[Sereff]

Hi everyone,

I am trying to implement patchFlowRateInjection for a DPM simulation on a boundary flow and I would like to inject some particles ramdomly into the domain. However there is really not a whole lot on how to setup the injectionModel{} in the kinematicProperties dictionary other than the source files. I have modified the kinematicProperties dictionary from the tutorial case but its giving the follwoing ERROR message.

T--> FOAM FATAL ERROR: 

    request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are
3(phi.air alphaPhi.air alphacf)

However I DO have phi.air file in my /0/ folder. After some digging, it seems that this ERROR message appeared when executing kinematicCloud.evolve(), line 94 of DPMFoam.C. After some further searching, I found this post, https://bugs.openfoam.org/view.php?id=1717 reporting an issue of some boundary conditions do not support names other than "phi". But I doubt this was the issue since in my ERROR message it explicitly mentioned "phi.air" is the one that is correct.

Does anyone have idea on how to solve this issue? Following is my the injectionModels{} part of the kinematicProperties dictionary file.

injectionModels
    {
        model1
        {
            type            patchFlowRateInjection;
            patch           inlet;
            SOI             0;
            duration        0.5;

            massTotal           0.1;    // total mass to be injected (kg)
            parcelBasisType     fixed;  // options of representing particles.(fixed, number, mass)
            parcelsPerSecond    10;

            nParticle           10;     // number of particles to be injected
            concentration       0.6;    // parcel concentration in fluid ???
            parcelConcentration 10;
            //positionsFile   "kinematicCloudPositions";
            //U0              (0 0 0);
            sizeDistribution
            {
                type        fixedValue;
                fixedValueDistribution
                {
                    value   0.0025;
                }
            }
        }
    }

[ybapat]

The injection is looking for default flux field phi as no flux field is provided. Check if injection provides options to specify flux field name then you can specify flux field name as phi.air.

[Sereff]

Hi ybapat,

Yes, i tried your advise and included phi option in injectionModels{} and it fixed the problem. Apparently having phi.air in /0 folder is not enough and the user has to specify it in the injectionModels{} as well.

For those who are having similar issues on patchFlowRateInjection, I have the following injectionModels options to make it run, with U.continuousPhaseName, phi.continuousPhaseName, p, k.continuousPhaseName and nut.continuousPhaseName (LES kEqn model) in /0 folder,

injectionModels
    {
        model1
        {
            type            patchFlowRateInjection;
            patch           inlet;
            SOI             0;
            duration        0.5;

            massTotal           0.1;    // total mass to be injected (kg)
            parcelBasisType     fixed;  // options of representing particles.(fixed, number, mass)
            parcelsPerSecond    10;
            nParticle           10;     // number of particles to be injected
            concentration       0.6;    // parcel concentration in fluid ???
            parcelConcentration 10;
            phi                 phi.air;
            sizeDistribution
            {
                type        fixedValue;
                fixedValueDistribution
                {
                    value   0.0025;
                }
            }
        }
    }

[atul1018]

Hey Sereff


I wanted to use the patchFlowRateInjection model for my case. I tried to set up the parameters for it but I am not able to get particles injected. I guess, I don't provide correct inputs as I really don't understand the meaning of certain keyword, especially the keyword "concentration" and parcelConcentration", can you please help me to understand the injection model?


Best Regards
Atul

[Sereff]

Hi atul1018,

Sorry for the late reply. It has been a while since I last worked on DPMFoam and particle injuction model. Did you try the setup I provided in the thread, with different parameters of course? Also, may I see your setup file for injection model?

To answer your question, as far as I remember,

concentration

> controls the distribution of parcel injection rate over a period of time. 
> So by setting it up to 1.0 means that the injection rate is uniform over 
> the injection period.

parcelConcentration

> is based on local volumetric flow rate. And this is what actually controls 
> how much/fast parcels are injected.

As I said, it has been a very long time since I last worked with DPMFoam so take my answer with a grain of salt. I hope it is helpful for you.


kind regards,

[atul1018]

Hello


here you can find the settings I provide for my patchFlowRateInjection model:

injectionModels
    {
        model1
        {
            type            patchFlowRateInjection;
            phi              alphaPhi.air;
            patch           inlet;
            duration        1;         
            massTotal       5.257e-3; //won't be considered as parcelBasisType is fixed
            parcelBasisType fixed;
            nParticle       1; //in each parcel there will be only one particle
            SOI             0;
            concentration 1;
            parcelConcentration 77515609;
            sizeDistribution
            {
                type        normal;
                normalDistribution
                {
                    expectation 6.82e-5;
                    variance    1.09e-5;
                    minValue    3.55e-5;
                    maxValue    10.09e-5;
                }
            }
        }
    }

I looked into the source code of the model and I also thing the concentration keyword determines temporal variation of particle injection and setting it to 1 means the injection rate won't change over time. So the parcelConcentration is the term which one needs to calculate for this model, which in number of particles (or parcels) in 1 m3 of fluid flow in 1 sec.


Best Regards
Atul