[yogeshghadge314@gmail.com]

hi!
i was doing a simulation of convergent divergent nozzle , fluid taken as air , pressure at inlet and pressure at outlet is known. I want an efficient combination of convergent and divergent angle to have min drag on the incoming fluid. taken viscous fluid, energy equation is ON.

OK, now coming to problem.
first I did the steady state analysis and I found that the solution didn't converge due formation of eddies in the divergent section. So I went with a transient simulation and monitored Cd plot. It was seen that series shocks were produced in the divergent section. As Cd plot converged I tried to converge the solution at a particular time step, as I thought that the oscillation of residual between 1e-04 and 1e-05 is due the eddies in the flow.

so I used time step size = 0.1s
time steps = 1
and increased the no. of iteration/time step in order to converge the solution below 1e-06.
but I found that the residual fall a little but didn't converged below 1e-06, residual started oscillating around 1e-05.

but when I reduced the time step to 1e-05 the solution converged below residuals 1e-06.
I don't understand why the model is showing such a behaviour. is it due to shocks or the eddies?

Any help is appreciated

[FMDenaro]

You wrote a lot of things that, however, are of no help.
What about:
1) 2d/3d geometry
2) Formulation of the governing equations
3) Numerical discretization/software
4) BCs. setting


and, would be of some help if you post some result.

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

You wrote a lot of things that, however, are of no help.
What about:
1) 2d/3d geometry
2) Formulation of the governing equations
3) Numerical discretization/software
4) BCs. setting


and, would be of some help if you post some result.

1. 2D geometry with axisymmetric assumption
2. Navier stokes eqs with transition SST model, density based solver.
3. Ansys fluent
4. Bcs. pressure inlet = 101325 pa , T = 298 K
pressure outlet = 33800 pa
wall :- no slip, heat flux = 0
axis

[FMDenaro]

Well, due to the axisymmetric assumption and the RANS modelling, the existence of a time-dependent fluctuation in the eddies has no physical meaning.
What I see is that you have a subsonic inflow (one condition must be set free to adapt from the interior) but the outflow is a mix of supersonic/subsonic flow regions. That should be one of the reasons of the convergence problem.
As you did not write nothing about the numerical integration in time and space, I can suppose also problems in the numerical stability constraints.
Furthermore, the turbulence model could add problems.
However, to check the viscous drag you should have a wall-resolved grid.



I strongly suggest to run first a standard test-case and check if you are able to produce a good solution.

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

Well, due to the axisymmetric assumption and the RANS modelling, the existence of a time-dependent fluctuation in the eddies has no physical meaning.
What I see is that you have a subsonic inflow (one condition must be set free to adapt from the interior) but the outflow is a mix of supersonic/subsonic flow regions. That should be one of the reasons of the convergence problem.
As you did not write nothing about the numerical integration in time and space, I can suppose also problems in the numerical stability constraints.
Furthermore, the turbulence model could add problems.
However, to check the viscous drag you should have a wall-resolved grid.



I strongly suggest to run first a standard test-case and check if you are able to produce a good solution.

Thank you for your reply.
I am not able to follow your second point can you please elaborate.

[FMDenaro]

Originally Posted by yogeshghadge314@gmail.com

Thank you for your reply.
I am not able to follow your second point can you please elaborate.

What exactly?

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

What exactly?

Having a subsonic flow at inlet and mixed subsonic/supersonic flow at outlet, how does it leads to convergence problem?

[FMDenaro]

Originally Posted by yogeshghadge314@gmail.com

Having a subsonic flow at inlet and mixed subsonic/supersonic flow at outlet, how does it leads to convergence problem?

According to the characteristic directions, supersonic outflow has different BC setting from a subsonic outflow. If the eddies at the outflow cause the fluctuation of the Mach number at the outlet, the solver can have problem in convergence.
On the other hand you are integrating in time and further problems can be in the numerical stability, check the correct CFL.
However, without details about the numerical integration is difficult to see your problem.
Again, solve first a well assessed test-case from the literature.

