[edu_aero]

SOLVED!! 17-09-2015

Fluent is only able to report the mass flow of the Eulerian problem, so Fluent is not going to give you the information of the mass flow of liquid (Lagrangian problem).
If you want to get that value, you have to do it by yourself postprocessing the data and integrating around the particles.
I have done it through a compiled macro.
[2D simulation has been carried out in order to understand the problem, please read its description in message #8]

Hello to everybody!

I am writting here because I am having some issues with the DPM model in Fluent 15 simulating a 3D model.

It is the first time that I am working with a Discrete Phase Model. I am supposed to be simulating a fuel injection. But, because I am having some issues with the DPM model, I am just simulating it on a cylinder of diameter 6mm and length of 100mm without temperature changed in order to understand the model. The cylinder has just mass flow inlet, pressure outlet and wall as boundary conditions.

Characteristic of DPM:
Interaction with continuous phase
Unsteady Particle Tracking
Particle Time Step Size (s)= 0.0001
Step Lenght Factor= 5

The inlet mass flow rate is made of 0,23% 02 and the rest N2 and it has a value of 0.004 Kg/s.
I simulate the problem and it easily converges.
After it, the injection is defined taking into account stocastic phenomenous. The characteristics of the injection are the following ones:

Injection type: Cone, Angle: 30º, Number of streams: 500
Particle type: Droplet
Material: Methyl-alcohol-liquid (Desnity=780Kg/s)
Position[m]: (0, 0, 0.0005)
Diameter[m]: 0.0001
Velocity[m/s]: (0, 0, 10)

My problem is that the mass flow rate expected on the outlet:
Mass flow rate is called as M_

[ M_inlet(0.004Kg/s) + M_injection(0.0018Kg/s) = M_outlet ]
so M_outlet should be 0.0058 Kg/s

The solution is converged for a mass flow rate of 0.00411 Kg/s!

After, spending some time thinking about it. For me, it seems like the problem is coupled problem. I explain that.
s=Particle Time Step Size (s)
p=Density
D=Diameter
SUM= Sumatory of all particles
M_injection=(1/s)SUM[p*(D^3*4/3*pi)]

So the program is requesting more variables than needed,isnt it?
Or is it because the number of particles are used for stochastic purpose?

Postprocesing, I am able to see the particles and it seems like the path is the correct

I will appreciate some help. I started looking for information on ANSYS tutorials, after it on the Internet, and finally now I am reading books about the Discreate Phase Model. However it seems like an obvious mistake that I am not able to find.

[edoan]

Just a quick comment: are you sure all your particles that are injected are escaping at the outlet or are some being trapped or is the calculation aborted (max number of particle steps reached). When an injection is released during a DPM iteration a summary will be displayed of number of particles released, trapped, escaped etc.

[edu_aero]

Originally Posted by edoan

Just a quick comment: are you sure all your particles that are injected are escaping at the outlet or are some being trapped or is the calculation aborted (max number of particle steps reached). When an injection is released during a DPM iteration a summary will be displayed of number of particles released, trapped, escaped etc.

Firstly, I want to thank you the answer =)

I have just escaped, coalesced and shed particles.
Postprocessing, I draw the particles track and it is according to this. It can be seen how every particle come out by the outlet.

However postproccesing, in reports, fluxes, mass flow rate I select all the boundaries and the resaults are:

Inlet:0.004 Kg/s
Outlet: -0.00411 Kg/s
Wall: 0 Kg/s

In the screen is printed:
DPM Mass Source 0.00011

So, it seems like the mass flow rate of the ijection is the one that it does not fit.

Again, thank you very much for your answer, I really appreciate it!!

[`e`]

Instead of the cone injection type, try using the single particle injection method and check the mass flow rate (inlet versus outlet). If that works, then have a closer look at your settings for the cone type.

I'm not sure what you mean by this statement:

Originally Posted by edu_aero

So the program is requesting more variables than needed,isnt it?

The number of streams (say 500) is not the same as the number of particles. The DPM uses a parcel method where many particles are tracked in each parcel.

