# Fluent-OpenFoam pipe flow comparison

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 January 7, 2014, 04:28 Fluent-OpenFoam pipe flow comparison #1 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 Dear all, I am trying to get the same results in Fluent and OpenFoam for a simple pipe flow (periodic). Unfortunately, the results are quite different and I am wondering if that is just normal for two solvers or if I am doing something wrong. My settings are: DN25 pipe, standard k-e-model, mean velocity = 7 m/s, water, y+=1. I use "enhanced wall treatment" in Fluent and lowRe-wall functions in OpenFoam. These are some results: U-comparison-ske.png k-comparison-ske.png epsilon-comparison-ske.png My feeling says something is wrong... __________________ The skeleton ran out of shampoo in the shower.

 January 7, 2014, 08:26 #2 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 which Turbulence Model did you use in OpenFOAM? If it can help you: Wall treatment with geometrical restriction __________________ In memory of my friend Hervé: CFD engineer & freerider

 January 7, 2014, 08:27 #3 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 It's both the standard k-epsilon without any addition. __________________ The skeleton ran out of shampoo in the shower.

 January 7, 2014, 09:26 #4 Super Moderator     Maxime Perelli Join Date: Mar 2009 Location: Switzerland Posts: 2,972 Rep Power: 30 As far as I know there is no "enhanced wall treatment" option in OF like in Fluent for standard k-epsilon turbulence model. But you can use k-Omega SST model with nutUSpaldingWallFunction. Then set k and omega with uniform value 1e-10 instead of zeroGradient, especially if you have low y+ (y+<=1) __________________ In memory of my friend Hervé: CFD engineer & freerider

 January 7, 2014, 09:30 #5 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,098 Rep Power: 19 I can confirm your results in fluent. Is the "standard" k-epsilon model exactly the same in both solvers, i.e. are the same values used for the coefficients? Messing with the coefficients in fluent, one can approximately reproduce the results from OpenFoam

 January 7, 2014, 09:34 #6 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 Hi, I think the coefficients are the same for the standard k-epsilon. Most likely the boundary conditions are different, also I can't find exactly what Fluent does with all different turbulence values at the walls. __________________ The skeleton ran out of shampoo in the shower.

 January 7, 2014, 09:37 #7 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 Max, I also wrote in the thread you linked: I don't understand why you would set omega to zero for y+<=1 case. It should be some very high value instead. __________________ The skeleton ran out of shampoo in the shower.

 January 7, 2014, 09:46 #8 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 K-Omega-SST comparison: U-comparison-komegasst.jpg k-comparison-komegasst.jpg omega-comparison-komegasst.jpg __________________ The skeleton ran out of shampoo in the shower.

January 7, 2014, 10:21
#9
Super Moderator

Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
Quote:
 Originally Posted by RodriguezFatz Max, I also wrote in the thread you linked: I don't understand why you would set omega to zero for y+<=1 case. It should be some very high value instead.
Thanks for correcting me.
__________________
In memory of my friend Hervé: CFD engineer & freerider

 January 8, 2014, 08:05 #10 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 __________________ The skeleton ran out of shampoo in the shower.

 January 10, 2014, 02:38 Standard k-epsilon model #11 New Member   Geon-Hong Kim Join Date: Feb 2010 Location: Ulsan, Republic of Korea Posts: 27 Rep Power: 7 Although you applied low Re BC on the wall, the standard k-epsilon model can not resolve appropriate turbulent field near the wall since it does not include a damping function. Setting y+ to be close to the unity near the wall for the "standard" k-epsilon model is quite nonsense and I don't expect the solution to be correct with such settings. It seems that you are trying to tighten a screw using pliers instead of screwdrivers. You can tighten screw somewhat using the pliers but it will not be tight enough. Meanwhile the k-omega sst model can inherently resolve the viscous sub layer, and it is natural to estimate reasonable solution with y+ ~ 1. If you want to maintain the y+ near the wall and use a k-epsilon family model, I'd recommend you to apply low Re k-epsilon model with low Re BC's, such as Launder-Sharma k-epsilon model.

 January 10, 2014, 02:45 #12 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 Hey Geon-Hong. Great! Thank you for the answer. That sounds pretty logical. I thought that maybe the wall function will patch all near boundary cells to apply the damping. But I didn't have a look at the source code, which should have revealed what you wrote... Thanks again! AshwaniAssam likes this. __________________ The skeleton ran out of shampoo in the shower.

 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 florian_krause OpenFOAM 22 June 13, 2013 21:25 avi@lpsc FLUENT 4 April 8, 2012 06:12 mazhar1613 ANSYS Meshing & Geometry 1 January 12, 2012 00:18 Michel_sharp OpenFOAM 6 October 24, 2009 04:09 pertupd ANSYS 0 August 12, 2009 08:36

All times are GMT -4. The time now is 21:24.

 Contact Us - CFD Online - Top