[colinjd]

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

[olivierG]

hello,

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

regards,
olivier

[Joe Wang]

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

[colinjd]

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.

[olivierG]

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

[markusrehm]

Hi Colin,

is it the same case you posted here ?

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

Regards, Markus

[fchagas]

Does anyone know if Colin has published his work, a dissertation or a paper, maybe?