CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM

Lagrangian Boundary Condition (interstitialInletVelocity

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

LinkBack Thread Tools Display Modes
Old   March 14, 2014, 03:27
Lightbulb Lagrangian Boundary Condition (interstitialInletVelocity
Senior Member
maysmech's Avatar
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Hello Foamers,

I have a question about interstitialInletVelocity inlet BC which is used in lagrangian/MPPIC/Goldschemidt testcase.
        type            interstitialInletVelocity;
        inletVelocity   uniform (0 0 1.875);
        value           uniform (0 0 1.875);
        phi             phi.air;
        alpha           alpha.air;
What is its difference with fixedvalue in application?
in its .h description it says:

HTML Code:
    Inlet velocity in which the actual interstitial velocity is calculated
    by dividing the specified inletVelocity field with the local phase-fraction.
To find its difference with uniformFixedValue I compared average magnitude of inlet velocity (By using Integration over bottom patch) and found that in fixedvalue (0 0 2) the average of inlet velocity is 2, But in interstitialInletVelocity of ( 0 0 2 ) the average velocity is 4.8 m/s.
I calculated average alpha.air magnitude in this patch = 0.42 and understood that 4.8 m/s=2.0/0.42 as described in .h file.
Seeing the contour of inlet in this condition shows the magnitude of air varies between 4 to 6.51 m/s with the average of 4.89 (is attached) and I don't know why it increases the stated 2 m/s to higher magnitudes. If it considers the solid fractions in inlet patch so it should be some zero magnitude velocities on inlet but there is not seen.
Attached Images
File Type: png value2-bottomContour-interstitialInletVelocity.png (13.1 KB, 20 views)
maysmech is offline   Reply With Quote

Old   March 23, 2014, 14:29
Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Maysam,

If you take a look into the C file:
Originally Posted by src/finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity/interstitialInletVelocityFvPatchVectorField.C
void Foam::interstitialInletVelocityFvPatchVectorField::updateCoeffs()
    if (updated())

    const fvPatchField<scalar>& alphap =
        patch().lookupPatchField<volScalarField, scalar>(alphaName_);

It essentially defines that the fixed boundary value for U at the inlet should be defined as "inletVelocity_/alphap". Therefore, this apparently assumes that:
  1. "inletVelocity_" is a reference velocity for a full "alphap" value, namely "1.0".
  2. "alphap" can never be zero, otherwise it would result in a crash with a SIGFPE:
  3. The logic might be that the phase proportion is inversely proportional to the velocity, possibly due to a vacuum-like effect. I.e., when there is very little of this phase (smaller than 1.0), it acts as high-speed+low-pressure combination.

Best regards,
wyldckat is offline   Reply With Quote


Thread Tools
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 On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Radiation interface hinca CFX 15 January 26, 2014 18:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
Setting outlet Pressure boundary condition using CAFFA code Mukund Pondkule Main CFD Forum 0 March 16, 2011 04:23
Domain Imbalance HMR CFX 3 March 6, 2011 21:10
How exactly the "pressure outlet" bdry condition compute properties on the boundary? yating9901 FLUENT 3 June 28, 2010 12:26

All times are GMT -4. The time now is 16:26.