# Symmetrical Model With Non Symmetrical Solution

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

 November 1, 2007, 13:05 Hi, I have a pipe that is i #1 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 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

 November 1, 2007, 13:47 IMHO when the geometry and bc #2 New Member   Luca Liberti Join Date: Mar 2009 Location: Rome, Italy Posts: 22 Rep Power: 10 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 ?

 November 2, 2007, 16:00 Hi, Thanks, my thoughts exa #3 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 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

 November 2, 2007, 16:22 It seems to me it is a mesh re #4 New Member   Luca Liberti Join Date: Mar 2009 Location: Rome, Italy Posts: 22 Rep Power: 10 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.

 November 4, 2007, 06:53 Hello Jason and Luca, I also #5 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 Hello Jason and Luca, I also have a classical example of a symmetric geometry that produces asymmetric solution: Dragos

 November 4, 2007, 06:56 In the previous message, the f #6 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 In the previous message, the first image shows a flow at Re = 20, while the second is at Re = 200.

 November 4, 2007, 07:06 Oh, and by the way, this asymm #7 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 Oh, and by the way, this asymmetry seems to be physical (according to what we learn in school it is called solution bifurcation).

 November 4, 2007, 07:50 Hi all 1) Sovers used? 2) #8 Member   Tommaso Lucchini Join Date: Mar 2009 Posts: 84 Rep Power: 10 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. Please let us know. Bye Tommaso

 November 4, 2007, 10:10 Hi Tommaso, I put the case on #9 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 Hi Tommaso, I put the case on my personal web page: Dragos Moroianu I hope it will be helpfull! Dragos

 November 4, 2007, 19:38 Dragos, as a matter of fact t #10 New Member   Luca Liberti Join Date: Mar 2009 Location: Rome, Italy Posts: 22 Rep Power: 10 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 BlnPhoenix likes this.

 November 5, 2007, 03:05 Hello again Luca, What you sa #11 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 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

 November 5, 2007, 05:05 Dragos, I noticed from the in #12 New Member   Luca Liberti Join Date: Mar 2009 Location: Rome, Italy Posts: 22 Rep Power: 10 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 BlnPhoenix likes this.

 November 5, 2007, 05:34 Almost fully agreeing with you #13 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 Almost fully agreeing with you Luca 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

 November 5, 2007, 14:35 Hi all, many thanks for the co #14 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 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 velocity inlet, zerogradient pressure. 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

 November 5, 2007, 14:44 Now why didn't that work? Lets #15 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 Now why didn't that work? Lets try this... Jason

 November 5, 2007, 14:55 Also, Dragos, I ran your ca #16 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 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 For the Re=200 case however... 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

 November 5, 2007, 15:15 Jason, Nothing to worry about #17 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 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.

 November 5, 2007, 15:34 Jason, looking at your geomet #18 New Member   Luca Liberti Join Date: Mar 2009 Location: Rome, Italy Posts: 22 Rep Power: 10 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

 November 6, 2007, 02:42 Hi Jason, As Srinath said, th #19 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 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

 November 6, 2007, 16:30 Hi, I ran a few more tests, #20 Member   Jason Dale Join Date: Mar 2009 Location: UK Posts: 73 Rep Power: 10 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 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, 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Virag CFX 2 July 8, 2007 13:50 Amer FLUENT 0 May 8, 2007 02:59 justin Main CFD Forum 0 January 17, 2007 13:36 Dave FLUENT 2 April 2, 2004 06:55 Martin FLUENT 4 June 18, 2001 10:12

All times are GMT -4. The time now is 07:09.