access to velocity gradient for Lagrangian paticles
Dear all
I am kind of get stuck at finding the velocity gradient at a particular position for the Lagrangian particle dynamics. My question is how I should calculate the velocity gradient if I have the velocity vector "U_". Is there some utility like "curl" that I can use to calculate it? Thank you very much. 
Hi jie
It seems not. And it seems that the gradient is only reasonable for a Euler field. A possible way is calculating the gradient from an Eulerian field converted from particle lagrangian velocity field Junwei 
Quote:

Oh sorry.
I am confused last night. Just use fvc::grad(U_) and make an interpolation on the particle location like this volTensorField gradU=fvc::grad(U_); autoPtr<interpolation<tensor> >gradUInterpolator_ = interpolation<tensor>::New(interpolationSchemes, gradU); //interpolationSchemes is a word for assigning interpolation schemes("cell", "cellPoint" or "cellPointFace") tensor gradUatPoint = gradUInterpolator>interpolate(ball.position(), ball.cell()); If the gradient vary little across the space, interpolation can be neglected, and use the gradient at the cell center to represent the gradient at the particle location. In this situation, just use the following code tensor gradUatPoint =gradU[ball.cell()]; ball is the particle defined in OpenFOAM. Hope this helps regards, Junwei Su 
Sampling tool for Lagrangian Particles
Dear su_junwei
Is there a sampling tool for Lagrangian particles ? i.e, I would like to collect particle statistics such as mean particle size, mean particle velocity etc., at an arbitrary surface inside the domain DURING the simulation ? I saw from another post that there is an utility called functionObject for doing this for Eulerian fields. I am looking for the lagrangian particles. Please let me know Thanks Vaidya 
Hi Vaidya
I don't think there is a tool in OpenFOAM which can sample particles on a arbitrary surface in the solution domain. I didn't find one. Actually, at a certain time point, there may be no particles hitting the surface concerned exactly. If you want to get a distribution(of particle size, velocity, etc) on a certain plane, I think you'd better make a conversion from Lagrangian field to Eulerian field and then use the sampling tool in OpenFOAM. The sample utility in OpenFOAM is located at ../OpenFOAM/OpenFOAM1.6/src/sampling Regards, Junwei 
Thanks Sujunwei. I will keep looking. Hopefully the developers Hrvoje Jasak or Henry Weller might have some idea. But unfortunately no body else seems to know
Thanks Vaidya 
Quote:
I am sorry about the confusion caused, the "U_" is the parcel velocity and it is a vector but not a vector field. Hence, I got some error complaining about "volTensorField gradU=fvc::grad(U_);" I assume that maybe I could calculate the velocity gradient with the velocity filed U and interpolate the velocity gradient at the parcel position. Thanks a lot 
Hi Jie
What force do you want to calculate for a particle, I haven't encountered a force for granular flow. Are you trying to implement a meshless method? I usually make a conversion from the lagrangian field to euler field when calculating the Euler properties of granular fields. If you don't want a conversion, you can search all the particles around the particle concerned, calculate the gradient and do a average. This is common in meshless method, the formulation can be found in text book about meshless method. Regards, Junwei 
Hi JunWei
I am trying to calculate the drag and lift force acting on the particle so that I need the velocity gradients from the Eulerian field at the position of the particle. I will try to create a volVectorField GradU that contains all the velocity gradients and interpolate them on to the position of the particle. One quick question about the createFields.H: Info << "Reading field U\n" << endl; volVectorField U ( IOobject ( "U", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); It creates and initialises the volVectorField U and U is calculated from other mechanisms, right? So I can just do the followings to create GradU? Info << "Reading field GradU\n" << endl; volVectorField GradU ( IOobject ( "GardU", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); However, there are 9 components of the velocity gradients. Should I create and initialise each of them as GradU1, GradU2 and etc? Or should I use the "voltensorFields"? volTensorField gradU(fvc::grad(U)); I am pretty new to OpenFOAM so I am still learning myself. Thanks 
Quote:
Hi Jie you can do it like the following code (you don't have to initialize it using the file) volTensorField GradU ( IOobject ( "GardU", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), fvc::grad(U) ); PS: Don't forget recalculate gradU before using it. Regards,Junwei 
That means at each point of the tensor field of GradU, it should have 9 velocity gradient components as GradU.xx(), GradU.xy(), GradU.xz() ...?

exactly
Junwei 
Hi JunWei
I managed to get gradU calculated and updated during the simulation. However, I have problem to access gradU. All my particle dynamics is defined in a file called "mySolidParticle.C". It gives some error of "mySolidParticle.C:83: error: ‘gradU’ was not declared in this scope" when I tried to compile my solver after I added in the following code: autoPtr<interpolation<tensor> >gradUInterpolator_ = interpolation<tensor>::New(cell, gradU); How should I access the tensor field gradU other than the main "SOLVER.C" (SOLVER.C contains the main mechanism for solver)? Thank you 
Hi Jie
You don't have to declare the gradU in createField.H. You just get the value where you use it. In your case, declare it before the interpolator for instance like this volTensorField gradU=fvc::grad(U_); autoPtr<interpolation<tensor> >gradUInterpolator_ = interpolation<tensor>::New(cell, gradU); If you U_ is not accessible. you can lookup it through ObjectRegistry using the the function const volVectorField &U=[db or simular, you can get ObjectRegistry].lookupObject<volVectorField>("U"); you can also lookup gradU, if it is declared elsewhere createFields.H for instance. const volTensorField & gradU=[db...].lookupObject<volTensorField>("gradU"); Regards, Junwei 
Thanks JunWei
I will give the lookup it through ObjectRegistry a try. 
Hi JunWei
Now I am trying to write out the gradU for each particle. So I add "gradU.write();" in the "solidparticleIO.C". This should create a file at /xxx/lagrangian/defaultCloud/gradU where xxx is the time step at which OpenFOAM output the data. At /xxx/lagrangian/defaultCloud/, there are files of d, positions, U, gradU where d is the diameter of the particles, position is the locations of the particles, U is the velocity at the location of the particles, gradU should be the velocity gradients at the location of the particles. In my d and U fields, they contain the corresponding information of all the particles in the flow field. However, it only contains the velocity gradients information for one particle at the location where it releases the particle in the flow field in gradU. Would you have any idea about this? 
how to set correct mass flow rate for lagrangian particles ?
Dear Junwei
I am running a simulation where a simple nozzle is injecting compressible gas + solid particles jet into an open atmosphere. I am using OF 1.6.x I know the mass flow rate of the particles, density of the particles and the particle diameter distribution from the experiments. I am using the patchInjection option to inject particles from the inlet patch. The code works without a problem But I am not quite sure how to set the mass flow rate of the particles correctly in the kinematicCloud1Properties file My simple question is this: Can you please tell me what is the relationship between parcelsPerSecond, massTotal, volumeflowRate, SOI and duration ? Please help me Thanks Vaidya 
Quote:
gradU=fvc::grad(U) ; regards,Junwei 
Quote:
The meaning of these keywords may be parcelsPerSecond: The total number of particles should be injected a second after start starttime of Injection(SOI) massTotal: the total mass of particles should be injected between SOI and SOI+duration. volumeFlowRate: the total volume of the particles should be injected a second after SOI SOI: start of injection duration: The injection time segment. Injecting particle from SOI to SOI+duration regards,Junwei 
All times are GMT 4. The time now is 21:50. 