[atul1018]

Hello All,


I am trying to simulate patricle-laden backward facing step (BFS) case using DPMFoam solver in version OpenFoam-v1912. The particles are injected at inlet with speed of 10.5 m/s along with fluid (air). Fluid field has turbulent flow condition (turbulent flow profile with max. velocity 10.5 m/s, average velocity 9.39 m/s). The solver runs successfully and particle seems to move with the fluid. I am using RANS model with KomegaSST model for solving CFD domain considering flow to be turbulent. To incorporate the turbulent effects on particles, both the gradientDispersionRAS and stochasticDispersionRAS model are tried.



But the problem is that...I cannot see much particles in span-wise direction (y-axis) i.e. particle dispersion is not occurring inspite of using gradientDispersionRAS/stochasticDispersionRAS dispersion model.


I am wondering, what could be the probable reason for that? I am also not sure about the boundary conditions provided at inlet for U.air, p, nut.air, k.air and Omega.air. I am using mappedField BC (for U.air, k.air and Omega.air) to represent turbulent flow at inlet.


PS: for the reference, I am attaching the screenshot of simulation results showing almost no particle dispersion in span-wise direction (y-axis). Also the compressed case files are provided.









Hope to get some help.


Kind Regards
Atul

[oswald]

Did you compare your case to the same case without dispersion activated? Is there no difference or is there little difference? If there is only little difference, maybe your TKE is just too small to be relevant. Did you have a look at this?

[atul1018]

Originally Posted by oswald

Did you compare your case to the same case without dispersion activated? Is there no difference or is there little difference? If there is only little difference, maybe your TKE is just too small to be relevant. Did you have a look at this?

Hello Oswald,


Thanks for your reply!


Yes, I did simulated the case with and without dispersion model.I cannot see major difference in particle motion and its dispersion along span (y-axis). However, very small number of particles are found near to lower wall towards outlet, when dispersion model (gradientDispersionRAS) model is used. I am attaching the screenshots of simulations (a) without any dispersion model (b) with dispersion model (graddientDispersionRAS).


Regarding turbulent kinetic energy (TKE), I assumed initial turbulence energy as 5% of max velocity (10.5 m/s). Which means I have provided in 0/k directory k==0.331 m2/s2 as an initial guess. Correct me if I am wrong, this iniial value of turbulence kinetic energy provided in 0/k directory is just an initial guess and actual value of it gets modelled depending upon which turbulence model (I am using komegaSST) you use. So value of this initial guess is not really important, right?


I am also attaching the screenshot of k.air at the end of simulation along with k.air directory. Please let me know if you find something wrong or any way to get better results.

0/k.air


dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0.331;

boundaryField
{
    inlet
    {   
       /* type            zeroGradient;*/
        
        type                mapped;
        value               uniform 2e-05;
        interpolationScheme cell;
        setAverage          true;
        average             2e-05;
   }
    outlet
    {
        type            zeroGradient;
    }    
    walls
    {
        type            kqRWallFunction;
        value           uniform 0.331;
    }
    sides
    {
        type            empty;
    }  
}

Best Regards
Atul Jaiswal

[oswald]

Thanks for providing the additional information.


I think the dispersion model works just as it is intended. GradientDispersionRAS.H states that "The velocity is perturbed in the direction of -grad(k)". This means that particles are pushed more in direction of low values of k. In your case, this seems to in general the region where the particles are without dispersion. So they tend to stay there. I would assume that using the stochastic model would result in some more particles going downwards?



Regarding your k-BCs: At the moment you are using a mapped BC, meaning that the actual value is mapped from somewhere inside the domain. But you prescribe an average of 2e-5, so only the distribution might be altered by scaling the values at the offset plane to reach the desired average. Your picture suggests that the inflow is not fully developed. Maybe you could change to not prescribing the average? You could also try to approximate your k-Value with these hints: https://www.cfd-online.com/Wiki/Turbulence_intensity


One thing more to consider: The velocity in x-direction is approximately 10m/s, the average k-Values seem to be in the order of 1 m²/s². This would result in turbulent velocity fluctuations with a variance of approx. 0.8 m/s. Even when seeing this velocity all the time (in ~68% of the time it should be less), the particles would only get once from top to bottom while flying through the domain.

