CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Verification & Validation

Poor Correlation of compressibleInterFoam for Water-Air Mixture in Vertical Pipe

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 29, 2015, 12:09
Question Poor Correlation of compressibleInterFoam for Water-Air Mixture in Vertical Pipe
  #1
New Member
 
Colin
Join Date: Mar 2015
Location: UK
Posts: 3
Rep Power: 7
colinjd is on a distinguished road
Hi everyone,

I’m looking to share some results and seek some ideas for a problem that I’m having when correlating OpenFOAM against experimental predictions with compressibleInterFoam.

The experiment was performed on a 4m vertical pipe with a 90 degree bend at the top (see image attached). The air-water mixture entered at the bottom of the pipe and developed into an “intermittent” or “churn” flow regime before reaching the bend. Note that this is a similar flow regime to “slugging” and occurs when the gas volume flowrate is higher than the liquid volume flowrate.

Initially, the experiment was replicated in CCM+ and good correlation was achieved in terms of liquid distributions and force measurements on the bend. Replicating the study in OpenFOAM was less successful – the liquid distribution is significantly different (“annular” rather than “intermittent” flow) and, subsequently, the bend forces are reduced. The flowfields from CCM+ and OpenFOAM 2.3.1 are presented in the attached file.

I realise that you’ll need more information to give this a full diagnosis but here are the key ingredients:
  • Solver settings from depthCharge3D tutorial
  • LES turbulence settings from nozzleFlow2D tutorial (interFoam)
  • Variable timestep with max Courant = 0.5
  • Constant velocity inlet, pressure outlet (1barg), no-slip on the walls
  • Fluid properties from depthCharge3D tutorial, except that water is rhoConst (only interested in gas compression)
  • Mesh exported from CCM+
  • Surface tension (sigma) is 0.07kg/s2

In order to improve the correlation, I’ve applied a few tweaks to the method but have not seen much improvement:
  • Reduced max Courant to 0.2
  • Repeated simulation in interFoam (assuming compressibility effects to be of a lower order)
  • Increased nOuterCorrections from 1 to 2 (PIMPLE rather than PISO solver)
  • Applied higher order Div schemes (from linear to cubic)
  • Tried a range of Dynamic and Constant Wall Contact Angles with fairly arbitrary settings
  • Tried cAlpha = 0, 1 and 2 to gauge the sensitivity to interface compression

At this stage, I’m just wondering if anyone has done a similar correlation exercise and whether they were successful? Published literature is obviously minimal but any references would also be appreciated, and I can provide more information of my setup if required.

Are there any know limitations of compressibleInterFoam in respect of this type of problem?

Kind regards,

Colin
Attached Images
File Type: jpg compressibleInterFoam Flow Distribution.jpg (38.6 KB, 130 views)
colinjd is offline   Reply With Quote

Old   June 30, 2015, 08:27
Default
  #2
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14
olivierG is on a distinguished road
hello,

I have some interest for this.
Could you provide your fvScheme & fvSolution ?
and ideally, can you share your experimental data ?

regards,
olivier
olivierG is offline   Reply With Quote

Old   December 3, 2015, 22:04
Default
  #3
New Member
 
Jue Wang
Join Date: Apr 2014
Posts: 22
Rep Power: 8
Joe Wang is on a distinguished road
Hi,
I'm also interested in compressibleInterFoam. But I failed to setup the solver with turbulent model. Did you mean you applied LES model for compressibleInterFoam? If so, how did you modified the fvscheme and fvsolution files? Besides, have you ever tried RAS model for compressibleInterFoam? Thank you.

Joe
Joe Wang is offline   Reply With Quote

Old   February 24, 2016, 07:00
Default
  #4
New Member
 
Colin
Join Date: Mar 2015
Location: UK
Posts: 3
Rep Power: 7
colinjd is on a distinguished road
Please find attached the fvSchemes and fvSolution as requested.

I have only looked at LES in detail. Laminar and k-e were also considered but did not improve the solution.

As an update to the orginal post: refining the mess in the cross-sectional plane from ~500 to ~2000 gave a good match to experimental data, with all of the settings in the original post and the fvSchemes/fvSolution attached.
Attached Files
File Type: zip fvSchemesSolution.zip (1.4 KB, 25 views)
colinjd is offline   Reply With Quote

Old   February 29, 2016, 04:24
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14
olivierG is on a distinguished road
hello,

In your setting you use gauss upwind (1 order) for a LES model !
If refining your mesh give you better result, then you really need to check your mesh.
By the way, how fine is your mesh ? tetra or hexa type ? This may change a lot of things.

regards,
olivier
olivierG is offline   Reply With Quote

Old   March 2, 2016, 07:43
Default
  #6
Senior Member
 
Markus Rehm
Join Date: Mar 2009
Location: Erlangen (Germany)
Posts: 184
Rep Power: 13
markusrehm is on a distinguished road
Hi Colin,

is it the same case you posted here ?

http://www.cfd-online.com/Forums/ope...ical-pipe.html

Regards, Markus
markusrehm is offline   Reply With Quote

Old   August 8, 2019, 15:43
Default
  #7
New Member
 
Felipe Chagas
Join Date: Feb 2019
Posts: 11
Rep Power: 3
fchagas is on a distinguished road
Does anyone know if Colin has published his work, a dissertation or a paper, maybe?
fchagas is offline   Reply With Quote

Reply

Tags
compressibleinterfoam, openfoam 2.3.1, slug flow, vertical pipe, water and air

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
air flux through a boundary with air-water mixture Hale OpenFOAM Post-Processing 11 January 6, 2015 12:56
Boundary condition of velocity and pressure at interface for air water pipe flow jignesh_thaker2007 OpenFOAM Running, Solving & CFD 7 June 19, 2014 10:12
energy conservation in vertical pipe Atit Koonsrisuk CFX 1 March 30, 2005 11:41
Tangential Air Flow in a circular pipe Scott Turner Main CFD Forum 3 January 31, 2005 14:59
My Revised "Time Vs Energy" Article For Review Abhi Main CFD Forum 2 July 9, 2002 09:08


All times are GMT -4. The time now is 15:38.