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

Flow goes the wrong way

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2005, 11:41
Default in the example a flow enters a
  #1
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 8
klaus is on a distinguished road
in the example a flow enters a volume at a given angle (picture) and i would
assume that it will keep the direction for a while. The initial velocity in
the volume is zero. But to my surprise the flow starts to change direction
immediatelly. There is no pressure gradient in this direction. Only the mesh
is not orthogonal but i included:

nCorrectors 4;
nNonOrthogonalCorrectors 8;


Has somebody an explanation?



Greetings,
Klaus
klaus is offline   Reply With Quote

Old   August 11, 2005, 17:15
Default Which solver/what flow conditi
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Which solver/what flow conditions? Are you having problems with boudnary conditions? How about trying potentialFoam for starters to see what you get (that one is easy) and then trying a restart from the potential solution.

Your picture looks like it has already blown up pretty much + I cannot say whether you've got a velocity going through the bottom boundary - is that meant to be a wall? Try checking the pressure and velocity b.c. on that patch.

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

Old   August 13, 2005, 11:44
Default Hrvoje, i followed your pro
  #3
New Member
 
Klaus Wittig
Join Date: Mar 2009
Posts: 20
Rep Power: 8
klaus is on a distinguished road
Hrvoje,

i followed your proposal to use potentialFoam but the problem is not solved. I
attached a picture of a part of the structure together with the flow. Its a
turbo-charger turbine (half of it is displayed). You see the flow-velocity in
y direction which is nearly circumferential. In the picture you see that the
circumferential velocity is changing to zero after leaving the bladed
section. Of course this is wrong. The rotational momentum of the flow should
stay but it does not. I use the "cyclic" boundary-condition as shown in the
scetch.

This is very disturbing. Are there are some known limitations on using the
"cyclic" conditions? Any other ideas?




regards,
Klaus
klaus is offline   Reply With Quote

Old   August 13, 2005, 20:28
Default I've also observed some proble
  #4
ali
Member
 
Ali Heidari
Join Date: Mar 2009
Location: Surrey, London, United Kingdom
Posts: 39
Rep Power: 8
ali is on a distinguished road
I've also observed some problems with "cyclic" boundaries in OpenFOAM, especially when dealing with "gamma" for interface flows.

I can provide a case that proves cyclic boundary has problems at least for gamma.
ali is offline   Reply With Quote

Old   August 14, 2005, 07:33
Default Well, cyclic has been in the c
  #5
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Well, cyclic has been in the code for about 10 years now and it has been tested in a lot of detail. Regarding the cyclic problems for the Gamma scheme, I have never seen any (and I have implemented both) so if you've got a test case showing the problem please post it to me or the Bugs mailing list asap.

As for the turbine case, I don't see anything unusual about it and FOAM should solve this kind of thing without any trouble. However, the potential flow is only a first step. Consider what happens in this case if you say that U equals grad p - that's what you get from the potential solution. Behind the rotor, there is no circumferential pressure gradient (right?), so the potential solution gives you no rotation - you need inertia for that. Try restarting the full Navier-Stokes solution from this.

Incidentally, how are you dealing with the fact that the rotor is rotating? Do you have the whole domain "spinning" (needs centrifugal and Coriolis forces added into the code) or do you have a sliding interface? Sorry, I don't usually do turbomachinerey so I don't know the customary approach.

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

Old   August 21, 2005, 16:49
Default Of course, there's nothing wro
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Of course, there's nothing wrong with the cyclic boundary: the case provided by Ali was set up all wrong.

For future reference, please note: BOTH sides of the cyclic boundary belong into the same patch, such that the first half is one side and the second is the opposite. (this may change in the near future, but is the case for foam-1.1). Also, reading the manual sometimes helps...

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

Old   August 21, 2005, 20:28
Default So sorry Hrv, bad mistake, I w
  #7
ali
Member
 
Ali Heidari
Join Date: Mar 2009
Location: Surrey, London, United Kingdom
Posts: 39
Rep Power: 8
ali is on a distinguished road
So sorry Hrv, bad mistake, I was under impression cyclic needs certain settings as inlet boundary does for "gamma" variable (phase indicator) and although I had looked through sampleb tutorials, I totally forgot that may be the problem.
ali 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
Where I am wronG lam OpenFOAM Running, Solving & CFD 3 August 8, 2007 03:56
what's wrong with it???????? zhu FLUENT 1 August 29, 2006 09:35
what wrong with my udf? tristan FLUENT 0 April 20, 2006 04:27
Boundary layer flow goes the wrong way andimb OpenFOAM Running, Solving & CFD 2 March 20, 2006 09:51
laminar pipe flow? Fluent gives wrong result SAM FLUENT 2 November 5, 2004 02:39


All times are GMT -4. The time now is 20:38.