[rakadit]

Dear Friends,

I am modeling multiphase flow of water and air using ANSYS FLUENT Eulerian multiphase model. please tell how ansys is calculating derived parameter like dynamic pressure in a multiphase problem i.e how it is taking into account volume fractions inot account at a point .For example if at a point water has volume of fraction as .65 and air as .35, how derived properties are calculated with these VOF.

thanks in advance,

Rakesh

[vinerm]

Fluid properties are based on volume fractions. For any property in a liquid-gas system, property used in conservation equation is , where represents volume fraction of phase .

[rakadit]

Thanks Mr. Vineram once again for the reply.
But my doubt is still pending. In eulerian multiphase model, water and air are separately modelled. The relation which you have shown will be useful for the cumulative effect of two phases at a point.Kindly help .
Thanks,
Rakesh

[vinerm]

In your previous post you asked how these were calculated for VOF (Do note VOF is also an Eulerian model). As far as Euler-Euler model is concerned, there is no such requirement, however, if required, the formulation will be same, e.g., for mixture turbulence model.

[rakadit]

Thanks once again.

I think ,I am not able to put across my point clearly. I once again put my query like this:
I am modeling water like pseudo fluid and air gravity flow using multiphase Eulerian model with ANSYS Fluent software. The flow is considered laminar. At a certain point of the flow, the values of different parameters are like this (actual values):
Secondary fluid (water like )
Density=445 kg/m3
VOF=0.8
velocity=10.31 m/s
Dynamic pressure=23.69 kPa (agrees with 1/2 *density* vel^2 relation)
Primary fluid (air)
Density=1.22 kg/m3
Velocity=5.15 m/s
VOF=0.2
Dynamic pressure=32.54 Pa (Not agrees with 1/2 *density* vel^2 relation)
why the value of dynamic pressure of air is double of the expected value? My question is how VOF is correlated with dynamic pressure. Can you please explain specifically with reference to the given values?
with regards,

Rakesh

[vinerm]

Where are you measuring these values? Are these values averaged over some zone?

Dynamic pressure is not directly affected by volume fraction.

[rakadit]

Thanks for the quick response.

The values are not measured but simulated values and extracted through CFD post. Fluid is flowing down a channel with gravity. Air is atmospheric around the dense fluid. Both air and water phase properties are simulated by the model.The values mentioned are at a particular depth 0.2m above ground.

Regards,
Rakesh

[vinerm]

By measurement I did not mean experiment rather the averaging procedure used. CFD does not give single values. User needs to average over boundary or cell zones. Since you mentioned integral values, those might have been averaged over some zone. And averaging requires care.

[rakadit]

Thanks,

I have not used any averaging function. These are instantaneous values.

Regards,
Rakesh

[vinerm]

Velocity is a field, so are density and dynamic pressure. You cannot represent those using single values.

[rakadit]

You are right. But here it is velocity magnitude only. Question remains when VOF of one phase is very high ,0.8 to 1.0 ,it's dynamic pressure values are matching the theoretical relation but if reverse is there, VOF is low in the range of 0.2 or less, simulated values don't follow theoretical relation.
Regards,

Rakesh

[vinerm]

Whether it is low volume fraction or high, the relation is always maintained because this is the equation used to calculate dynamic pressure. Fluent does not solve any conservation or other equation for dynamic pressure that is not linked with velocity. The solution is for velocity components only and then those are used to derive magnitude of velocity or dynamic pressure.

However, you have mentioned only single values. I don't think you have single cell or single face in your simulation. So, if these values are taken at a boundary or at a point in the domain, you have to be careful about how you fetched those values. If you created a point and use vertex average or facet average for velocity and dynamic pressure, do not these are not calculated in a straightforward manner. That's why it is very important to know how and at what location did you fetch these values from Fluent?

[rakadit]

Thanks for providing a very nice insight into the problem solution.

Yes, I created some points in the CAD(Gambit) and usng probe tool in the CFD post, I am entering coordinates of those points. This is done to have comparison with some experimental values. So, it means Fluent is picking values from the adjoining points/cells.That is why matching issues. Is there any other better way to do this comparison?

regards,

Rakesh

[vinerm]

Better is to use cell centered value and fetch only the primitive variables, i.e., velocity and density instead of fetching derived variables, such as, dynamic pressure. Calculate dynamic pressure yourself.

[rakadit]

Thanks for the reply and useful suggestions.

Regards,

Rakesh

[pachputesharad]

Follow the blog for" CFD Flow Engineering" for Multiphase flow Modeling in FLUENT, Star CCM and COMSOL

https://cfdflowengineering.com/turbu...se-combustion/