[atul1018]

Thank you so much for your answers. It is really helping me.

I think the dispersion model works just as it is intended. GradientDispersionRAS.H states that "The velocity is perturbed in the direction of -grad(k)". This means that particles are pushed more in direction of low values of k. In your case, this seems to in general the region where the particles are without dispersion. So they tend to stay there. I would assume that using the stochastic model would result in some more particles going downwards?

-yes, I did try with stochastic dispersion model (stochasticDispersionRAS) too and I could not see major difference between gradient and stochastic dispersion. I am attaching the screenshot of particles at the end of simulation where I used stochastic dispersion model. In fact, with stochastic dispersion model i see even lesser number of particles near to lower wall.

Regarding your k-BCs: At the moment you are using a mapped BC, meaning that the actual value is mapped from somewhere inside the domain. But you prescribe an average of 2e-5, so only the distribution might be altered by scaling the values at the offset plane to reach the desired average. Your picture suggests that the inflow is not fully developed. Maybe you could change to not prescribing the average? You could also try to approximate your k-Value with these hints: https://www.cfd-online.com/Wiki/Turbulence_intensity

-As I mentioned in previous texts that I assumed initial turbulence intensity to be 5%, providing the value of k.air=0.331 m2/s2 (corresponding to bulk velocity 9.39 m/s) as initial guess. I have looked into the thread (https://www.cfd-online.com/Wiki/Turbulence_intensity) to estimate the turbulence intensity depending on Reynold's number. The Reynolds number are ~14000 and ~18000 at inlet ( for half channel height) and at step location (for step height) respectively and estimated turbulence intensity are 0.0485 and 0.047 respectively. these estimated values are very close to my assumed values 5% (0.05). So I believe my boundary condition for k is fine.

-I am using mapped bc to get fully developed turbulent flow and my offset location is 0.067m downstream from inlet. Regarding scaling the k and omega, This time I turned the averaging off and run the simulation (the boundary conditions files are attached for reference) with stochastic dispersion model. I believe that this time I get fully developed flow at inlet (as per my knowledge: fully developed flow profile doesn't change w.r.t. space). I am attaching the fluid flow profiles at x=-0.1335 (inlet), -0.13, -0.1 and 0 (step location). From the profiles, you can see that they don't change as we move in x-direction. However, I am getting max. velocity of 10.41 m/s which should be 10.5 m/s (don't know why?). The no-slip condition is not satisfied at x=-0.1335 (inlet) but by x=-0.13 we can see the velocity at walls equal to zero (no-slip condition satisfied). Do you think that my understanding of fully developed turbulent flow is correct and the profiles I am getting is fully developed?

blockMeshDict (only inlet is shown)

inlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 mappedPatch;
　　　　　　　 sampleMode　　　　　 nearestCell;
　　　　　　　 sampleRegion　　　 region0;
　　　　　　　 samplePatch　　　　 none;
　　　　　　　 offsetMode　　　　　 uniform;
　　　　　　　 offset　　　　　　　　　 (0.067 0 0);
　　　　　　 
　　　　　　　 
　　　　　　 /* type　　　 patch; */
　　　　　　　 faces
　　　　　　　 (
　　　　　　　　　　　 (4 7 3 0)
　　　　　　　 );
　　　 }

k.air

dimensions　　　　　 [0 2 -2 0 0 0 0];

internalField　　 uniform 0.331;

