|
[Sponsors] |
October 8, 2007, 13:22 |
Dear all,
I have the follow
|
#1 |
Senior Member
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 121
Rep Power: 17 |
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 |
|
October 10, 2007, 03:13 |
I guess my posts must be reall
|
#2 |
Senior Member
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 121
Rep Power: 17 |
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 |
|
October 10, 2007, 07:14 |
Hi Oliver!
This might, or m
|
#3 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
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 |
|
October 10, 2007, 07:45 |
Thanks a lot for the link! I h
|
#4 |
Senior Member
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 121
Rep Power: 17 |
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 |
|
October 10, 2007, 07:54 |
Careful with the boundary cond
|
#5 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,906
Rep Power: 33 |
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 |
|
October 10, 2007, 08:18 |
The pressure looks ok to me. H
|
#6 |
Senior Member
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 121
Rep Power: 17 |
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 |
|
October 10, 2007, 08:20 |
just found a flaw in my line o
|
#7 |
Senior Member
Oliver Gloth
Join Date: Mar 2009
Location: Todtnau, Germany
Posts: 121
Rep Power: 17 |
just found a flaw in my line of thinking - BC for pressure should be a gradient in y-direction ...
|
|
October 22, 2007, 20:12 |
> Another question: Do you rec
|
#8 |
New Member
Giro
Join Date: Mar 2009
Posts: 13
Rep Power: 17 |
> 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 |
|
October 22, 2007, 22:15 |
I don't understand the followi
|
#9 |
Senior Member
Join Date: Mar 2009
Posts: 225
Rep Power: 18 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
UDF for sloshing | Alamedda | FLUENT | 1 | November 13, 2013 01:29 |
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 17:02 |
sloshing | baned | FLUENT | 0 | September 19, 2003 03:53 |