Mass flow inlet in Eulerian VOF model

  • 163 Views
  • Last Post 13 December 2018
daniela posted this 11 December 2018

Hey everyone, 

I'm right now trying to simulate the inflow in a rainwater channel. Therefore I've chosen the Eulerian Multi Fluid model, with air as phase 1, water as phase 2. 

As my boundary condition for the inlet I've chosen a mass flow inlet. I've set 0 kg/s for air and 12.5 kg/s for water with a volume fraction of 1. 

I've done a initialization from the inlet and the velocity is generated correctly. After the calculation the post-processing shows a mass flow of max 6e-1 kg/s/m2 at the inlet instead of the set 12.5 kg/s (the area is about 0.088 m2, so it should be aroung 143 kg/s/m2). 

Can anyone tell me how this is possible? Is it not possible to choose a mass flow inlet in a VOF model? Or could there be another reason? 

Thanks in advance, 

 

Regards. 

Daniela

Order By: Standard | Newest | Votes
abenhadj posted this 11 December 2018

1/Is it 2D or 3D?

2/How are you doing the post-processing?

3/Can you confirm that you are using the Eulerian Model?

Share screenshots of the models and of the boundary (bulk and phase) and post-processing.

Best regards,

Amine

kkanade posted this 12 December 2018

also please share screen shots of outlet boundary conditions, models used, other set up etc. 

daniela posted this 12 December 2018

General set up Models 1Models 2Cell Zone ConditionsBoundary 1Boundary 2Boundary 3Boundary outInitialization1Initialization2PatchPhasesRunPost with CFD Post

abenhadj posted this 12 December 2018

What you are now post-processing is just the mass-flux applied at the boundary. You can imagine that Fluent will scale your input of mass-flow at with facets at your inlet so you will see that variation: Fluent divide your 12 kg/s by the water density and total area of inlet to get the normal velocity. What you are now showing is this normal velocity times density divided by the facet area. More important to verify under Report that the mass flow rate for the mixture and water-phase is what you provided as a boundary condition. 

Best regards,

Amine

daniela posted this 12 December 2018

Thanks for the quick response! 

I think I got the calculation of the flux and flow. But as my area of the inlet is only 0.088 m2, I was thinking of a flux of about 143 kg/s/m2. 

I've attached the report in the bottom, but I didn't see any specifications on the mass flow there. 

 

Thanks in advance, 

best regards, 

Daniela

<FluentXMLReport>

<version>

Fluent

Version: 3d, pbns, eulerian, rngke, transient (3d, pressure-based, Eulerian, RNG k-epsilon, transient)

Release: 19.2.0

Title: 

</version>

 

<Models>

 

Models

------

 

   Model                              Settings                         

   -----------------------------------------------------------------

   Space                              3D                               

   Time                               Unsteady, 1st-Order Implicit     

   Viscous                            RNG k-epsilon turbulence model   

   Wall Treatment                     Standard Wall Functions          

   RNG Differential Viscosity Model   Disabled                         

   RNG Swirl Dominated Flow Option    Disabled                         

   Multiphase k-epsilon Models        Mixture k-epsilon                

   Heat Transfer                      Disabled                         

   Solidification and Melting         Disabled                         

   Species                            Disabled                         

   Coupled Dispersed Phase            Disabled                         

   NOx Pollutants                     Disabled                         

   SOx Pollutants                     Disabled                         

   Soot                               Disabled                         

   Mercury Pollutants                 Disabled                         

 

</Models>

 

<MaterialProperties>

Material Properties

-------------------

 

   Material: water-liquid (fluid)

 

      Property                        Units     Method     Value(s)   

      -------------------------------------------------------------

      Density                         kg/m3     constant   998.2      

      Cp (Specific Heat)              j/kg-k    constant   4182       

      Thermal Conductivity            w/m-k     constant   0.6        

      Viscosity                       kg/m-s    constant   0.001003   

      Molecular Weight                kg/kmol   constant   18.0152    

      Thermal Expansion Coefficient   1/k       constant   0          

      Speed of Sound                  m/s       none       #f         

 

