CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Symmetrical Model With Non Symmetrical Solution (https://www.cfd-online.com/Forums/openfoam-solving/59278-symmetrical-model-non-symmetrical-solution.html)

 jason November 1, 2007 13:05

Hi, I have a pipe that is i

Hi,

I have a pipe that is initially a single pipe which then smoothly splits into four pipes and then smoothly back into a single pipe. At one end is an inlet and at the other a constant pressure outlet. The pipe is symmetric in all axis, the pipes are all the same diameter and the flow is normal to the inlet and outlet. Basically its a manifold that splits a flow into four amounts and then back again.

Common sense tells me that the flow should split into four equal amounts and I get an equal flow to each pipe. However, when I run this case the flow tends to prefer 2 or 3 of the pipes and skews off the centre line. This happens if I do a full model or a cut down model with symmetry boundaries or as laminar or turbulent. The mesh is also built symmetrically and everything converges nicely.

My first thoughts are that the model is 'so' symmetric that it is very sensitive to any numerical errors or there is some transient phenom that I am not catching. I've seen this before somewhere but I can't remember...I'm either getting old or mad...

Much appreciate any ideas.

Regards

Jason

 fugu November 1, 2007 13:47

IMHO when the geometry and bc

IMHO when the geometry and bc are symmetrical the solution has to show the same symmetry at least in fully laminar cases. In transitional and turbulent flow this is not true, however the velocity field should show fluctuations, not some kind of steady state 'skewness. I'd check carefully the geometry and try to run a case at very low Re. Also what happens if you symmetrically close two of the four pipes ?

 jason November 2, 2007 16:00

Hi, Thanks, my thoughts exa

Hi,

Thanks, my thoughts exactly. When I run at Re=5 I get a very nice symmetrical solution for the 4 pipes. When I symmetrically close 2 of the 4 pipes I get a very nice symmetrical solution for Re=5. When I use an exact copy of the same models and increase upto Re=2e6 the flow skews off down 2 or 3 of the pipes in the 4 pipe case and but works correctly in 2 out of 4 closed case.

A quarter of the geometry was made in SolidWorks which was then mirrored in two axis so the geometry should be symmetric. I used gmsh to tet mesh the model and then into OF. Its possible that gmsh didn't construct the mesh symmetrically so I made a quarter mesh then mirrored it in two axis in OF but this still doesn't work. The problem also occurs with 2 further refined meshes made in the same way.

I'm stuck.

Jason

 fugu November 2, 2007 16:22

It seems to me it is a mesh re

It seems to me it is a mesh related issue.
Just to exclude other issues:
- What solver are you using ?
- What turbulence model ?

Also if you could post the geometry I might take a quick look.

 dmoroian November 4, 2007 06:53

Hello Jason and Luca, I also

Hello Jason and Luca,
I also have a classical example of a symmetric geometry that produces asymmetric solution:
http://www.cfd-online.com/OpenFOAM_D...ges/1/5866.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/5867.jpg

Dragos

 dmoroian November 4, 2007 06:56

In the previous message, the f

In the previous message, the first image shows a flow at Re = 20, while the second is at Re = 200.

 dmoroian November 4, 2007 07:06

Oh, and by the way, this asymm

Oh, and by the way, this asymmetry seems to be physical (according to what we learn in school it is called solution bifurcation).

 lucchini November 4, 2007 07:50

Hi all 1) Sovers used? 2)

Hi all

1) Sovers used?
2) boundary conditions?
3) Courant number?
4) Numerical schemes?
5) BlockMeshDict file?

These results cannot be commented without explaining all these things.

Bye

Tommaso

 dmoroian November 4, 2007 10:10

Hi Tommaso, I put the case on

Hi Tommaso,
I put the case on my personal web page:
Dragos Moroianu

I hope it will be helpfull!

Dragos

 fugu November 4, 2007 19:38

Dragos, as a matter of fact t

Dragos,
as a matter of fact there are a number of papers on steady flow asymmetry on a sudden expansion
(e.g. R. M. Fearn , T. Mullin and K. A. Cliffe Nonlinear flow phenomena in a symmetric sudden expansion). However physical asymmetries like the ones you see happen at low Re and might be considered as the beginning of transitional flow. Increasing Re the flow becomes time dependent and the asymmetries are regained in the average flow.
Jason gets the asymmetry at relatively high Re (2e6). I agree with Tommaso that we should get more info on how the runs were performed.

