[Luttappy]

Dear Friends,
I was trying to simulate unsteady flow in corrugated channel.
When i considered full domain (domain with 15 repeated wavy modules) i was not able to capture unsteady flow. (BCs:- Inlet-uniform flow, outlet- pressure outlet/outflow)
But when i considered single module with periodic boundary conditions i was able get unsteady flow.
In experiment, they reported unsteady flow in the considered Re (Re = 600).
Interestingly, time-averaged velocity contour/streamlines are same in both cases.
Anyone know the reason for not able to capture unsteady flow when i consider full domain?
NOTE: I used ANSYS Fluent CFD package

Please help
Thanks alot

[FMDenaro]

Originally Posted by Luttappy

Dear Friends,
I was trying to simulate unsteady flow in corrugated channel.
When i considered full domain (domain with 15 repeated wavy modules) i was not able to capture unsteady flow. (BCs:- Inlet-uniform flow, outlet- pressure outlet/outflow)
But when i considered single module with periodic boundary conditions i was able get unsteady flow.
In experiment, they reported unsteady flow in the considered Re (Re = 600).
Interestingly, time-averaged velocity contour/streamlines are same in both cases.
Anyone know the reason for not able to capture unsteady flow when i consider full domain?
NOTE: I used ANSYS Fluent CFD package

Please help
Thanks alot

How do you judge that the solution is steady in the full geometry case? The physics of the whole geometry and that one of the single and periodic geometry implies different meaning in the solution. The former is a space evolving flow, the latter is a time evolving flow.

[Luttappy]

Originally Posted by FMDenaro

How do you judge that the solution is steady in the full geometry case? The physics of the whole geometry and that one of the single and periodic geometry implies different meaning in the solution. The former is a space evolving flow, the latter is a time evolving flow.

Thank you for your reply.
I think considering single module with periodic boundary condition represent periodically fully developed flow in the wavy channel.
In other words, it should represent the flow in the wavy modules in the center portion of the channel (like 5th, 6th, 7th, 8th. module for 15 wavy module case, such that flow is periodically fully developed in these modules).

I was monitoring the velocity signals at different points in both periodic as well as full domain case. In full domain i was not getting any oscillations, while for periodic BC case i was getting oscillations for the same Re considered. Experiments from literature also confirms that the flow is unsteady at that Re.

[FMDenaro]

Originally Posted by Luttappy

Thank you for your reply.
I think considering single module with periodic boundary condition represent periodically fully developed flow in the wavy channel.
In other words, it should represent the flow in the wavy modules in the center portion of the channel (like 5th, 6th, 7th, 8th. module for 15 wavy module case, such that flow is periodically fully developed in these modules).

I was monitoring the velocity signals at different points in both periodic as well as full domain case. In full domain i was not getting any oscillations, while for periodic BC case i was getting oscillations for the same Re considered. Experiments from literature also confirms that the flow is unsteady at that Re.

Well, you cannot say that is for sure, it depends also on the Re number and the type of inflow. To correlate physically the flow as same as in the fully periodic case you could need of a larger length.
However, what about the inflow condition?
Post the fields

[LuckyTran]

Re=600 is laminar? Is it realistic to expect fully developed flow after 5 modules?

Inflow conditions are obviously different.


What about running your 16 module case with periodic BC's as a sanity check? To make sure nothing else changed....

Originally Posted by Luttappy

Interestingly, time-averaged velocity contour/streamlines are same in both cases.

That's arithmetically not possible because any additional unsteadiness/moments imparts a bias onto the mean flow.

[Luttappy]

Originally Posted by FMDenaro

Well, you cannot say that is for sure, it depends also on the Re number and the type of inflow. To correlate physically the flow as same as in the fully periodic case you could need of a larger length.
However, what about the inflow condition?
Post the fields

Thank you sir for the reply.
I will try simulating a case with more number of wavy modules like 30 modules, and i will let you know the outcome.