boundaryField
{
　　　 inlet
　　　 {　　 
　　　　　　 /* type　　　　　　　　　　　 zeroGradient;*/
　　　　　　　 
　　　　　　　 type　　　　　　　　　　　　　　　 mapped;
　　　　　　　 value　　　　　　　　　　　　　　 uniform 2e-05;
　　　　　　　 interpolationScheme cell;
　　　　　　　 setAverage　　　　　　　　　 false;
　　　　　　　 average　　　　　　　　　　　　 2e-05;
　　 }
　　　 outlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }　　　 
　　　 walls
　　　 {
　　　　　　　 type　　　　　　　　　　　 kqRWallFunction;
　　　　　　　 value　　　　　　　　　　 uniform 0.331;
　　　 }
　　　 sides
　　　 {
　　　　　　　 type　　　　　　　　　　　 empty;
　　　 }　 
}

omega.air

dimensions　　　　　 [0 0 -1 0 0 0 0];

internalField　　 uniform 129.448;

boundaryField
{
　　　 inlet
　　　 {
　　　　　　　　　 /*type　　　　　　　　　　　　　　　 zeroGradient;*/
　　　　　　　　　 type　　　　　　　　　　　　　　　 mapped;
　　　　　　　　　 value　　　　　　　　　　　　　　 uniform 2e-05;
　　　　　　　　　 interpolationScheme cell;
　　　　　　　　　 setAverage　　　　　　　　　 false;
　　　　　　　　　 average　　　　　　　　　　　　 2e-05;
　　　 }
　　　 outlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }
　　　 walls
　　　 {
　　　　　　　 type　　　　　　　　　　　 omegaWallFunction;
　　　　　　　 value　　　　　　　　　　 uniform 129.448;
　　　 }
　　　 sides
　　　 {
　　　　　　　 type　　　　　　　　　　　 empty;
　　　 }
}

nut.air

dimensions　　　　　 [0 2 -1 0 0 0 0];

internalField　　 uniform 0; 

boundaryField
{　　 
　　　 inlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }
　　　 outlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }　　　 
　　　 walls
　　　 {
　　　　　　　 type　　　　　　　　　　　 nutkWallFunction;
　　　　　　　 value　　　　　　　　　　 uniform 0;
　　　 }
　　　 sides
　　　 {
　　　　　　　 type　　　　　　　　　　　 empty;
　　　 }　 
}

p

dimensions　　　　　 [0 2 -2 0 0 0 0];

internalField　　 uniform 0; 

boundaryField
{　　　 
　　　 inlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }
　　　 outlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 fixedValue;
　　　　　　　 value　　　　　　　　　　 uniform 0;
　　　 }　　 
　　　 walls
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }
　　　 sides
　　　 {
　　　　　　　 type　　　　　　　　　　　 empty;
　　　 }
}

U.air

dimensions　　　　　 [0 1 -1 0 0 0 0];

internalField　　 uniform (0 0 0); 

boundaryField
{ 
　　　 inlet
　　　 {
　　　　　　　 type　　　　　　　　　　　　　　　 mapped;
　　　　　　　 value　　　　　　　　　　　　　　 uniform (9.39 0 0);
　　　　　　　 interpolationScheme cell;
　　　　　　　 setAverage　　　　　　　　　 true;
　　　　　　　 average　　　　　　　　　　　　 (9.39 0 0);
　　　 }
　　　 outlet
　　　 {
　　　　　　　 type　　　　　　　　　　　 zeroGradient;
　　　 }
　　　 walls
　　　 {
　　　　　　　 type　　　　　　　　　　　 noSlip;
　　　 }
　　　 sides
　　　 {
　　　　　　　 type　　　　　　　　　　　 empty;
　　　 } 
}

One thing more to consider: The velocity in x-direction is approximately 10m/s, the average k-Values seem to be in the order of 1 m²/s². This would result in turbulent velocity fluctuations with a variance of approx. 0.8 m/s. Even when seeing this velocity all the time (in ~68% of the time it should be less), the particles would only get once from top to bottom while flying through the domain.

-sorry nut I really don't get this point. I am new to CFD and forgive me for not understanding obvious things/asking silly questions.

[atul1018]

Dear Oswald,

I am not able to attach the profile plots (don't know why??). may bes ome server problem or something. If you need to see them let me know..I will try to attach them here or will send you by some other means.

