[mmengineer]

Hello everyone,

i´m simulating an Open-Channel problem and i´m trying to get Drag values of bridge inside that open channel. The simulations works and i´m getting results for the Drag coefficient. The global courant number of the problem is under 1 with a time step size of 0.005 s and the calculated drag-coefficient is about 0.9.

But when I change the time-step-size to 0.0025 s the drag-coefficient jumps up to about 1.1 and will stay there.

When i change the time-step-size to 0.00005 s the drag-coefficient jumps up to about 30.

When i look at the calculated drag forces the same thing will happen, so i guess it´s not a problem of reference values or something, but a problem inside the simulation. But i can´t figure out what causes the problem, since the courant number is below 1 in every of the simulations.

Shouldn´t the result be unaffected of changes in time step size as long as the time step are not too big or way too small?

Can anyone help me with this problem or does anyone at least have an idea what causes this behaviour of the simulation.

Thank you very much

[lalupp]

I also getting the same issue
But in my case the time advancement is 1st Order backward Euler
I dont know this pattern prevails in higher order time advancement schemes
Anyway I am also curious

[FMDenaro]

Originally Posted by mmengineer

Hello everyone,

i´m simulating an Open-Channel problem and i´m trying to get Drag values of bridge inside that open channel. The simulations works and i´m getting results for the Drag coefficient. The global courant number of the problem is under 1 with a time step size of 0.005 s and the calculated drag-coefficient is about 0.9.

But when I change the time-step-size to 0.0025 s the drag-coefficient jumps up to about 1.1 and will stay there.

When i change the time-step-size to 0.00005 s the drag-coefficient jumps up to about 30.

When i look at the calculated drag forces the same thing will happen, so i guess it´s not a problem of reference values or something, but a problem inside the simulation. But i can´t figure out what causes the problem, since the courant number is below 1 in every of the simulations.

Shouldn´t the result be unaffected of changes in time step size as long as the time step are not too big or way too small?

Can anyone help me with this problem or does anyone at least have an idea what causes this behaviour of the simulation.

Thank you very much

Without the details of your setup no one can address an opinion...

[mmengineer]

Thanks for your reply, here are same details of my setup:
It´s a 3D VOF Multiphase Simulation with water and air as fluids.
Open Channel Wave BC with free surface option and k-omega SST Turbulence Model.
I already tried different solver methods and i also tried it with a 2D open channel simulation with a simple square as object of which i´m calculationg the drag and the same issue occured.

[arjun]

Originally Posted by mmengineer

Thanks for your reply, here are same details of my setup:
It´s a 3D VOF Multiphase Simulation with water and air as fluids.
Open Channel Wave BC with free surface option and k-omega SST Turbulence Model.
I already tried different solver methods and i also tried it with a 2D open channel simulation with a simple square as object of which i´m calculationg the drag and the same issue occured.

It is a known problem and it occurs from two things:

1. The flux dissipation (Rhie Chow term mainly) depends on time stepsize.
2. Flux dissipation does not go to zero as it shall go in theory upon convergence.





If this aspect is critical to you then using cartesian type cells would help since there you have change to achieve (2)

[FMDenaro]

What is not clear to me is if your case is statistically time-dependent or not. In the latter case, you are using a pseudo-transient to get a convergent steady state? Do you get the same convergence with different time-steps or not?
Some numerical stabilization can alter the final solution when the time step is reduced because they retain a contribute that does not vanish.

[mmengineer]

I´m doing transient simulation. My case is an open channel with a bridge inside of which I want to get the drag force.
The water is flowing at the bridge with 5 m/s. Since the flow regions around the bridge are surely turbulent I thought I have to use the transient solver to get accurate results.

[arjun]

Originally Posted by mmengineer

I´m doing transient simulation. My case is an open channel with a bridge inside of which I want to get the drag force.
The water is flowing at the bridge with 5 m/s. Since the flow regions around the bridge are surely turbulent I thought I have to use the transient solver to get accurate results.

what software are you using???

[mmengineer]

i´m using ansys fluent 2020

[arjun]

Originally Posted by mmengineer

i´m using ansys fluent 2020

If it makes you feel any better the problem exists in starccm too. :-D

PS: My solver one can switch off the Rhie chow dissipation but your problem is something i am supposed to study when i am free next because we have known of it for long time (more than 8 years at least).

[FMDenaro]

Originally Posted by mmengineer

I´m doing transient simulation. My case is an open channel with a bridge inside of which I want to get the drag force.
The water is flowing at the bridge with 5 m/s. Since the flow regions around the bridge are surely turbulent I thought I have to use the transient solver to get accurate results.