Regarding BC's i used,
Full domain
Inlet-uniform flow; outlet- pressure outlet

Periodic domain
Inlet and Outlet- periodic BC

[Luttappy]

Originally Posted by LuckyTran

Re=600 is laminar? Is it realistic to expect fully developed flow after 5 modules?
Inflow conditions are obviously different.
What about running your 16 module case with periodic BC's as a sanity check? To make sure nothing else changed....
That's arithmetically not possible because any additional unsteadiness/moments imparts a bias onto the mean flow.

Thank you sir for the reply.
At Re = 600, flow is still in laminar but in quasi-periodic regime.
I will simulate the case with 16 module case with periodic BC and i will let you know the outcome.

[FMDenaro]

Originally Posted by Luttappy

Thank you sir for the reply.
I will try simulating a case with more number of wavy modules like 30 modules, and i will let you know the outcome.

Regarding BC's i used,
Full domain
Inlet-uniform flow; outlet- pressure outlet

Periodic domain
Inlet and Outlet- periodic BC

The uniform inlet velocity is clearly a problem, you need some lenght to let the flow developing and forget the inviscid inlet condition. Why don't you try to set as inlet a laminar velocity profile?

I think you could start using 20 modules but analyse the velocity in time only for the last 2-3 modules to see if the onset of unsteady character appears

[Luttappy]

Originally Posted by FMDenaro

The uniform inlet velocity is clearly a problem, you need some lenght to let the flow developing and forget the inviscid inlet condition. Why don't you try to set as inlet a laminar velocity profile?

I think you could start using 20 modules but analyse the velocity in time only for the last 2-3 modules to see if the onset of unsteady character appears

Thank you sir, i will try this.

[Luttappy]

Originally Posted by FMDenaro

The uniform inlet velocity is clearly a problem, you need some lenght to let the flow developing and forget the inviscid inlet condition. Why don't you try to set as inlet a laminar velocity profile?
I think you could start using 20 modules but analyse the velocity in time only for the last 2-3 modules to see if the onset of unsteady character appears

I considered 30 module case with uniform inlet and fully developed velocity inlet boundary condition.
In both cases, i was not getting any unsteady flow in the channel (Nowhere in the channel).

Originally Posted by LuckyTran

Re=600 is laminar? Is it realistic to expect fully developed flow after 5 modules?
Inflow conditions are obviously different.
What about running your 16 module case with periodic BC's as a sanity check? To make sure nothing else changed....
That's arithmetically not possible because any additional unsteadiness/moments imparts a bias onto the mean flow.

I also tried 30 module case with periodic boundary conditions at inlet and outlet. Here also, i was not getting any unsteady flow in the domain.

[FMDenaro]

Originally Posted by Luttappy

I considered 30 module case with uniform inlet and fully developed velocity inlet boundary condition.
In both cases, i was not getting any unsteady flow in the channel (Nowhere in the channel).



I also tried 30 module case with periodic boundary conditions at inlet and outlet. Here also, i was not getting any unsteady flow in the domain.

Well, first of all let us considering some numerical issues:
1) what about the cell Reynolds distribution of your grid? Were you able to get O(1) everywhere?
2) what about the setting of the scheme in Fluent? You should set a second order discretization in time and space for the laminar flow, do not use any upwinding.


Then, are you sure that the experiment has no relevant 3D effects you are not considering? Have you a sketch of the experimental configuration?
Could you show how the unsteady measurments are obtained?

[Luttappy]

Originally Posted by FMDenaro

Well, first of all let us considering some numerical issues:
1) what about the cell Reynolds distribution of your grid? Were you able to get O(1) everywhere?
2) what about the setting of the scheme in Fluent? You should set a second order discretization in time and space for the laminar flow, do not use any upwinding.
Then, are you sure that the experiment has no relevant 3D effects you are not considering? Have you a sketch of the experimental configuration?
Could you show how the unsteady measurments are obtained?

Thank you sir for the reply.

1. I calculated cell Re (Ulocal*Characteristic Length/mu) based on the equation. Ratio of cellRe with Re is in the order of 1 in the grid.
2. I considered second order discretization in time and space in my computations.

Regarding experiments: I referred literature. Mostly in literature they did flow visualization experiments to see the unsteady flow characteristics. Flow will become unsteady in the Re range of 350-450 and becomes three-dimensional in the Re range of 550-700 depends upon the geometric configurations.