Best Regards
Atul Jaiswal

[oswald]

-yes, I did try with stochastic dispersion model (stochasticDispersionRAS) too and I could not see major difference between gradient and stochastic dispersion. I am attaching the screenshot of particles at the end of simulation where I used stochastic dispersion model. In fact, with stochastic dispersion model i see even lesser number of particles near to lower wall.

Strange... There is one thing I realised just now: As the case is 2D, the gradient dispersion model behaves a little different:

// In 2D calculations the -grad(k) is always
            // away from the axis of symmetry
            // This creates a 'hole' in the spray and to
            // prevent this we let fac be both negative/positive
            if (this->owner().mesh().nSolutionD() == 2)
            {
                fac = rnd.scalarNormal();
            }
            else
            {
                fac = mag(rnd.scalarNormal());
            }

So in 2D the particles are allowed to move in both direction of grad(k). It looks like this was intended for axisymmetric cases, but might not make sense for planar symmetry?

-I am using mapped bc to get fully developed turbulent flow and my offset location is 0.067m downstream from inlet. Regarding scaling the k and omega, This time I turned the averaging off and run the simulation (the boundary conditions files are attached for reference) with stochastic dispersion model. I believe that this time I get fully developed flow at inlet (as per my knowledge: fully developed flow profile doesn't change w.r.t. space). I am attaching the fluid flow profiles at x=-0.1335 (inlet), -0.13, -0.1 and 0 (step location). From the profiles, you can see that they don't change as we move in x-direction. However, I am getting max. velocity of 10.41 m/s which should be 10.5 m/s (don't know why?). The no-slip condition is not satisfied at x=-0.1335 (inlet) but by x=-0.13 we can see the velocity at walls equal to zero (no-slip condition satisfied). Do you think that my understanding of fully developed turbulent flow is correct and the profiles I am getting is fully developed?

This sounds like now a fully developed turbulent flow is established. If the profile doesn't change along the flow, is seems okay. No need to attach the plots

-sorry nut I really don't get this point. I am new to CFD and forgive me for not understanding obvious things/asking silly questions.

Short and simple: The turbulent fluctuations are simply not high enough to push the particles far enough.


A last thing for now: You should first calculate the flow until it is steady and then inject the parcels. Maybe you can double the calculation time to 1s and change the SOI in the injection model to 0.5.

[atul1018]

Thank you so much for your answers.

Strange... There is one thing I realised just now: As the case is 2D, the gradient dispersion model behaves a little different.
So in 2D the particles are allowed to move in both direction of grad(k). It looks like this was intended for axisymmetric cases, but might not make sense for planar symmetry?

-yes the case is 2-D case. As you said the particle should move in both direction of grad(k), but I can not see my particles dispersing in span-wise direction (y-axis). If the dispersion model works fine then why not many particles are dispersed? Turbulent fluctuations are not big enough (~1m/s).

This sounds like now a fully developed turbulent flow is established. If the profile doesn't change along the flow, is seems okay. No need to attach the plots

-Thanks for confirming. At least I have now fully developed flow in the domain and I am sure about it.

Short and simple: The turbulent fluctuations are simply not high enough to push the particles far enough.

-Yes, it seems the turbulent fluctuation are not enough big. I am attaching screenshot (at the end of simulation) of the particle velocity (U) and turbulent fluctuation added to particle velocity (Uturb). From the screenshot it is also clear that most of the particles in the domain have UTurb ~1m/s. I don't know how can I get higher values of UTurb, so that significant dispersion occurs.

A last thing for now: You should first calculate the flow until it is steady and then inject the parcels. Maybe you can double the calculation time to 1s and change the SOI in the injection model to 0.5.

-The screenshots I attached are of the case where SOI = 0.5 and Simulation duration =1 sec. No improvement in particle dispersion is observed as you can see it from attached screenshot.