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

According to the characteristic directions, supersonic outflow has different BC setting from a subsonic outflow. If the eddies at the outflow cause the fluctuation of the Mach number at the outlet, the solver can have problem in convergence.
On the other hand you are integrating in time and further problems can be in the numerical stability, check the correct CFL.
However, without details about the numerical integration is difficult to see your problem.
Again, solve first a well assessed test-case from the literature.

I read about this problem a bit. It was said that the time dependent oscillations are due to the shock-boundary layer interaction which is an unsteady phenomenon. The position of the shocks tends to move to and fro by a slight amount which brings an unsteady behaviour in the model.

[JBeilke]

A time step size of 0.1s is simply too big. Adjust this value the get a courant number somwhere between 0.5 and 5 (depends on the solver).



@FMD
He is using the normal Fluent settings and this is a well defined testcase. No need to be overacademic.

[FMDenaro]

Originally Posted by JBeilke

A time step size of 0.1s is simply too big. Adjust this value the get a courant number somwhere between 0.5 and 5 (depends on the solver).



@FMD
He is using the normal Fluent settings and this is a well defined testcase. No need to be overacademic.

Using a viscous and turbulent model in this test case is quite redundant to be really a test-case. First of all he should be able to get a steady solution in standard conditions for checking the BC.s setting.

Then, using the axisymmetric condition is valid for a statistically steady flow. In case of a physical description of the oscillations, the gemoetry must be 3D.
Thus, I see too many mixed issues in this problem.

[yogeshghadge314@gmail.com]

@Jbeilke @FMD
Thank you both for your reply. I will consider your suggestions and perform the simulation again.
@FMD
Can you please explain why the flow should be statically steady for axisymmetric assumption.

[FMDenaro]

Originally Posted by yogeshghadge314@gmail.com

@Jbeilke @FMD
Thank you both for your reply. I will consider your suggestions and perform the simulation again.
@FMD
Can you please explain why the flow should be statically steady for axisymmetric assumption.

Fluctuations in a real turbulent field are not axisymmetric even if the geometry is axisymmetric. For this reason what you see is numerical, not a real physical aspect of the flow.

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

Fluctuations in a real turbulent field are not axisymmetric even if the geometry is axisymmetric. For this reason what you see is numerical, not a real physical aspect of the flow.

Thanks. Got it

[FMDenaro]

You can find in literature papers about the turbulent flow structures in a converging-diverging nozzle, using DNS/LES/URANS.
But I suggest to check if you are able to replicate this test case
https://www.researchgate.net/publica...d_Dynamics_CFD

[Howwikis]

United States Banking

[yogeshghadge314@gmail.com]

Originally Posted by FMDenaro

You can find in literature papers about the turbulent flow structures in a converging-diverging nozzle, using DNS/LES/URANS.
But I suggest to check if you are able to replicate this test case
https://www.researchgate.net/publica...d_Dynamics_CFD

Thanks, I will take a look.

[yogeshghadge314@gmail.com]

@FMD
I tried to set the time step by CFL based time setting. It is showing that the time step required for courant no. to be 1 is 6e-10 s. which is too small and taking a very large computational time for the solution to converge. But on the positive side, the solution is showing sign of convergence.

[FMDenaro]

Originally Posted by yogeshghadge314@gmail.com

@FMD
I tried to set the time step by CFL based time setting. It is showing that the time step required for courant no. to be 1 is 6e-10 s. which is too small and taking a very large computational time for the solution to converge. But on the positive side, the solution is showing sign of convergence.

Not strange at all, the CFL take into account acustic waves for the stability of explicit method.

Generally, an implicit method is used in order to adopt a greater time-step. However, try to reach a convergent solution with this small time-step before to proceed further with change in the setting.

[JBeilke]

The time step size for Co=1 should not be so small. There are some error messages on the mesh picture. Please check the mesh quality at first.