[walid abou hweij]

Hello fluent users,

Currently I am working on Discrete Phase Modeling (DPM) and I am encountering few problems. I appreciate it if you can help.

My case is steady continuous flow with steady particle injections, one way coupling with no interactions.

1. I am using surface type injection from inlet, however, the number of particles is restricted by the number of meshed cells at the inlet (no specified number of streams like point or group injection types) . Can I increase the number of particles without changing mesh density?

2. I would like to display contours of the particle distribution on a 2 D plane; is their a method to do this?

3. How can I plot the residence time distribution at outlet knowing that my study is steady bulk/ continuous flow and steady particle injections?

Thanks in advance

[walid abou hweij]

Any answer please it is urgent !!

[`e`]

Originally Posted by walid abou hweij

1. I am using surface type injection from inlet, however, the number of particles is restricted by the number of meshed cells at the inlet (no specified number of streams like point or group injection types) . Can I increase the number of particles without changing mesh density?

Not with the surface injection type, use an injection file instead.

Originally Posted by walid abou hweij

2. I would like to display contours of the particle distribution on a 2 D plane; is their a method to do this?

The particles are tracked in the Lagrangian reference frame, how are you expecting Fluent to create the contours?

Originally Posted by walid abou hweij

3. How can I plot the residence time distribution at outlet knowing that my study is steady bulk/ continuous flow and steady particle injections?

You could write a boundary condition UDF for DPM where the particle residence time and location are saved to a text file.

[walid abou hweij]

Thanks for your reply.

What i need to display on a 2 d plane is the particle location not the contours of velocity or anything else. Do you have an idea how to plot them ?

[MetricDevice]

Originally Posted by walid abou hweij

1.Can I increase the number of particles without changing mesh density?

2. I would like to display contours of the particle distribution on a 2 D plane; is their a method to do this?

3. How can I plot the residence time distribution at outlet knowing that my study is steady bulk/ continuous flow and steady particle injections?

1) You could use the Discrete Random Walk - Model
2) Nope
3) Create a sample at the outlet and import the data into MS Excel

[walid abou hweij]

Thanks for your reply.

I am working with laminar flow not turbulent flow so I can't use the RWM . Do you suggest another method to increase number of injections from the surface independent of mesh ?

Regarding the 2 d plane, how could I display how the particle poaitions are changing as they move in the pipe. In other words how can i see the effect of bortices on the particle positions?

Regards

[walid abou hweij]

Vortices not bortices "wrong typing"

[MetricDevice]

Vortices in completely laminar flow? Sounds strange to me...

[`e`]

Originally Posted by walid abou hweij

What i need to display on a 2 d plane is the particle location not the contours of velocity or anything else. Do you have an idea how to plot them ?

Plot the particle positions via Results > Graphics > Particle Tracks and orient the view to the plane. Note: all particles are shown, not one "plane" of particles, because a plane would intersect no discrete particles (simulated as point masses in DPM).

Originally Posted by walid abou hweij

I am working with laminar flow not turbulent flow so I can't use the RWM . Do you suggest another method to increase number of injections from the surface independent of mesh ?

As pointed out earlier, I recommend you use an injection file.

Originally Posted by walid abou hweij

Regarding the 2 d plane, how could I display how the particle poaitions are changing as they move in the pipe. In other words how can i see the effect of bortices on the particle positions?

As above and save figures at each time step. Or save particle positions to files and visualise with another program.

Originally Posted by MetricDevice

Vortices in completely laminar flow? Sounds strange to me...

Vortices can occur in laminar flow, here's a discussion.

[MetricDevice]

You are right, sorry.

Vortices (which can be present in laminar flow) and turbulent eddies are two different phenomena, I've mixed that up.

By the way:
You can filter your particle tracks using a mesh coordinate. It is not possible to view the tracks in a 2D plane but in this way you can isolate the results a bit.

[walid abou hweij]

Once I save the position of particles, which program can plot the particle position and visualize them?

[CeesH]

for point 2, you could make a UDF which loops over all particles, and adds a count in a user defined memory when a particle is registered.
Below should do the trick:

DEFINE_ADJUST(meancounter,d)
{
Injection *I;
Injection *dpm_injections = Get_dpm_injections();
Particle *p;

Domain *domain;
cell_t cell;
Thread *tr;

domain=Get_Domain(1);

// clean instantaneous
  thread_loop_c (tr,domain)
{
 begin_c_loop (cell,tr)
         {

C_UDMI(cell,tr,0) = 0;


         }
       end_c_loop (cell,tr)
}




loop(I,dpm_injections)
{
loop(p,I->p)
{
C_UDMI(P_CELL(p),P_CELL_THREAD(p),0) +=1;
}
}
}

Now, you can just make a plot-plane like you would do for any parameter. Do keep in mind that, unless no. particles >>> no. cells, the results will be highly noisy. If your simulation is steady on average (i.e. you expect no changes in the mean particle distribution in time), you can average over a large number of instantaneous fields to get an idea of the particle distribution. May be easiest to do that in an external program, but you can also add a second UDM:

  thread_loop_c (tr,domain)
    {
       begin_c_loop (cell,tr)
         {


C_UDMI(cell,tr,1) = ((C_UDMI(cell,tr,1)*NS)+ C_UDMI(cell,tr,0))  /(NS+1) ;    

         }
       end_c_loop (cell,tr)

This would keep a moving average of the number of particles for each cell, with NS the averaging window size (in number of timesteps - this is for fixed timestepping).

[walid abou hweij]

I am very thankfull for your help.I will check thant and see what I will get .

Regards

[kattulanitin]

Hi all,
1.) I have a problem in which I am injecting nanometer-sized particles into a
pipe with water as fluid and giving the heat flux boundary condition on the
wall but there is no interaction with the continuous phase although the
option of interaction with continuous phase is selected.
2.) I am not sure, How to give volume fraction of nanoparticles?

[alburkatyhasan@yahoo.com]

Hello, For injection of the particles, I am using surface type injection from the inlet to produce the most accurate solution; however, the number of particles is limited by the number of meshed cells at the inlet. The particle tracking scheme utilized within the injection system thus allowed the use of the previously mentioned two-way step coupling. So, my question is, how do get particle numbers in the parcel when I use surface type injection from the inlet? Is there a way to use the number of particles in the inlet with the surface type injection? thank you.