-One more thing: Meanwhile I also checked the convergence of my fluid field. As the case is transient, I was not sure how can I check the convergence of solution. I found this thread (Convergence in OpenFoam) and as suggested in thread, I plotted the initial residuals. From the attached residual plot you can see that initial residuals for U.air(x), U.air(y), k.air, omega.air falls below 10^-3. but the p has relatively higher value of residuals (`0.05). Is my solution converged? If not, how can I achieve the convergence?



-I am wondering if my kinematicCloudProperies dictionary has something wrong, which is causing this problem. I am attaching my kinematicCloudProperies dictionary here. Let me know if there is anything wrong or chance of improvement. I am consider two-way coupling and particle-particle interaction is neglected.



kinematicCloudProperties

solution
{
    active          true;
    coupled         true;
    transient       yes;
    cellValueSourceCorrection off;
    maxCo           0.3; 

    interpolationSchemes
    {
        rho.air             cell;
        U.air               cellPoint;
        mu.air              cell;
    }

    integrationSchemes
    {
        U               Euler;
    }

    sourceTerms
    {
        schemes
        {
            U           semiImplicit 1;
        }
    }
}

constantProperties
{
    rho0            8800;
    youngsModulus   1.3e5;
    poissonsRatio   0.35;
    constantVolume  false;

    alphaMax        0.99;

}

subModels
{
    particleForces
    {
        sphereDrag;
        
        gravity;
    }

    injectionModels
    {
    model1
    {
            type             patchInjection;
            patch            inlet;
            duration         0.5;
        parcelsPerSecond 33261;
            massTotal        0;
            parcelBasisType  fixed;
            flowRateProfile  constant 1;
            nParticle        1;
            SOI              0.5;
            U0               (10.5 0 0);
            sizeDistribution
            {
                type        fixedValue;
                fixedValueDistribution
                {
                    value   0.00007;
                }
            }

        }
    }

    dispersionModel stochasticDispersionRAS;

    patchInteractionModel standardWallInteraction;

    standardWallInteractionCoeffs
    {
        type rebound;
        e    0.97;
        mu   0.09;
    }

    surfaceFilmModel none;

    stochasticCollisionModel none;
    
    collisionModel none;    

    pairCollisionCoeffs
    {
        maxInteractionDistance  0.00007;

        writeReferredParticleCloud no;

        pairModel pairSpringSliderDashpot;

        pairSpringSliderDashpotCoeffs
        {
            useEquivalentSize   no;
            alpha               0.12;
            b                   1.5;
            mu                  0.52;
            cohesionEnergyDensity 0;
            collisionResolutionSteps 12;
        };
        
        wallModel wallSpringSliderDashpot;

        wallSpringSliderDashpotCoeffs
        {
            useEquivalentSize no;
            collisionResolutionSteps 12;
            youngsModulus   1e10;
            poissonsRatio   0.23;
            alpha           0.12;
            b               1.5;
            mu              0.43;
            cohesionEnergyDensity 0;
        };
        U     U.air;
    }
}

cloudFunctions
{
    voidFraction1
    {
        type            voidFraction;
    }
}

[oswald]

I don't think that there are major issues with your case setup. Why do you think that your results are not right?


The rise in p's initial residuals might come from the 2-way-coupling with the particle phase. Do you think the coupling is necessary?

[atul1018]

I don't think that there are major issues with your case setup. Why do you think that your results are not right?

-My case setup looks fine. Flow is fully developed and flow seems to be converged as initial residuals of all fluid parameters are below the 1*e-3 expect pressure. I do believe that my fluid flow field are absolutely correct. I compared the fluid flow profiles at several locations along the flow with measured velocity profiles and I am getting good match.


-But when I compare the particle velocity profiles at several locations along the flow (x/H=2,5,7,9,12) at the end of simulation. I am getting strange results. The simulated particle velocity and profiles are strange and almost no particle is found below the step (y/H=1). That's why, I suspect that turbulent dispersion is not happening properly. I am attaching the particle velocity profiles which I compared with literature (blue line is the simulated particle velocity).

