
Sloshing Lin FLUENT 1 September 7, 2007 06:11
Sloshing Prabodh FLUENT 0 May 1, 2006 09:36
sloshing Zaher CFX 8 March 27, 2004 18:02
sloshing baned FLUENT 0 September 19, 2003 03:53


All times are GMT -4. The time now is 22:36.