Luca

 dmoroian November 5, 2007 03:05

Hello again Luca, What you sa

Hello again Luca,
What you said is true not only for the sudden expansion, but also for a flow behind a cylinder (increasing the Re number the averaged solution becomes assymetric).
At least for the above case, it doesn't matter what is the solver or the numerical alghorithm or what turbulence model (in case of high Re) you use. Just to answer short: the above results are done using laminar simpleFoam (for a long answer take a look at the case files I made available above). But I used also fluent and starcd with first and second order upwind discretization and the result is similar. The only difference is that transition starts at a higher Re, the lower the order of discretization you choose.

Dragos

 fugu November 5, 2007 05:05

Dragos, I noticed from the in

Dragos,
I noticed from the input files that no turbulence model was used. If your point is that symmetry in
bc and geometry does not imply symmetry in the solution I totally agree with you.
There a number of examples possible in the turbulent/transitional flows bunch (Von Karman wakes etc.).
As for the tests with different codes I would expect to get the same results since the asymmetry, as you said, is physical. Using lower order of discretization introduces numerical diffusion that artificially increases the viscosity and thus reduces the 'real' Re.
However, I think the asymmetries should disappear at higher Reynolds.
Did you observe similar things happening in fully developed turbulent flows?

Luca

 dmoroian November 5, 2007 05:34

Almost fully agreeing with you

Almost fully agreeing with you Luca http://www.cfd-online.com/OpenFOAM_D...part/happy.gif
The computations show that even at high Reynolds numbers (fully turbulent), the asymmetry is present in the averaged solution, at least for the sudden expansion case.

Dragos

 jason November 5, 2007 14:35

Hi all, many thanks for the co

Hi all, many thanks for the comments, I knew I had seen this somewhere before, therefore I am not yet completely mad.

My meshes are too big to post but here are some plots on a course mesh at low Re laminar, high Re laminar and high Re K-e.

/image{pic1}
/image{pic2}
/image{pic3}

I am using simpleFoam.
I am using default solver setting, the same as Dragos except I found a few non-orthogonal correctors helps my case.
Fluid is water,nu=1e-6
Fixed pressure outlet, zero gradient inlet.
No slip walls.
K and e were specified at inlet for the K-e case, calculated as shown in the user guide.
Same fvSchemes used as Dragos.

I can see the similarities to Dragos.

Jason

 jason November 5, 2007 14:44

Now why didn't that work? Lets

Now why didn't that work? Lets try this...

http://www.cfd-online.com/OpenFOAM_D...ges/1/5880.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/5881.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/5882.jpg

Jason

 jason November 5, 2007 14:55

Also, Dragos, I ran your ca

Also,

Dragos, I ran your case in icoFoam with a large timestep, though since the velocity is so low the courant number was always much less than 1.

For the Re=20 case I get a similar result to you above, see here

http://www.cfd-online.com/OpenFOAM_D...ges/1/5884.jpg

For the Re=200 case however...

http://www.cfd-online.com/OpenFOAM_D...ges/1/5885.jpg

I haven't changed your files, just changed it to transient. Did I do something wrong, shouldn't they give the same result?

Regards

Jason

 msrinath80 November 5, 2007 15:15

Jason, Nothing to worry about here. The other solution (asymmetric) will show up if you perturb the velocity/pressure field slightly on one side. There are three solutions at the same Re. I believe this is referred to as transcritical (pitch fork) bifurcation in fluid mechanics stability theory.

 fugu November 5, 2007 15:34

Jason,
looking at your geometry I was wondering if you tried to switch inlet/outlet and/or rotate the
geometry 90 degrees around the main axis to see
if you get the same asymmetries.
Luca

 dmoroian November 6, 2007 02:42

Hi Jason, As Srinath said, th

Hi Jason,
As Srinath said, there is no problem with your results, you just need to wait more, or again as mentioned above you need a perturbation in the flow field. The easiest way would be just to increase the Re (make it turbulent).

Dragos

 jason November 6, 2007 16:30

Hi, I ran a few more tests,

Hi,

I ran a few more tests,

Luca
1/ I get the same results if I make my outlet an inlet and my inlet an outlet. The flow skews off down the same pipes as before.
2/ I get the same result if I rotated my mesh 45 deg or 90 deg and again the flow skews off down the same pipes as before.

Srinath/Dragos
1/ I ran your Re-200 case for 1000000 time steps in icoFoam and your right, I end up with the steady solution that you posted originally, see here

http://www.cfd-online.com/OpenFOAM_D...ges/1/5892.jpg

2/ I ran your case with Re=200000 in simpleFoam with the K-e model and get basically the opposite of the first one, although not as well defined due to the turbulence, see here,

http://www.cfd-online.com/OpenFOAM_D...ges/1/5893.jpg

So, my next question...this is not good for my design, how can I get rid of it and get the equal flow to each pipe that I require, play with the geometry, upset the symmetry? Any ideas?

Regards

Jason

All times are GMT -4. The time now is 12:14.