
[Sponsors] 
October 26, 2015, 06:29 
Axisymmetric flow problem in constricted pipe

#1 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Dear All,
I'm trying to run an LES (with Smagorinsky model) simulation in OpenFOAM for a constricted pipe flow (Reynolds Number = 500). I've tried to run the same simulation with tetrahedral meshes from 100000 elements to 1500000 elements. Although this flow should be axisymmetric at the region after constriction, in my LES simulations the flow deflect either to upper side or to lower side of the pipe wall (I put a screen shot as an example in the directory attached to this post). I've tried lots of things (increasing the mesh resolution, reducing the tolerance values for p and U, changing the solver type for p and U) but I couldn't get the correct result. Do you have any idea about the solution of this problem? I send my 0 system and constant directories (except polyMesh directory in constant directory) in the attachment if it helps to solve the problem. Best regards, Kamil 

October 28, 2015, 10:36 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Hey, I am currently discussing a case that sounds pretty much the same like yours in the "Main CFD" forum. Since you did not post any picture I am not that sure about your exact geometry.
Conical Diffuser Edit: Ok, I found the picture. Are those time averaged values?
__________________
The skeleton ran out of shampoo in the shower. 

October 28, 2015, 10:47 

#3 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Hi Rodriguez,
Thanks for your interest at first. Yes these are time averaged values. I read the problem you faced with. Both cases look very similar. Do you have any suggestions for me to do? Regards, Kamil 

November 5, 2015, 04:24 

#4 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Dear OpenFOAM Users,
As you know from my previous posts I'm trying to solve an axisymmetric constricted pipe flow problem with pisoFoam solver by using Smagorinsky LES model of OpenFoam. It is expected to have an axisymmetric flow after constriction in my problem. Although I get this expected flow behaviour with a structured mesh (consisted of hexahedral elements), when I'm trying to solve this problem with an unstructured mesh (consisted of prismatic and tetrahedral elements) the flow always tends to be asymmetric. I have to mention that all other parameters of the analyses are same except the mesh. Is this a bug of OpenFoam or is there a possible error that I've done? I'm sending the radial cross sectional views of my unstructured and structured meshes and my 0 system and constant directories for both in the link below if it helps to solve the problem. https://www.dropbox.com/s/i7hc72u0gv...eFlow.zip?dl=0 [^] Best Regards, Kamil 

November 5, 2015, 04:56 

#5 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Hi Kamil,
What Reynolds number are you dealing with? Your meshes look very, very coarse. From these meshes I guess, you use wall modeled LES? Even in wall modeled LES you have strong requirements for the mesh, in all three directions x+, y+, z+. From the way your mesh looks like I don't think you satisfy them. Also you have these sudden jumps of cell volumes, which is very bad for LES, because the spatial filtering doesn't work here. Did you calculate such values as x+,y+,z+?
__________________
The skeleton ran out of shampoo in the shower. 

November 5, 2015, 05:08 

#6 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Hi Rodriguez,
I'm conducting simulations for Re=500. I've tried several meshes (from 100000 up to 1.5 million elements  You can see the radial cross section of the one with 1.5 million elements in the attachment) for the unstructured case. However, I always got the asymmetry problem for unstructured meshes. I've never done any x+,y+,z+ calculations. Could you please inform me about how can I do these calculations for a constricted pipe flow case? Best Regards, Kamil 

November 5, 2015, 05:09 

#7 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Re=500, so this is laminar. Why do you use a turbulence model at all?
__________________
The skeleton ran out of shampoo in the shower. 

November 5, 2015, 05:12 

#8 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Yes this is laminar for the straight pipe flow. But I want to see if there is any transition to turbulence occurs due to constriction at the pipe even for Re=500.
Kamil 

November 5, 2015, 05:14 

#9 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
If you run your case, just type "yPlusLES latestTime" in your terminal. Openfoam will show you some numbers and also will calculate a field for the latest time step for you to view in paraFoam.
Edit: As far as I know you can not use Smagorinsky model for laminar flow, because it produces nonzero eddy viscosity in laminar flows.
__________________
The skeleton ran out of shampoo in the shower. 