   Material: air (fluid)

 

      Property                        Units     Method     Value(s)     

      ---------------------------------------------------------------

      Density                         kg/m3     constant   1.225        

      Cp (Specific Heat)              j/kg-k    constant   1006.43      

      Thermal Conductivity            w/m-k     constant   0.0242       

      Viscosity                       kg/m-s    constant   1.7894e-05   

      Molecular Weight                kg/kmol   constant   28.966       

      Thermal Expansion Coefficient   1/k       constant   0            

      Speed of Sound                  m/s       none       #f           

 

   Material: aluminum (solid)

 

      Property               Units    Method     Value(s)   

      ---------------------------------------------------

      Density                kg/m3    constant   2719       

      Cp (Specific Heat)     j/kg-k   constant   871        

      Thermal Conductivity   w/m-k    constant   202.4      

 

</MaterialProperties>

 

<CellZoneConditions>

Cell Zone Conditions

--------------------

 

   Zones

 

      name                    id   type    

      ----------------------------------

      negativgro--freeparts   3    fluid   

 

   Setup Conditions

 

      negativgro--freeparts

 

         Condition       Value   

         ---------------------

         Frame Motion?   no      

         Mesh Motion?    no      

 

</CellZoneConditions>

 

<BoundaryConditions>

Boundary Conditions

-------------------

 

   Zones

 

      name                         id   type              

      -------------------------------------------------

      inlet                        6    mass-flow-inlet   

      wall-negativgro--freeparts   1    wall              

      outlet                       7    pressure-outlet   

      wall1                        8    wall              

      wall2                        9    wall              

      wall3                        10   wall              

      wall4                        11   wall              

      wall5                        12   wall              

      wall6                        13   wall              

 

   Setup Conditions

 

      inlet

 

         Condition   Value   

         -----------------

 

      wall-negativgro--freeparts

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      outlet

 

         Condition   Value   

         -----------------

 

      wall1

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      wall2

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      wall3

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      wall4

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      wall5

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

      wall6

 

         Condition     Value   

         -------------------

         Wall Motion   0       

 

</BoundaryConditions>

 

<SolverSettings>

Solver Settings

---------------

 

   Equations

 

      Equation          Solved   

      ------------------------

      Flow              yes      

      Volume Fraction   yes      

      Turbulence        yes      

 

   Numerics

 

      Numeric                         Enabled   

      ---------------------------------------

      Absolute Velocity Formulation   yes       

 

   Unsteady Calculation Parameters

 

                                           

      ----------------------------------

      Time Step (s)                   10   

      Max. Iterations Per Time Step   5    

 

   Relaxation

 

      Variable                     Relaxation Factor   

      ----------------------------------------------

      Pressure                     0.3                 

      Density                      1                   

      Body Forces                  1                   

      Momentum                     0.7                 

      Volume Fraction              0.5                 

      Turbulent Kinetic Energy     0.8                 

      Turbulent Dissipation Rate   0.8                 

      Turbulent Viscosity          1                   

 

   Linear Solver

 

                                   Solver     Termination   Residual Reduction   

      Variable                     Type       Criterion     Tolerance            

      ------------------------------------------------------------------------

      Pressure                     V-Cycle    0.1                                

      X-Momentum                   Flexible   0.1           0.7                  

      Y-Momentum                   Flexible   0.1           0.7                  

      Z-Momentum                   Flexible   0.1           0.7                  

      Volume Fraction              Flexible   0.1           0.7                  

      Turbulent Kinetic Energy     Flexible   0.1           0.7                  

      Turbulent Dissipation Rate   Flexible   0.1           0.7                  

 

   Pressure-Velocity Coupling

 

      Parameter   Value                  

      --------------------------------

      Type        Phase Coupled SIMPLE   

 

   Discretization Scheme

 

