
[Sponsors] 
October 5, 2015, 16:56 
Computational Fluid Dynamics Simulations of Pipe Elbow Flow

#1 
Senior Member
M. C.
Join Date: May 2013
Location: Italy
Posts: 117
Rep Power: 4 
Hi all,
I'm trying to solve the following case study using OpenFOAM 2.3.1; it is an incompressible, steady state turbulent internal flow inside a bended pipe (simpleFoam). Here's the paper: http://prod.sandia.gov/techlib/acces...004/043467.pdf I chose to use this case to better understand turbulence modelling. I managed to prepare the boundary layers according to what is written on the paper: first layer 0,15mm to the wall and by looking at the pictures, I also added 4/5 layers (1,2 expansion factor). I chose to use the komega turbulence model for the calculation; the reason is because using the RNGkEpsilon model (or standard kE), OF crashes at the beginning of each calculation. Can't understand why; I also tried to run the case as laminar in the beginning, and then switching to turbulence, but every time it crashes. (Why?) Initial conditions as for paper, I only set for the pressure value to 0Pa at outlet, and to 0,1Pa for the internal field. I get a solution converged in about (monitoring massflow difference between inlet & outlet) 1800 iterations. Anyway when I plot (in paraview) the 45° section on the bend, I'm not able to see any secondary (inertial) eddy as described in the paper (see fig.5). Even value for p to the wall seems different: I got about 9000Pa (p*rho) instead of 100000Pa (see fig.6) I can't really understand if my calculation is totally wrong and how should I check for mistakes, or simply it's a postprocessing visualization problem. Can someone help me? Thanks a lot. Michele PS: in the tar file there's the 1800 time folder. If you want to run the case, you should: 1  import the mesh from unv file 2 – using surfaceToPtach constant/triSurface/inlet.stl & surfaceToPtach constant/triSurface/outlet.stl to generate patches 3  correct the boundary file 4  run the case 

October 6, 2015, 09:53 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
1) Pressure: In the paper they plot the absolute pressure, in OpenFoam you will probably look at relative pressures.
2) Pressure: I don't think you need to multiply pressure with rho as you suggested for the incompressible solvers. It's just "p". 3) If you post the log output of the kepsilon crash, we can suggest some help. 4) How do the residuals look like in your converged solution? 5) Did you check your flowrate? Does it match the one from the paper?
__________________
The skeleton ran out of shampoo in the shower. 

October 6, 2015, 10:02 

#3 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Do you understand the paper? First, they state that the y+ is choosen to capture the strong gradients in the viscous boundary layer. Then they write about wall functions. Does that make sense?
__________________
The skeleton ran out of shampoo in the shower. 

October 6, 2015, 12:46 

#4  
Senior Member
M. C.
Join Date: May 2013
Location: Italy
Posts: 117
Rep Power: 4 
Hi and thanks for your kind reply.
Quote:
2) Sorry, but I disagree. I'm quite sure that for incompressible solver I have to multiply by rho, as you're supposed to define ni (m2/s) in the transport properties. By the way, it make no sense for me that: water flowing at a mean velocity rate of 5m/s on a pipe of 35,5 mm can generate a static pressure of 9 Pa only, on a 90° bend. I think this is no physically correct. Quote:
For my calculation, I only divided epsilon by k to estimate omega value, assuming right values given on paper. Definition of omega at CFD on line, it is said that for some solver, you should to use Epsilon/k/0,09. What should I use then? http://www.cfdonline.com/Wiki/Speci...ssipation_rate Quote:
Quote:
So I think it matches. futher: if you calculate v*pipeArea*3600=17.84m3/h Quote:
Inlet velocity profile for turbulent pipe flow using swak4Foam In anycase, I can't still understand how to model that inertial effects. Or in other words: should these behaviour only be predicted by using a lowRe turbulence model or not? Or is it only a matter of postprocessing I don't know? Or did I understand nothing? Thank you very much 

October 6, 2015, 17:33 

#5  
Senior Member
M. C.
Join Date: May 2013
Location: Italy
Posts: 117
Rep Power: 4 
Quote:
If they write to use wall functions, they plan to not resolve the viscous sublayer, putting the y+ node in the loglayer. So these two considerations contradict each other... Quote:
Keeping the opinion that this paper is right, my question is: why I can't see any inertial effect on the 45° plane? the answers I could give are: 1) there aren't any and my calculation is true; 2) I made some errors; 3) I don't know how to analyze data correctly. 

October 7, 2015, 01:44 

#6 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Ok, you are absolutely right about pressure normalization.
So they plot the "inplane velocity" I guess that means the part of the velocity that is parallel to the diagonal plane. I don't know how to get this in paraFoam, but it's not just the velocity magnitude. If you still want kepsilon running you can reproduce the crash and post some log.
__________________
The skeleton ran out of shampoo in the shower. 

October 7, 2015, 01:52 

#7 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,274
Rep Power: 18 
Here you go:
view secondary flow in paraFoam
__________________
The skeleton ran out of shampoo in the shower. 

October 8, 2015, 07:28 

#8 
Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 46
Rep Power: 11 
I just tried, your mesh is running with kEpsilon turbulence model without any problems. With the postprocessing described in Philipps link, you can clearly see the secondary flow in the elbow.
Anyway I have not checked the absolute values (p and U) and compared with the values given in the reference. I also set a uniform (homogenous) inlet velocity as I have not installed the swakForFoam library. Best regards, Jan 

October 9, 2015, 10:37 

#9 
Senior Member
M. C.
Join Date: May 2013
Location: Italy
Posts: 117
Rep Power: 4 
Ok, thanks to all.
About secondary flow, it was only a problem about postprocessing. I rerun the case with the kEpsilon model as well and yes, it worked for me too. I remeshed the geometry many times, so maybe this time it fits to kepsilon model better. I remember there was a floating point exception error; this error use to disappear when the n coefficient for the inlet profile was > 1. So, at that time, my conclusions were that for very small cells, some ratio about coefficient of the matrix Ax=b, gives to the linear solver a division by very small number like 1/0; but I didn't know how to check this. It would be of help to know how to map (sometimes) these floating points error; I mean if it is possible to look at the matrix, at the cell or whatever... I have one more question about the p & U value at the wall in order to check the matching between paper and my calculation, but I'm making this last one on postproccessing forum. Bye. 

Tags 
eddy, komega, paraview, simplefoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Flow in pipe elbow  Martin1  FLUENT  2  May 6, 2015 15:20 
Gate valve flow simulations...  nikesh  FloEFD, FloWorks & FloTHERM  5  January 28, 2014 02:31 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
Double Walled Pipe Boundary  dahvqaz  FLUENT  2  December 5, 2012 11:14 
Fluid Dynamics Eng  PAX Mixer  San Rafael, CA  Gary Jong  FLUENT  0  February 25, 2008 21:46 