Multiphase flow modelling
 

Hi.

I have a problem with my set up. I want to simulate a flow with solid particles dispersed in the continous phase. I have created the solid particles myself. After setting up the default domain and the boundary conditions I am left with one error message: "
In Analysis 'Flow Analysis 1' - Domain 'Default Domain': The following materials require Viscosity to be defined: 'Particle hydrates'".

I have read under in CFX Pre Help under " Gas-Solid and Liquid-Solid Flow" that one should assign the solid phase a small insignificant molecular viscosity. My problem is that I cannot find any place to even insert any viscosity. Under "Material" and "Material Properties" there are no place to insert any viscosity (most likly becasue I have set the thermodynamic state as "solid").

Can anyone help me out?

click and edit the ccl in your dispersed solid material definition and add the following line under properties (or mixture properties if its a mixture)

DYNAMIC VISCOSITY:
Dynamic Viscosity = 0.1 [kg m^-1 s^-1]
Option = Value
END

Thank you ckleanth for your reply.

I tried to do it, but I got another error message saying "The object "DYNAMIC VISCOSITY" is present in the object "/LIBRARY/MATERIAL:Particle hydrates/PROPERTIES" but it is not physically valid."

My command editor looks like this now (I removed the thermal conductivity):

LIBRARY:
&replace MATERIAL: Particle hydrates
Material Description = Particle hydrates
Material Group = Particle Solids
Object Origin = User
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
DYNAMIC VISCOSITY:
Dynamic Viscosity = 0.1 [kg m^-1 s^-1]
Option = Value
END
EQUATION OF STATE:
Density = 1140 [kg m^-3]
Molar Mass = 0.1377 [kg mol^-1]
Option = Value
END
END
END
END

How can I get this right?

just ignore the message

Hi.

I tried to do that last night, and the solver runs successfully. But in Post i get several error messages of the type;
WARNING, Object(s) ”Hydrates Volume Fraction” referenced in object ”Inlet/Colour Variable” either do not exist or have a scheduler type.

I get the same message for “outlet” and “wall” and all other planes and contours I've previously made in Post.

What can I do?

Hi,

It seems you are simulationg the solid particles using eulerian approach. In that case you have to define your particles as fluid & define some viscosity too. In domain tab you will get an option for fluid details where you can define them as solid particles.

If not, then use lagrangian approach. define solid as solid in material tab & in domain tab activate particle tracking.

Regards,

--Sanyo

redo the planes contours etc on a fresh state file from your newly created results file.

try changing material group to user. than u can define viscosity for solids too.