      Variable                     Scheme               

      -----------------------------------------------

      Pressure                     Second Order         

      Momentum                     First Order Upwind   

      Volume Fraction              Compressive          

      Turbulent Kinetic Energy     First Order Upwind   

      Turbulent Dissipation Rate   First Order Upwind   

 

   Solution Limits

 

      Quantity                         Limit    

      ---------------------------------------

      Minimum Absolute Pressure        1        

      Maximum Absolute Pressure        5e+10    

      Minimum Temperature              1        

      Maximum Temperature              5000     

      Minimum Turb. Kinetic Energy     1e-14    

      Minimum Turb. Dissipation Rate   1e-20    

      Maximum Turb. Viscosity Ratio    100000   

 

</SolverSettings>

 

</FluentXMLReport>

 

 

daniela posted this 13 December 2018

"mfr_air_inlet-rfile"

"Time Step" "mfr_air_inlet etc.."

("Time Step" "mfr_air_inlet" "flow-time")

0 0 0

1 0 10

2 0 20

3 0 30

4 0 40

5 0 50

6 0 60

7 0 70

8 0 80

9 0 90

10 0 100

11 0 110

12 0 120

13 0 130

14 0 140

15 0 150

16 0 160

17 0 170

18 0 180

19 0 190

20 0 200

 

 

"mfr_mixture_inlet-rfile"

"Time Step" "mfr_mixture_inlet etc.."

("Time Step" "mfr_mixture_inlet" "flow-time")

0 12.49999999999998 0

1 12.49999999999998 10

2 12.49999999999998 20

3 12.49999999999998 30

4 12.49999999999998 40

5 12.49999999999998 50

6 12.49999999999998 60

7 12.49999999999998 70

8 12.49999999999998 80

9 12.49999999999998 90

10 12.49999999999998 100

11 12.49999999999998 110

12 12.49999999999998 120

13 12.49999999999998 130

14 12.49999999999998 140

15 12.49999999999998 150

16 12.49999999999998 160

17 12.49999999999998 170

18 12.49999999999998 180

19 12.49999999999998 190

20 12.49999999999998 200

 

 

"mfr_water_inlet-rfile"

"Time Step" "mfr_water_inlet etc.."

("Time Step" "mfr_water_inlet" "flow-time")

0 12.49999999999998 0

1 12.49999999999998 10

2 12.49999999999998 20

3 12.49999999999998 30

4 12.49999999999998 40

5 12.49999999999998 50

6 12.49999999999998 60

7 12.49999999999998 70

8 12.49999999999998 80

9 12.49999999999998 90

10 12.49999999999998 100

11 12.49999999999998 110

12 12.49999999999998 120

13 12.49999999999998 130

14 12.49999999999998 140

15 12.49999999999998 150

16 12.49999999999998 160

17 12.49999999999998 170

18 12.49999999999998 180

19 12.49999999999998 190

20 12.49999999999998 200

 

 

The flow rates seem to be correct (I've chosen different time steps now).  But the CFD Post is still showing the same for the flux. Is there any possibility to check the surface area in fluent? If I check it in DM it says 0.088 m2. And if I divide 12.5 kg/s by 0.088 m2, it should be 142 kg/s/m2, right? 

Could be that I got this wrong somehow. 

Best regards, 
Daniela

rwoolhou posted this 13 December 2018

In Fluent go to the Surface Integrals (Post Processing and/or Reports), one of those gives area. 

abenhadj posted this 13 December 2018

1/Is the contour plot from CFD-Post? Then please go to Calculators and make an area average of it at your Inlet

2/Area inf Fluent: Reports>Surface Integral>Choose Area and then your boundary

Best regards,

Amine

daniela posted this 13 December 2018

abenhadj posted this 13 December 2018

In CFD-Post make Area Integral of Mass Flow at the inlet. Does it fit your 12 kg/s?

Best regards,

Amine

daniela posted this 13 December 2018

No, it doesn't fit. Also if I choose global in z direction it's negative. 