[edu_aero]

Originally Posted by `e`

Instead of the cone injection type, try using the single particle injection method and check the mass flow rate (inlet versus outlet). If that works, then have a closer look at your settings for the cone type.

I'm not sure what you mean by this statement:



The number of streams (say 500) is not the same as the number of particles. The DPM uses a parcel method where many particles are tracked in each parcel.

Thank u very much, 'e'.

I have already tried changing the type of injection to single and surface and the result (M-outlet-M_inlet) does not fit the mass flow of the injection, the difference is close to zero.

Thank u, I missunderstood the definition of number os streams. So then, Fluent decide the number of parcels in order to fit the equation written before, isn't it?
It does make sense to have a defined problem =)

Todat, I was trying by decreasing the mass flow ratio of inlet and injection, just to know if the bad resault has been because of the high velocity. But it is not working neither

[`e`]

Originally Posted by edu_aero

I have already tried changing the type of injection to single and surface and the result (M-outlet-M_inlet) does not fit the mass flow of the injection, the difference is close to zero.

If the difference is close to zero then those injection types are performing as expected.

Originally Posted by edu_aero

Thank u, I missunderstood the definition of number os streams. So then, Fluent decide the number of parcels in order to fit the equation written before, isn't it?

Fluent allocates the number of particles in each parcel based on the particle diameter, density and mass flow rate.

Originally Posted by edu_aero

Todat, I was trying by decreasing the mass flow ratio of inlet and injection, just to know if the bad resault has been because of the high velocity. But it is not working neither

What azimuthal start/stop angles are you using? According to the user's guide, the mass flow rate must be appropriate for the defined sector. Perhaps if you're only injecting particles in a portion of the cone, then the mass flow rate should be proportional.

[edu_aero]

Thank u again =)

Sorry, may be I didn't explain myself properly, the injection is performed on the point (0,0,0.0005), after inlet. So that, the difference between inlet and outlet should be just the injection flow rate.

What azimuthal start/stop angles are you using? According to the user's guide, the mass flow rate must be appropriate for the defined sector. Perhaps if you're only injecting particles in a portion of the cone, then the mass flow rate should be proportional.[/QUOTE]

I am using as start angle 0º, and final 360º. I didn't know that Fluent worked on that way. However it seems like that is not my problem... =(

[edu_aero]

Because of the difficulties that I had with the Discrete Phase Model, I changed my model to 2D.


I have a square of 6mm (height) x100mm (length) in 2D with around 15.000 hexagonal elements. I define an injection, and just changing the injection material changes the mass flow ratio of the injection. I don’t understand that, I have always thought that 1 kg. of iron weight the same that 1 kg. of wood jejeje.


I am using:
Energy equation
Viscous – Standard k-e
Standard Wall Fn; Species – Species Transport (Diffusion Energy Force, mix material jp8(imported and made of n2,h20, o2, co, co2, pjp8(I have already tried before in 3D with other materials and the result was not correct neither))
Discrete Phase.


Firstly, I converged the problem without DPM, with the following boundary conditions:
Inlet: Velocity 5m/s, [Turbulent Intensity 10%, Hydraulic Diameter 0.006m]. Temperature 300K, Species Mass Fractions, 0.23 of 02.
Wall: Typical conditions of a wall with no slip. Adding DPM wall-film with DPM model.
Outlet: Gauge Pressure 0 Pa, [Turbulent Intensity 10%, Hydraulic Diameter 0.006m]. Temperature 300K, Species Mass Fractions, 0.23 of 02. DPM escape condition.




After converging the simulation, I define the following DPM:
Iteration with continuous Phase
Iterations per DPM Iteration: 10
Unsteady Particle Tracking
Particle Time Step (s): 0.00025s
Number of Time Steps: 1
Max. Number of steps: 50000
Step Length Factor: 5
Physical Models (Stochastic Collision, Coalescence, Breakup)
About the injection:
Surface from the inlet
Particle type: Droplet
Material: It has been tested with different materials achieving different result
Diameter Distribution: Uniform
Evaporation Species: n2,h20, o2, co, co2, pjp8
Velocity [m/s]: (5,0)
Diameter[m]: 0.0001
Temperature[k]: 300
Start Time; Stop Time [s]: 0;100
Total Flow Rate [Kg/s]: 0.0001
Physical Models, Drag Law: Dynamic-drag.