[FMDenaro]

Originally Posted by Luttappy

Thank you sir for the reply.

1. I calculated cell Re (Ulocal*Characteristic Length/mu) based on the equation. Ratio of cellRe with Re is in the order of 1 in the grid.
2. I considered second order discretization in time and space in my computations.

Regarding experiments: I referred literature. Mostly in literature they did flow visualization experiments to see the unsteady flow characteristics. Flow will become unsteady in the Re range of 350-450 and becomes three-dimensional in the Re range of 550-700 depends upon the geometric configurations.

Is it possibile that your bcs do not fully match the experimental setting?
Could you post such literature? Are you using unbounded second order central discretization?
What about the norm of the time derivatives you are fixing to assess that the solution is steady? Then, please post the time evolution of the velocity components in the station you are checking

[Luttappy]

Originally Posted by FMDenaro

Is it possibile that your bcs do not fully match the experimental setting?
Could you post such literature? Are you using unbounded second order central discretization?
What about the norm of the time derivatives you are fixing to assess that the solution is steady? Then, please post the time evolution of the velocity components in the station you are checking

Thank you sir for the reply.
I was referring the papers by Nishimura et al. and Rush et al.
I am monitoring x and y velocity component of different points in the domain. Variation of x and y velocity components are straight line with respect to time when i consider full domain (30 Modules). It is oscillatory when i consider periodic domain. Even though velocity signals are not given in experiments, flow visualization study indicates that the flow is unsteady at the Reynolds number 600.

[FMDenaro]

Originally Posted by Luttappy

Thank you sir for the reply.
I was referring the papers by Nishimura et al. and Rush et al.
I am monitoring x and y velocity component of different points in the domain. Variation of x and y velocity components are straight line with respect to time when i consider full domain (30 Modules). It is oscillatory when i consider periodic domain. Even though velocity signals are not given in experiments, flow visualization study indicates that the flow is unsteady at the Reynolds number 600.

Yes, an unsteady pattern clearly appears in the experiment at Re=650 but they do not report any numerical simulation at that Re number.
Again you did not answer providing the details of your setting.

Could you post your geometry and the grid used around a single module?

[Luttappy]

Originally Posted by FMDenaro

Yes, an unsteady pattern clearly appears in the experiment at Re=650 but they do not report any numerical simulation at that Re number.
Again you did not answer providing the details of your setting.
Could you post your geometry and the grid used around a single module?

Sorry I missed to post details regarding solver I used.
Package: ANSYS Fluent
Scheme: SIMPLE
Spatial Discretization:
o Gradient- Least Square Cell Method
o Pressure:- Standard
o Momentum:- QUICK
Transient Formulation:- Second order implicit
Under Relaxation Factors
o Pressure: 0.3
o Momentum: 0.7
I used same schemes for full domain case and periodic domain case.
Structured mesh has been used for computations.

[LuckyTran]

30 modules with periodic BC's does not produce unsteady flow but 1 module does.....

We have to consider now user error in the setup. This is no longer a question of periodic BC's vs uniform inlet.

Btw, if you run your 1 module case on a Sunday, does it also not produce unsteady result? Sunday is a joke, but there's clearly a problem with reproducibility here.

On a serious note, just dump all your settings. Viscous model = ? time-step size? number of iterations per time-step. Results?

[FMDenaro]

Originally Posted by Luttappy

Sorry I missed to post details regarding solver I used.
Package: ANSYS Fluent
Scheme: SIMPLE
Spatial Discretization:
o Gradient- Least Square Cell Method
o Pressure:- Standard
o Momentum:- QUICK
Transient Formulation:- Second order implicit
Under Relaxation Factors
o Pressure: 0.3
o Momentum: 0.7
I used same schemes for full domain case and periodic domain case.
Structured mesh has been used for computations.

First of all, set second order time integration and second order unbounded central scheme in space. QUICK scheme is definitely to not be used here.
You can also use NITA scheme.
Have you tried to run exactly the same experimental gemoetry with the inlet section, ten modules and the outlet section?