The rise in p's initial residuals might come from the 2-way-coupling with the particle phase. Do you think the coupling is necessary?

-As particle mass flow rate is 10% of fluid mass flow rate (dispersed case), the coupling and no- coupling will not have any major effect on particle dispersion. because of less number of particles in the domain, particle-particle interaction is really not important and I haven't considered this (4-way coupling). I simulated the case with or without the coupling, still I cant find enough particles below the step. I also took particle at other time steps but every-time very less number of article are below the step.



-p is related to fluid phase and i don;t think coupling may have any impact on residuals of p. As my fluid velocity profiles are giving good match with measurement, I think the residuals are acceptable and my fluid-phase results are correct.


-I am getting strange results only for particle velocity profiles and really can't find the reason of discrepancy between simulated and measured particle velocity profiles.


Best Regards
Atul

[Msure]

Hello,

Have you tried to run it in 3D? Because sometimes the 2D condition will make the problem unphysical when I simulate some cases with OpenFOAM.

[atul1018]

Hello

Have you tried to run it in 3D? Because sometimes the 2D condition will make the problem unphysical when I simulate some cases with OpenFOAM

Yes , I tried with 3-D cases using symmetry bc in z-direction. Particle dispersion seems to be same as that of 2-D cases, no particle dispersion below the step at measurement locations.


Which bc you use to make 3-D cases. Using of symmetry bc to make 3-D case is correct?


Best Regards
Atul Jaiswal

[Msure]

Hello,

I am doing it. I found your thread and some papers today. Because I also need to use the backward case as a validation of Openfoam's DEM method. I will show my results to you in recent days and discuss my results with you.

[Msure]

Originally Posted by atul1018

Hello

Have you tried to run it in 3D? Because sometimes the 2D condition will make the problem unphysical when I simulate some cases with OpenFOAM

Yes , I tried with 3-D cases using symmetry bc in z-direction. Particle dispersion seems to be same as that of 2-D cases, no particle dispersion below the step at measurement locations.


Which bc you use to make 3-D cases. Using of symmetry bc to make 3-D case is correct?


Best Regards
Atul Jaiswal

Hello,

I am doing it. I found your thread and some papers today. Because I also need to use the backward case as a validation of Openfoam's DEM method. I will show my results to you in recent days and discuss my results with you.

[Msure]

Originally Posted by atul1018

Hello

Have you tried to run it in 3D? Because sometimes the 2D condition will make the problem unphysical when I simulate some cases with OpenFOAM

Yes , I tried with 3-D cases using symmetry bc in z-direction. Particle dispersion seems to be same as that of 2-D cases, no particle dispersion below the step at measurement locations.


Which bc you use to make 3-D cases. Using of symmetry bc to make 3-D case is correct?


Best Regards
Atul Jaiswal

And in another paper, the lagaragian method also lost some particle informtion in the lower part, and you can see the Euler method works better.

[Msure]

Originally Posted by atul1018

Hello

Have you tried to run it in 3D? Because sometimes the 2D condition will make the problem unphysical when I simulate some cases with OpenFOAM

Yes , I tried with 3-D cases using symmetry bc in z-direction. Particle dispersion seems to be same as that of 2-D cases, no particle dispersion below the step at measurement locations.


Which bc you use to make 3-D cases. Using of symmetry bc to make 3-D case is correct?

Best Regards
Atul Jaiswal

Also, I can not generate the mesh correctly using your BlockMeshDict, it seems you lost a face in the boundary. I just see that your g=9.8 is in the x-direction. I didn't check it in detail, is it right? Or you should set g in the y-direction.

