Lagrangian Boundary Condition: interstitialInletVelocity

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

March 14, 2014, 03:27
Lagrangian Boundary Condition: interstitialInletVelocity
#1
Senior Member

Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
Hello Foamers,

I have a question about interstitialInletVelocity inlet BC which is used in lagrangian/MPPIC/Goldschemidt testcase.
Code:
```    bottom
{
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:
```Description
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
 value2-bottomContour-interstitialInletVelocity.png (13.1 KB, 40 views)

March 23, 2014, 14:29
#2
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,659
Blog Entries: 39
Rep Power: 99
Greetings Maysam,

If you take a look into the C file:
Quote:
 Originally Posted by src/finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity/interstitialInletVelocityFvPatchVectorField.C Code: ```void Foam::interstitialInletVelocityFvPatchVectorField::updateCoeffs() { if (updated()) { return; } const fvPatchField& alphap = patch().lookupPatchField(alphaName_); operator==(inletVelocity_/alphap); fixedValueFvPatchVectorField::updateCoeffs(); }```
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: http://en.wikipedia.org/wiki/SIGFPE#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,
Bruno
__________________

 March 9, 2016, 18:09 #3 Senior Member   Join Date: Jan 2013 Posts: 301 Rep Power: 6 Dear Bruno, This boundary condition 'interstitialInletVelocity' is used in the lagrangian and multiphase solvers: Code: ```lagrangian/MPPICFoam/Goldschmidt/0/U.air:40: type interstitialInletVelocity; lagrangian/DPMFoam/Goldschmidt/0/U.air:40: type interstitialInletVelocity; multiphase/reactingTwoPhaseEulerFoam/laminar/fluidisedBed/0/U.air:25: type interstitialInletVelocity; multiphase/reactingTwoPhaseEulerFoam/RAS/fluidisedBed/0/U.air:25: type interstitialInletVelocity; multiphase/twoPhaseEulerFoam/laminar/fluidisedBed/0/U.air:25: type interstitialInletVelocity;``` . It seems that this is always used in the inlet BC of continuous phase. So in this case, the item 'inletVelocity' corresponds to the actual velocity predicted from the mass flow rate? So the inlet velocity which is from 'inletVelocity / alpha' is always bigger than the actual one. Do we also need to use this BC for the dispersed phase inlet BC? Thank you so much. OFFO

March 13, 2016, 12:58
#4
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,659
Blog Entries: 39
Rep Power: 99
Quote:
 Originally Posted by openfoammaofnepo It seems that this is always used in the inlet BC of continuous phase.
Yes...

Quote:
 Originally Posted by openfoammaofnepo So in this case, the item 'inletVelocity' corresponds to the actual velocity predicted from the mass flow rate?
yes...

Quote:
 Originally Posted by openfoammaofnepo So the inlet velocity which is from 'inletVelocity / alpha' is always bigger than the actual one.
Greater or equal. If alpha is 1.0, then it's equal.

Quote:
 Originally Posted by openfoammaofnepo Do we also need to use this BC for the dispersed phase inlet BC?
I'm out of context here.
• If the dispersed phase is Lagrangian, then you probably cannot use this boundary condition.
• If it's another fluid, you just need to configure it accordingly in the names.
The paradigm should be simple enough: if I'm not mistaken, the Lagrangian "phase" will act as a physical net that constrains the fluid passing through it.
__________________

 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 Zerzura FLUENT 0 January 20, 2016 05:21 Saima CFX 45 September 22, 2015 10:53 Sanyo CFX 17 August 15, 2015 06:20 hinca CFX 15 January 26, 2014 18:11 volo87 CFX 5 June 14, 2013 17:44

All times are GMT -4. The time now is 04:04.

 Contact Us - CFD Online - Top