November 5, 2015, 05:31 

#10 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Thanks for your informing Rodriguez. I've written the command you said to me and OpenFoam gave me
y+ : min: 0.0183674 max: 2.06231 average: 0.524659 What should I understand from these values? How can I calculate what my y+ value should be? Best Regards, Kamil 

November 5, 2015, 05:42 

#11 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
The problem is, that your flow isn't turbulent and I don't think these numbers have any meaning here. As I wrote above, I think you use a wrong model.
__________________
The skeleton ran out of shampoo in the shower. 

November 5, 2015, 13:43 

#12 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Thank you Rodriguez for your feedbacks. I'll try to solve the problem as laminar and give information. Which solver do you suggest me to use for laminar flow for such a problem?
Regards, Kamil 

November 6, 2015, 02:51 

#13 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
Hi Rodriguez,
I've conducted the same analysis as laminar by using pisoFoam solver. However, I'm still getting asymmetry in the flow after constriction. Best Regards, Kamil 

November 6, 2015, 03:57 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Yes, I think the asymmetry is physical. However, clever people from the other thread still have doubts and gave me some homework
I think if you create a very fine mesh with hexaedral or with tetrahedral cells you will find both solutions showing asymmetry. In my simulations it always became symmetric when I had the larger numerical errors.
__________________
The skeleton ran out of shampoo in the shower. 

November 6, 2015, 04:09 

#15 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
When I'm conducting DNS simulations with another code, I'm always getting symmetric flow. Also, there are experimental studies working with this geometry having symmetric flow. May this be a bug in OpenFOAM? What do you suggest me to do?
Regards, Kamil 

November 6, 2015, 04:15 

#16 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
I get the same in fluent. What other code do you use?
If you get the asymmetry, how do you resolve the turbulence?
__________________
The skeleton ran out of shampoo in the shower. 

November 6, 2015, 07:03 

#17 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
I'm using a DNS code called Nektar++ and I got the flow after constriction symmetric as expected for Re=500. Also there are other works I saw solved the same problem by using OpenFOAM with pisoFoam solver and OneEqEddy turbulence model. In this work also symmetric flow is obtained for Re=500 as seen Figure 5 of the paper.
http://dl.acm.org/citation.cfm?id=2660919 Best Regards, Kamil 

November 6, 2015, 07:06 

#18 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Do you know if this code has real low numerical diffusion? As I wrote above, I get symmetric separation if I use lower numerical schemes with high diffusion. And I get asymmetric separation with very good schemes (low diffusion).
__________________
The skeleton ran out of shampoo in the shower. 

November 6, 2015, 07:27 

#19 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
In DNS (Direct Numerical Simulation) codes Navier–Stokes equations are numerically solved without any turbulence model.
Regards, Kamil 

November 6, 2015, 07:32 

#20 
New Member
Kamil ÖZDEN
Join Date: Feb 2013
Posts: 20
Rep Power: 4 
In DNS (Direct Numerical Simulation) codes Navier–Stokes equations are numerically solved without any turbulence model.
Regards, Kamil 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Axisymmetric pipe flow example  Gowingeng  SU2  3  February 12, 2014 17:31 
3D Swirl flow in the pipe: convergence problem  Sachin U. Nimbalkar  FLUENT  4  January 2, 2014 13:20 
simpleFoam problem validating 3D pipe flow  inf.vish  OpenFOAM Running, Solving & CFD  6  August 11, 2013 23:18 
transient, impregnating flow problem  fgommer  FLUENT  0  February 29, 2012 17:10 
simpleFoam convergence problems for pipe flow problem  Mike Graham  OpenFOAM Running, Solving & CFD  0  January 30, 2012 15:40 