I have carried the injection with different materials, only changing the material that was injected. The results of DPM mass flow ratio were the following ones (all in Kg/s):
ARGON

7,53E-05

FUEL OIL

2,19E-15

KEROSENE

8,99E-17

NITROGEN

9,43E-05

TOLUENO

7,84E-06

WATER LIQUID

6,40E-06

The only one that was close to the solution expected was Nitrogen, lower by a percent of 5.7%


I have made an Excel table in order to look for correlations between materials characteristics and the mass flow of injection. However I cannot see any correlation.


I will love to have some help about this model because I am really struggling with it.


Thank you very much for your consideration and sorry for the length of the message. However, I wanted to describe thoroughly the simulation.


Thank you very much

NEW

Continue making different simulations, I have enclosed the problem.
The mass flow that I obtain is only the mass flow of the injection that has been evaporated. So it makes sense according to the data of matirials mass flow exposed before.
I would love to know if someone knows why this happens. I clearly can see the injection by tracking particles on a graph.
https://www.dropbox.com/s/jomo9pubaj...CTION.png?dl=0

NEW 2

Finally, it seems like I have found the problem.
I have been using as DPM condition on the outlet'escaped'. However I don't know why but the particles that cross the surfaces are not taken into account when I make the difference of mass flow between inlet and outlet.
Nevertheless, if the condition on the outlet is trapped, everything works smoothly obtaining the expected results.
Now, I am able to continue working, I'd be glad if someone can explain me why it happens.
At the same time, I will be glad that this will be useful for someone in the future.

Thank you to 'e' and 'edoan' for your comentaries and interest.

[`e`]

Originally Posted by edu_aero

I have been using as DPM condition on the outlet'escaped'. However I don't know why but the particles that cross the surfaces are not taken into account when I make the difference of mass flow between inlet and outlet.
Nevertheless, if the condition on the outlet is trapped, everything works smoothly obtaining the expected results.
Now, I am able to continue working, I'd be glad if someone can explain me why it happens.

How are you calculating the mass flux of the particles at inlet and outlet? Particles that hit a boundary with type "escape" are removed from the simulation whereas "trapped" particles remain in the simulation. Perhaps the particle flux is not saved/accumulated in your method; therefore escaped particles are not counted but trapped particles are counted.

[edu_aero]

Originally Posted by `e`

How are you calculating the mass flux of the particles at inlet and outlet? Particles that hit a boundary with type "escape" are removed from the simulation whereas "trapped" particles remain in the simulation. Perhaps the particle flux is not saved/accumulated in your method; therefore escaped particles are not counted but trapped particles are counted.

Firstly, I want to grateful your help again =) and telling you that I am sorry for taking that long to answer. Here, where I am, weekend is Friday and Saturday =).

I am calcultaing the mass flow by a monitor, selecting as a report type mass flow rate and then the surfaces (outlet and inlet). I do it in order to use it as a convergence criteria.

I thought the same that you have just said, that for some reason the particles that escape are not saved.

However I can't see the point why the program is developed on that way or how I will be able to change.

Now, I want to see the differences between the boundary condition escape and trapped. I hope that it is not crucial for getting an accurate solution. Nevertheless, I think that it will have some influence, so I have to quantify that influence and making it as little as possible or learning how to save the data about the particles that escape.

This is my new step, however at least now I can achieve to get some data =)

Thank you very much

[`e`]

Particle trajectory calculations are terminated for both the escaped and trapped DPM boundary conditions. There shouldn't be any difference in effects on the fluid unless the particles evaporate or there's combustion (mass is transferred to the surrounding fluid). Remember that the DPM treats particles as point masses and therefore the trapped particles don't occupy volume in the domain.

[edu_aero]

Originally Posted by `e`

Particle trajectory calculations are terminated for both the escaped and trapped DPM boundary conditions. There shouldn't be any difference in effects on the fluid unless the particles evaporate or there's combustion (mass is transferred to the surrounding fluid). Remember that the DPM treats particles as point masses and therefore the trapped particles don't occupy volume in the domain.