Thanks! 

Best regards, 

Daniela

abenhadj posted this 13 December 2018

Can you please go back to Fluent and check there 2. In Fluent I am not aware about such a variable called mass flow but with dimension of flux.

 

Are you working with *.dat file in CFD-Post or with *.cdat file? Which version are you using?

Best regards,

Amine

daniela posted this 13 December 2018

In Fluent I can't find the variable mass flow. 

I'm using version 19.2, and for CFD-Post it's *.cdat. 

Best regards, 

Daniela

abenhadj posted this 13 December 2018

Hi,

That is what I've actually said: there is no variable called mass flow in Fluent. That is only what CFD-Post does understand when it comes into calculating mass flow based on mass flow variable. In multi-phase runs CFD-Post will try to calculate the integrated mass-flow (your input) based on that variable (which is kg/m^2s). Please build the sum of the variable "mass flow" in CFD-Post. I would say it would match the 12 kg/s.

Best regards,

Amine

abenhadj posted this 13 December 2018

There is no benefit for me to post-process this quantity. An integral report is better or getting contour of velocity and if compressible the density on the inlet is more appropriate. 

Best regards,

Amine

daniela posted this 13 December 2018

This fits. Thank you! 

Then there's another thing I don't understand: If I have 12.5 kg/s of inflow and I did run the calculation for 200 s, how is it possible, that the water only reached the point in the graphics (the canal has a length of 1m, so 0.088 m3). With a inflow of 12.5 kg/s of water it should be 2500 kg (or liter) after 200s, which is way more than the volume of the canal. Might be, that I misunderstand the contour "volume fraction". 

Thanks in advance, 

best regards. 
Daniela

abenhadj posted this 13 December 2018

Contour might be correct but as we do not have any idea about your model any comments will be only given by suspicion. We require some informations about your Case: Which boundaries are included and where? 

 

From the plot it looks after a sort of open channel flow (?) where the water flow is sub-critical and that is why the height is decreasing. Check if you have an outlet if water reached that outlet. Moreover post screenshot of Fluent Residuals.

 

It might be that water reached a level far away but due to coarse resolution the whole vof field is smeared..

 

Best regards,

Amine

daniela posted this 13 December 2018

Basically water is filled in an small open container and it should flow into another bigger container with open surface before getting into a pipeline. To model the open surface I've set atmospheric pressure at the top. 

The big tank has a volume of 2.5 m3, that's why I'm only simulating 200s right now, because I just wanted to see how the water reaches the end of the big container. 

 

I have already decreased the maximum of the volume fraction contour, but it still doesnt reach the end of the container or the pipe.

Thanks. 

Best regards, 

Daniela  

abenhadj posted this 13 December 2018

1/Ensure deep convergence every time step. From residual plot your run is not looking as it should. Share with us settings in FLUENT. 2/work with FLUENT post processing to avoid any issues.

Best regards,

Amine

abenhadj posted this 13 December 2018

Ensure gravity is set properly and free surface is set as symmetry or free slip wall. Include a air layer above water at inlet in case you want to use pressure boundary at top

Best regards,

Amine

daniela posted this 13 December 2018

Thanks! 

Is there a way to ensure convergence or do I just have to increase the number of iterations? 

Best regards. 

abenhadj posted this 13 December 2018

Rather smaller time step size and not more than max. of 20 iterations per time step. Post screenshot Of solution methods and operating conditions

Best regards,

Amine

daniela posted this 13 December 2018

abenhadj posted this 13 December 2018

Please use VOF model with implicit volume fraction and give thai density as operating density. Eulerian model for this case is too complicated 

Best regards,

Amine

daniela posted this 13 December 2018

Okay. 

Which density should I set as operating density? Water or air? 

Best regards, 

Daniela

abenhadj posted this 13 December 2018

Give air as first approximation

Best regards,

Amine

abenhadj posted this 13 December 2018

Check this

Best regards,

Amine

Close