[clecle69]

Hi everyone,

I am posting this new thread because I am quite new at StarCCM+ and cannot solve the following problem.

I want to simulate a flow in the geometry shown in the attached image. It has one inlet and one outlet and some holes in the fluid domain.

The flowrate is 2 m/s so I believe, considering the size (inlet and outlet diameters of 0.04m) and the fact that the fluid is water, that a laminar flow is sufficient, even though the fluid domain is a bit complicated.

I tried different meshes : polyhedral with prism layers mainly (up to 80 millions of cells) and the computation cannot converge.

I tried as BCs different configurations :
- Massflow rate or velocity at inlet
- Pressure outlet (w/ and w/o target mass flow rate)

The problem is that the mass flow rate at the outlet is very different from the one I impose at the inlet, although it should be almost exactly the same.

I am open to any help and can give you some more information if necessary.

Thanks to all

Clément

[kguntur]

Hi,

Referring to "some holes in the fluid domain", is any flow going out through the holes? How did you model them?
Is your outlet flow less than or greater than the inlet flow?

[clecle69]

First of all, thank you for your answer and trying to help me.

When I said "holes" I meant that the fluid domain is such that flow separation must occur. They are not actual holes.

When I check the mass flow rate on the different boundaries, the one referring to the wall is exactly 0 so there is no numerical leak.

The outlet flow rate is lower (25%) but it is due to the fact that this is not a converged solution. In fact, this is the problem : I am not able to reach convergence despite a large numer of cells.

Thank you for your help.

Cheers,

Clément

[kguntur]

if there is flow separation, I think that you should be using turbulent models. From the velocities and dimensions the flow seems to be laminar. But it could be locally turbulent.
Did you try with turbulent models?
Just out of curiosity, how many iterations did you rune the model for?

[clecle69]

I tried turbulent models at first but it does not help!

About ten thousands iterations were performed for my tests!

Thank you for your concern and help!

Clément

[azt]

Hi

Try changing to a velocity inlet and a pressure outlet. Monitor the mass flow on the outlet check the flow rate. If it's not correct change the velocity accordingly.

I don't think an incompressible flow with mass flow inlet is a very good idea.

If you must use a mass flow inlet then change the flow to compressible water. If you do this you probably need to run in double precision.

Use a turbulence model as well.

azt

[cwl]

For incompressible flow - Flow-Split Outlet will guarantee the mass ballance.

UserGuide says:

Mass Flow Inlet
A mass flow inlet boundary represents an inlet for which the mass flow rate
is known.
Application
The inlet to a simulation of compressible internal flows for which the mass
flow rate is known
Compatibility
• Should be used in combination with pressure outlet boundaries


Velocity Inlet
A velocity inlet boundary represents the inlet of a duct at which the flow
velocity is known.
Application
The inlet to a simulation of incompressible internal flows.
Compatibility
• Can be used in combination with pressure outlet and flow split outlet
boundaries


Flow Split Outlet
Application
Incompressible internal flows, with multiple outlets, for which the flow
split between the outlets is specified.
Compatibility
• Should not be used with compressible flows
• Cannot exist in the same continuum as pressure, stagnation and mass
flow boundaries, or mixing-plane interfaces
• Not suitable for outflow boundariesat which recirculation (inflow)
occurs


Pressure Outlet
A pressure outlet boundary is a flow outlet boundary at which the pressure
is specified.
Applications
• Outflow of compressible and internal flows
• A plenum, for example, the boundary surrounding a jet emanating into
a large chamber
Compatibility
• A pressure outlet boundary cannotexist in the same continuum as a
flow split outlet.
• Although STAR-CCM+ does not prevent a pressure outlet boundary
from being used as an inlet, a stagnation boundary is a better choice.

BUT: in Star-CCM+ samples combination of Mass Flow Inlet and Pressure Outlet for incompressible flow is freely used. Also - while using Pressure Outlet pay attention to backflow, this can be a reason for imballance.

[clecle69]

Hello,

First of all, thank you for trying to help me!

Actually, my model (picture contained in my first message) contains only one outlet but there are cavities where the fluid can not go in the middle of the domain which separate the flow.

Can I therefore use the flow split outlet BC? I thought it works only for multiple outlets flow.

Anyway, I'll try that and keep you informed.

Last question : what turbulence model would you use as the sections where the fluid evolve are very thin?

Thanks again.

[azt]

Hi

you can use a flow split outlet, set the split on your boundary to 1.0.

Try the k-w or k-e turbulence models.

azt

[cwl]

azt is right - Flow-Split Outlet with ratio set to 1.0 is correct.

Considering turbulence model - you should estimate your Reynolds number that describes flow in thin channels, the flow might be laminar as well.

[lcarasik]

Using, your velocity of 2 m/s and a diameter of 0.04 m and a kinematic viscosity of 1.004^10^-6 m^2/s, I get a Reynolds number of 79681, which is highly turbulent. You have to use a turbulence model.

Also, you are not suppose to use boundary conditions combinations such as a velocity/mass flow inlet with a mass flow or velocity defined outlet. It is over defining your boundary conditions and doesn't work with the solvers. That is partly why you were not converging properly.

(http://www.engineeringtoolbox.com/wa...ity-d_596.html)

[techtradezone]

hi guys i really love this subject of discuss,i am solving an analyzis on inpipe turbine, inlet velocity is 1.4m/s, outlet gauge pressure of 0 for scenario 1, and outlet unknown for scenario 2 using autodesk cfd, first ramp the turbine velocity to 2400, then change the rotatin region to free spinning. but my outlet flow rate was abit higher than inlet and the inlet velocity later her than specify one from the set up. changes to 1.6... m/s while plot the xy plot of a point at inlet and at outlet and the outlet velocity get to 1.5.. so please why is it like that?

[ftab]

Originally Posted by lcarasik

Also, you are not suppose to use boundary conditions combinations such as a velocity/mass flow inlet with a mass flow or velocity defined outlet. It is over defining your boundary conditions and doesn't work with the solvers. That is partly why you were not converging properly.

HiMr. Carasik,
Could you explain why for incompressible flow the combination of massflow inlet and mass flow outlet in steady simulation is wrong?