[Msure]

Hi，

Please see the attachment. I got it right. The particles fell down. In fact, it is just a small problem. The gravity is in y-direction which is -9.81, but you set it in x-direction. I read the paper (Fessler et al), the paper did make me misunderstand the experiment set up. But after I tried it, I am sure now it is right to set gravity in y-direction

Regards,
Shuo

[atul1018]

Hello

Originally Posted by Msure

Please see the attachment. I got it right. The particles fell down. In fact, it is just a small problem. The gravity is in y-direction which is -9.81, but you set it in x-direction. I read the paper (Fessler et al), the paper did make me misunderstand the experiment set up. But after I tried it, I am sure now it is right to set gravity in y-direction

Shuo

I don't think the gravity in -y direction is right. If you look at the experimental set-up of Fessler & Eaton, the gravity is acting in direction of flow (setup is held vertically in order to avoid unintended settling in of particles). if you rotate the image the setup (anticlockwise), you will realize, the value of gravity should be +9.81 m2/s in +x direction. (as per geometry for numerical simulation). The conclusion is that gravity is acting in same direction of flow. So if you set the fluid velocity at inlet as (9.39 0 0) in +x direction, the gravity should also be (9.81 0 0) also in +x direction.

Here is the paper of Fessler & Eaton, read the numerical setup carefully and let me know your thoughts: https://citeseerx.ist.psu.edu/viewdo...=rep1&type=pdf

One more thing: Even if you set g=-9.81, I cant see, the particles well dispersed below the step @ measurement locations. The particles seems to be dispersed towards the outlet not at measurement locations.

Best Regards
Atul

[Msure]

Hello,

Originally Posted by atul1018

Hello



I don't think the gravity in -y direction is right. If you look at the experimental set-up of Fessler & Eaton, the gravity is acting in direction of flow (setup is held vertically in order to avoid unintended settling in of particles). if you rotate the image the setup (anticlockwise), you will realize, the value of gravity should be +9.81 m2/s in +x direction. (as per geometry for numerical simulation). The conclusion is that gravity is acting in same direction of flow. So if you set the fluid velocity at inlet as (9.39 0 0) in +x direction, the gravity should also be (9.81 0 0) also in +x direction.

Here is the paper of Fessler & Eaton, read the numerical setup carefully and let me know your thoughts: https://citeseerx.ist.psu.edu/viewdo...=rep1&type=pdf

One more thing: Even if you set g=-9.81, I cant see, the particles well dispersed below the step @ measurement locations. The particles seems to be dispersed towards the outlet not at measurement locations.

Best Regards
Atul

Yes. In that paper, it shows the setup is held vertically, but I think it is only due to the limit of the paper size so they draw the setup in the vertical direction. The paper didn't describe the setup clearly, unfortunately. Then I searched other papers that conducted almost the same experiment. The gravity is in y-direction. Please see the attachment. The paper is here:https://www.sciencedirect.com/scienc...01932288900754

Also, I found the tutorial about the case based on Openfoam (German OpenFOAM User meeting 2017 (GOFUN 2017)
Particle Simulation with
OpenFOAM),
you could see in the slides, it set gravity in y-direction.

Anyway, I will compare my results with the exp data to see if the comparision is well.

Regards,
Shuo

[atul1018]

Hello

Yes. In that paper, it shows the setup is held vertically, but I think it is only due to the limit of the paper size so they draw the setup in the vertical direction. The paper didn't describe the setup clearly, unfortunately. Then I searched other papers that conducted almost the same experiment. The gravity is in y-direction. Please see the attachment. The paper is here:https://www.sciencedirect.com/scienc...01932288900754

-In the original reference experimental setup of Fessler & Eaton, it is clearly written that the setup is held vertically (See 2.1, first paragraph first sentence: https://citeseerx.ist.psu.edu/viewdo...=rep1&type=pdf)

Also, I found the tutorial about the case based on Openfoam (German OpenFOAM User meeting 2017 (GOFUN 2017)
Particle Simulation with
OpenFOAM),
you could see in the slides, it set gravity in y-direction.

-I also had downloaded the presentation from that seminar but in my slides the gravity is showed to set in +x direction (see attachement).

Anyway, I will compare my results with the exp data to see if the comparision is well.

-Yes, you should compare the particle velocity profiles at measurement locations.


Best Regards
Atul Jaiswal