Just in case this will be useful for someone someday, I want to document everything properly adding the following information. According to some manual on the Internet (url attached), trap boundary condition is defined as:
The trajectory calculations are terminated and the fate of the particle is recorded as “trapped”. In the case of evaporating droplets, their entire mass instantaneously passes into the vapor phase and enters the cell adjacent to the boundary. See Figure 24.25: “Trap” Boundary Condition for the Discrete Phase. In the case of combusting particles, the remaining volatile mass is passed into the vapor phase.
Figure 24.25: “Trap” Boundary Condition for the Discrete Phase
https://www.sharcnet.ca/Software/Ans...disp_boundtrap



I am trying to qualify the difference of evaporization between two different models. So, for me evaporization is the purpose of this study.


The problem that I am facing now is every particle on the outlet get evaporated.
I have tried making the difference of mass flow ratio, between inlet and a surface close to the outle, but not the outlet. However, it happens exactly the same than with the escape boundary condition, that particles are not stored and then not taken into account in order to make the difference between inlet and new outlet.


So, I am thinking how I can make Fluent to store and recognize the particles, and be able to accurately make the different between inlet and outlet.

[edu_aero]

I am checking on the Internet, and I think that the best solution for the problem it would be to change the code of the boundary condition according to the website attached.

http://www.cfd-online.com/Forums/flu...pm-bc-udf.html

However, I have never programme for Fluent (it doesn't seem difficult, similar to C). So, this can be a tricky solution for me.
I want to ask if someone knows if I can change the code of the boundary condition or do I have to programme the whole function by myself? Because the difference of work it is not insignificant.

Nevertheless, I think that it is too complicated for a solution that it is suppose to be widely used. I mean, one of the most popular ways of controlling the convergence with DPM model, it is that the mass flow ratio of inlet + injection = outlet. So, there has to be an easier way.

[`e`]

If your model requires evaporation (and the flux monitor isn't working the way you'd like) the best way forward is to have a custom DPM boundary condition (DEFINE_DPM_BC). Perhaps try and escape the particles (return PATH_END) and save the mass flow rates in user-defined memory on the outlet faces (sum the flux at the end of each time step or on demand).

[edu_aero]

Tomorrow, I will speak with my a professor about it. I will try to not get into macros by the moment.

However, for other times or just in case if I have to programme the boundary condition by myself, what sadly is likely.
Can I change the Fluent boundary condition? Is it allow to the user to get inside the code in order to modify it?

[`e`]

I don't believe you can access the source files directly (Fluent isn't open source), but have a read of the UDF manual because all the details you need are there.

[edu_aero]

I have been taking to the professor in charge of this experiment and finally I got the problem.
I am monitoring the difference mass flow rate between the inlet and the outlet. With that, obviously (stupid me!!) the difference is made only taking into account the flow, not the liquid, as doptlets.

So, that I have to calculate the mass of the droplets when they cross the outlet, and then everything should make sense.

[edu_aero]

I am struggling to calculate the mass of the droplets at the outlet. Does someone know how to do it? I will appreciate a guidelines about it
Because the mass flow takes into account only the mass of gas.
Thank you very much before hand

[`e`]

The P_FLOW_RATE macro returns the flow rate of a parcel in kg/s. Have you tried writing the UDF I mentioned earlier?

[edu_aero]

Originally Posted by `e`

The P_FLOW_RATE macro returns the flow rate of a parcel in kg/s. Have you tried writing the UDF I mentioned earlier?

I have not used UDF yet. I have just having a look of it, and it seems more complicated than I thought.
I am going to try to calculate it, by hand or by matlab exporting the data. But for that as I told u, I need some parameters that I don't know how to get them without getting into macros (it would take some days to learn it).

Becuase [Kg/s(droplets)]= SUM(from_n=1:k([Droplet_density_n]*[Droplet_volumen_n]) / Time(related with number of droplets)

The only problem that I have it is getting the data from Fluent depending on time. I have already export the particles track to Matlab (where there is the density and diameter), the problem is that there is not dependence with time. I mean, the data it is just for a determinated time