CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Defining Continuous Fluid's mass Flow Rate (http://www.cfd-online.com/Forums/cfx/133516-defining-continuous-fluids-mass-flow-rate.html)

brahmarishiraj April 16, 2014 05:25

Defining Continuous Fluid's mass Flow Rate
 
I am trying to model atomization of water in a venturi.
In general, when I define air and water as continuous fluid (or water as dispersed fluid) I am able to define the mass flow rates of air and water separately under "fluid value" tab.
However, when I define water as particle transport fluid, I am not able to define mass flow rate of air. In "fluid values" tab I just see water.

Plz suggest.

ghorrocks April 16, 2014 07:35

First of all - are you sure you are using the correct physical model? What are you trying to model? It sounds like water droplets in air which get atomised and evaporate. Is this correct? In that case this is a multiphase (gas and liquid) and multicomponent (water vapour and air. Is this what you have modelled?

brahmarishiraj April 16, 2014 11:56

Quote:

Originally Posted by ghorrocks (Post 486465)
First of all - are you sure you are using the correct physical model? What are you trying to model? It sounds like water droplets in air which get atomised and evaporate. Is this correct? In that case this is a multiphase (gas and liquid) and multicomponent (water vapour and air. Is this what you have modelled?


You are right in saying that it is multiphase. I am trying to model atomization but not evaporation.

ghorrocks April 16, 2014 19:45

OK, so your model is just multiphase. There is no mass transfer in the water from liquid to vapour.

I assume you are referring to if you make water a particle transport fluid in the domain tab, when you go to the inlet boundary condition you set the mass flow rate for the continuous phase, but you cannot find the mass flow rate for the particle phase.

Isn't it simply under Boundary Condition name/Fluid Values/Particle Behaviour and Select Define Particle Behaviour - then you define the particle mass flow rate.

brahmarishiraj April 16, 2014 22:47

Quote:

Originally Posted by ghorrocks (Post 486593)
OK, so your model is just multiphase. There is no mass transfer in the water from liquid to vapour.

I assume you are referring to if you make water a particle transport fluid in the domain tab, when you go to the inlet boundary condition you set the mass flow rate for the continuous phase, but you cannot find the mass flow rate for the particle phase.

Isn't it simply under Boundary Condition name/Fluid Values/Particle Behaviour and Select Define Particle Behaviour - then you define the particle mass flow rate.


Thank you for the reply.
I am sorry if I was not clear earlier.
In "default domain" I defined air as continuous phase and water as particle transport fluid.
Now, i defined one of the faces of geometry as "inlet" boundary and renamed it as "airinlet", i want to make it inlet for air (water is to be injected from other face of geometry).

when i double click "airinlet", under "fluid values" i see only "water", air is not there in the list. Now, in the same boundary (i.e Boundary: airinlet) if i define "mass flow rate" under "boundary details" tab, this mass flow rate would be for air or water??
I guess it would be water as only water is shown in list in "fluid values".

Kindly suggest.

Opaque April 17, 2014 00:15

Here is what the documentation states for the Fluid Values tab

Quote:

14.2.3. Boundary Fluid Values Tab
The Fluid Values tab for a boundary condition object is used to set boundary conditions for each fluid in an Eulerian multiphase simulation and each particle material when particle tracking is modeled.

The Boundary Conditions list box contains the materials of the fluid passing through the boundary condition. Selecting a material from the list will create a frame with the name of the material and properties available to edit. These properties are detailed in the following sections.
Your setup only contains a single Eulerian phase among Continuous Fluid, Dispersed Fluid and Dispersed Solid; therefore, your simulation qualifies as single phase plus a single particle transport model, i.e. it is not a Eulerian multiphase simulation. Consequently, the only fluid value available in the Fluid Values tab will be for the particle fluid (water in your case).

Hope the above helps,

brahmarishiraj April 17, 2014 03:08

Quote:

Originally Posted by Opaque (Post 486610)
Here is what the documentation states for the Fluid Values tab



Your setup only contains a single Eulerian phase among Continuous Fluid, Dispersed Fluid and Dispersed Solid; therefore, your simulation qualifies as single phase plus a single particle transport model, i.e. it is not a Eulerian multiphase simulation. Consequently, the only fluid value available in the Fluid Values tab will be for the particle fluid (water in your case).

Hope the above helps,


Thank you very much for the reply.
I am sorry but does it mean that I can not specify the mass flow rate for continuous fluid i.e. air in my case?
Plz suggest.

ghorrocks April 18, 2014 22:59

So from what I understand of your setup you set up the mass flow rate of the continuous phase is the normal place you define mass flow rates for inlet boundary conditions, and you define the flow rate of the particle phase at the boundary on the3 fluid tab.

Does that answer your question?

brahmarishiraj April 20, 2014 02:05

Quote:

Originally Posted by ghorrocks (Post 486954)
So from what I understand of your setup you set up the mass flow rate of the continuous phase is the normal place you define mass flow rates for inlet boundary conditions, and you define the flow rate of the particle phase at the boundary on the3 fluid tab.

Does that answer your question?

Dear Glen Horrocks,

I could not understand your last post fully.
I have attached some snapshots.
In my geometry, i want to define one boundary as air inlet boundary.
in "airinlet" boundary, i have defined a mass flow rate of 0.2 kg/s, however, in the same "airinlet" boundary, under "fluid values" tab, i see only "water", kindly see in the attachment.

My question is this 0.2 kg/s of mass flow rate is of air or water?

ghorrocks April 20, 2014 07:15

Is the 0.2kg/s air or water or both?

The answer is air or air/water mix. It should not matter. One of the fundamental assumptions of the lagrangian particle tracking approach is that the volume fraction/mass fraction of the particle phase is small, and therefore is insignificant compared to the continuous phase. This means the mass flow rate is of the continuous phase, but the particle phase must have a very small flow rate which does not significantly affect the total mass flow rate.

brahmarishiraj April 20, 2014 09:38

Quote:

Originally Posted by ghorrocks (Post 487112)
Is the 0.2kg/s air or water or both?

The answer is air or air/water mix. It should not matter. One of the fundamental assumptions of the lagrangian particle tracking approach is that the volume fraction/mass fraction of the particle phase is small, and therefore is insignificant compared to the continuous phase. This means the mass flow rate is of the continuous phase, but the particle phase must have a very small flow rate which does not significantly affect the total mass flow rate.

Thank you Glenn,

Will proceed with your words.

ghorrocks April 21, 2014 00:28

Sounds good. The other side of my comment is that if the particle volume flow rate is a significant proportion of the continuous phase volume flow rate then the particle tracking is not appropriate for your model. It is a fundamental assumption of the approach.


All times are GMT -4. The time now is 09:07.