It is not a deterministic transient but a statistical transient and if you don't have any time-dependent external forcing you should first check for the statistically steady solution (RANS). What seems you are trying to do is the Unsteady RANS formulation. That has nothing to do with the accuracy in the results is just a formulation where the turbulence appears unsteady only in the statistical variable. Furthermore, computing the drag force means you have to resolve the boundary layer with a very fine grid and no wall models must be prescribed.
If you are not expert in these issues you need to read some fundamental parts about turbulence over bluff bodies.

[mmengineer]

I´m not sure if it makes me feel better

Okay, but how did you handle that problem ?
Because now I can´t be sure with which time step size my results a right

[arjun]

Originally Posted by mmengineer

I´m not sure if it makes me feel better

Okay, but how did you handle that problem ?
Because now I can´t be sure with which time step size my results a right

If i understand things correctly then using body force weighted, second order or presto scheme should reduce the issue for you. Fluent provides them.



For VOF fluent already suggests body force weighted scheme so now i am not sure. If you are not using it then try it out.



(it basically tries to match pressure better at control volume faces thus shall reduce dissipation flux).

[mmengineer]

Hi Arjun,
thanks for your suggestions.
I did a little study with a simple geometry in 2D, using implicit and explicit vof scheme with varying time step sizes and the body weighted force option.
It looks like the problem is gone with the body weighted force option, I tried it with courant numbers of around 0.03, 0.30 and 3.00 and I received almost exactly the same results in every case.
I´m gonna try the same in 3D now.

Regards, Moritz

[arjun]

Please share the outcome of 3D cases too.


In August met prof. Peric and he mentioned a similar issue in starccm+ too. That time I mentioned to him that this in my opinion is the cause of the problem. Since my solver has body force weighted scheme he suggested me to test.
But I have been busy so had no time for it. This is why your findings could be very useful for us too.


Thank you


Arjun

[nashreonline]

What is not clear to me is if your case is statistically time-dependent or not. In the latter case, you are using a pseudo-transient to get a convergent steady state? Do you get the same convergence with different time-steps or not?
.

Book Template Indesign

[mmengineer]

Originally Posted by FMDenaro

It is not a deterministic transient but a statistical transient and if you don't have any time-dependent external forcing you should first check for the statistically steady solution (RANS). What seems you are trying to do is the Unsteady RANS formulation. That has nothing to do with the accuracy in the results is just a formulation where the turbulence appears unsteady only in the statistical variable. Furthermore, computing the drag force means you have to resolve the boundary layer with a very fine grid and no wall models must be prescribed.
If you are not expert in these issues you need to read some fundamental parts about turbulence over bluff bodies.

Hello Filippo, why do you think i have to resolve the boundary layers very fine to compute the drag coefficient? I guess you mean i have to reach a y+ value between 5 and 30 or at the best around 1.
I heard this very often when i was researching, but i could not really discover big differences in the computed drag coefficient with or without inflation layers. My model is by the way way too big to reach a y+ value of 1, it would end in too much computational time, because i have to simulate the problem quite often with varying Parameters.
I did some studies with smaller geometrys in 2D and 3D about the correlation of the y+ and the computed drag force, but I couldnt find any big differences between the models with and without inflation layers.
The y+ values varyied between 10 at the finest resolved model and 100 at the model without any inflation layers.
The only thing i found out is that the finer resolved models picture the "small" variations of the drag coefficient, due to waves and vortex better. But the time averaged drag force is almost exactly the same.
Does this make any sense in your opinion, or is there maybe something fundamentally wrong?
Regards, Moritz

[FMDenaro]

Originally Posted by mmengineer

Hello Filippo, why do you think i have to resolve the boundary layers very fine to compute the drag coefficient? I guess you mean i have to reach a y+ value between 5 and 30 or at the best around 1.
I heard this very often when i was researching, but i could not really discover big differences in the computed drag coefficient with or without inflation layers. My model is by the way way too big to reach a y+ value of 1, it would end in too much computational time, because i have to simulate the problem quite often with varying Parameters.
I did some studies with smaller geometrys in 2D and 3D about the correlation of the y+ and the computed drag force, but I couldnt find any big differences between the models with and without inflation layers.
The y+ values varyied between 10 at the finest resolved model and 100 at the model without any inflation layers.
The only thing i found out is that the finer resolved models picture the "small" variations of the drag coefficient, due to waves and vortex better. But the time averaged drag force is almost exactly the same.
Does this make any sense in your opinion, or is there maybe something fundamentally wrong?
Regards, Moritz

When talking about the viscous drag, you have to think that it depends on the product between the viscosity and the derivative of the streamwise velocity along the normal-to-wall direction. If you do not use a grid having at least 3-4 nodes in the viscous sublayer (y+<1) the numerical derivative will result in a wrong value.
To understand better, consider the wall law u+=y+ so that you have the exact derivative at the wall =1. Try to solve numerically a simple case with the first grid node at y+=10.

[FMDenaro]

Of course, I am talking of the case where you prescribe natural boundary condition, you cannot use the wall-modelled BC for computing the viscous drag.