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

How to use MPPICFoam with turbulence effects on particle motion?

Register Blogs Community New Posts Updated Threads Search

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 7, 2017, 07:18
Default
  #21
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Hi guys,

I also problem with kEpsilon model in DPMFoam OF2.2.x. I tried to add terms in scheme but it stills errors.

Code:
--> FOAM FATAL ERROR:

    request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are

6
(
phic_0
((interpolate((((1|A(Uc))*cloudVolSUSu)|rhoc))&S)+(Dp*(g&S)))
alphaPhic
phic
Dp
alphacf
)
Does anybody give me a suggest to fix it?

Thanks
hiuluom is offline   Reply With Quote

Old   June 7, 2017, 07:37
Default
  #22
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Hi all,

I solved the above problems by adding phic at inlet and outlet BC for k and epsilon

k
Code:
 inlet_pipe
    {
        type                    turbulentIntensityKineticEnergyInlet; 
        value                   $initialField; 
        phi             phic;
        alpha           alphac;
        intensity               0.03; 
    }
Code:
outlet
    {
        type               inletOutlet;
        phi             phic;
        alpha           alphac;
        inletValue         $internalField;
        value              $internalField;
    }
epsilon

Code:
inlet_pipe
    {
        type                    turbulentMixingLengthDissipationRateInlet; 
        value                   $initialField; 
        phi             phic;
        alpha           alphac;
        mixingLength            0.042; 
    }
Code:
outlet
    {
        type               inletOutlet;
        phi             phic;
        alpha           alphac;
        inletValue         $internalField;
        value              $internalField;
    }
But I get a new error with that:

Code:
Courant Number mean: 5.18008e-007 max: 0.0244965
Time = 2e-005

Evolving kinematicCloud

Solving 3-D cloud kinematicCloud
Cloud: kinematicCloud
    Current number of parcels       = 0
    Current mass in system          = 0
    Linear momentum                 = (0 0 0)
   |Linear momentum|                = 0
    Linear kinetic energy           = 0
    Rotational kinetic energy       = 0
    model1:
        number of parcels added     = 0
        mass introduced             = 0
    Parcels absorbed into film      = 0
    New film detached parcels       = 0
    Parcel fate (number, mass)      : patch inlet_pipe
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch outside_wall_pipe
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch inside_wall_pipe_1
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch symmetry_pipe
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch symmetry_2
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch outside_wall
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch outlet_ambient
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch inside_wall_pipe_2
      - escape                      = 0, 0
      - stick                       = 0, 0

DILUPBiCG:  Solving for Ucx, Initial residual = 1, Final residual = 1.25761e-009, No Iterations 2
DILUPBiCG:  Solving for Ucy, Initial residual = 1, Final residual = 9.96601e-010, No Iterations 2
DILUPBiCG:  Solving for Ucz, Initial residual = 1, Final residual = 1.65935e-006, No Iterations 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.00719945, No Iterations 18
GAMG:  Solving for p, Initial residual = 0.157115, Final residual = 0.00130879, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0174056, Final residual = 0.000154434, No Iterations 3
time step continuity errors : sum local = 1.30207e-007, global = -1.40036e-008, cumulative = -1.40036e-008
GAMG:  Solving for p, Initial residual = 0.00302915, Final residual = 1.90974e-005, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.00119684, Final residual = 6.68533e-006, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.000211614, Final residual = 7.64506e-007, No Iterations 5
time step continuity errors : sum local = 6.32305e-010, global = -7.29831e-011, cumulative = -1.40765e-008
DILUPBiCG:  Solving for epsilon, Initial residual = 0.000435878, Final residual = 1.6674e-008, No Iterations 1


--> FOAM FATAL ERROR:

    request for volVectorField U from objectRegistry region0 failed
    available objects of type volVectorField are

3
(
Uc_0
Uc
cloudVolSUSu
)


    From function objectRegistry::lookupObject<Type>(const word&) const
From a message OF, I do not know "request for volVectorField U" where BCs are or solution?

The velocity Uc as the same Goldschmidt OF tutorial. I hope foamers give me a recommendation to solve problem.

Thanks
hiuluom is offline   Reply With Quote

Old   June 7, 2017, 12:44
Default
  #23
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Hi again,

Finally, I solved the problems that some BCs require phi and U but these conditions do not get parameter for phi, U because DPM solver is using Uc and phic, rhoc for continuous or fluid phase. Therefore, it should add phic and Uc in BCs.

Here is the case

https://www.cfd-online.com/Forums/at...1&d=1496850233
Attached Files
File Type: zip DPMkEpsilon-case.zip (5.5 KB, 59 views)
hiuluom is offline   Reply With Quote

Old   May 24, 2018, 00:40
Default
  #24
Member
 
Min Zhang
Join Date: Mar 2017
Posts: 81
Rep Power: 9
minzhang is on a distinguished road
Hello,

I am wondering whether you could have a look at my post about MPPICFoam.
Simulate particle/liquid flow in a converging geometry with MPPICFoam

Thank you so much!
minzhang is offline   Reply With Quote

Reply

Tags
dispersion model, mppicfoam


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
UDF for multicomponent particle vaporization Mohsin Fluent UDF and Scheme Programming 17 January 27, 2021 03:57
Multiphase particle motion queries siw Main CFD Forum 0 February 14, 2012 11:00
Discussion: Reason of Turbulence!! Wen Long Main CFD Forum 3 May 15, 2009 10:52
Why Turbulence models are not universal. Senthil Main CFD Forum 4 July 5, 2000 05:34
turbulence modeling questions llowen Main CFD Forum 3 September 11, 1998 05:24


All times are GMT -4. The time now is 15:32.