CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   Flow goes the wrong way (

klaus August 11, 2005 11:41

in the example a flow enters a
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?


hjasak August 11, 2005 17:15

Which solver/what flow conditi
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.


klaus August 13, 2005 11:44

Hrvoje, i followed your pro

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

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


ali August 13, 2005 20:28

I've also observed some proble
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.

hjasak August 14, 2005 07:33

Well, cyclic has been in the c
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.


hjasak August 21, 2005 16:49

Of course, there's nothing wro
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...


ali August 21, 2005 20:28

So sorry Hrv, bad mistake, I w
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.

All times are GMT -4. The time now is 04:32.