Learning Forum

[Mehmet D.]

My aim is to accurately determine the free surface elevation when a wing moves over the free surface. I am trying to do (2D NACA0012 AoA 5, h/c =1, Fnc = 1) but the free water surface does not deform (even when I make h/c = 0.2). I am using  2D mesh as below using the multiphase VOF model with the SST k-w solver . I have enabled gravity and implicit body forces. I opened "Open Channel Flow". I canceled to use "Open Channel Flow". However, although cl and residual graphs  converge, free surface didn't change as shown below. 

 

I turned off "Open Channel Flow" and I defined two different velocity inlet for "inlet_air" and "inlet_water". After initializing (compute from "inlet_air"), I defined a region to patch water. however, I get errors like "Turbulent viscosity limited" or "Reverse Flow". I extended outlet place. It was 15c (c refers to chord length), i changed it as 30c but results were same

[Rob]

How does the mesh look around the wing and between the wing and free surface? In a normal wing model we'd set all the fluid flow at some speed and have a fixed wing (see the various tutorials). With a free surface that's not so simple as we'd probably get a hydraulic jump and waves forming. 

[Mehmet D.]

I have successfully validated both 2D and 3D wings under single-phase conditions. Please refer to the attachments for details on my mesh and boundary conditions. To clarify, my wing is stationary and does not move

 

[Mehmet D.]

General view of my mesh and boundary conditions

[Rob]

How does the flow velocity look under the wing? 

[Mehmet D.]

The velocity contour is shown below with a freestream velocity (U∞) of 10 m/s. I am uncertain about how to define the reference pressure location. Additionally, when I change the upper boundary condition from "Symmetry" to "Pressure Outlet," the free surface starts to deform, but I encounter a "Reverse Flow" error. Interestingly, the reverse flow appears near the inlet and at the uppermost part of the domain (i.e., along the upper boundary). The shape and position of the reverse flow change as I adjust the reference pressure location. Still, I use "Open Channel Flow" so I have "Pressure Inlet" BC. I should use "Open channel flow" for my problem or I should use velocity inlet BC ?

 

[Rob]

The location shouldn't matter, and if you're using open channel that ought to solve the water side. However, what is the air density value that you're using?

The velocity field looks a little odd at the free surface, as in I'd expect some gradient between the air and water. Can you replot with node values off and alter the scale to focus on the under wing range (5-10m/s ish). 

 

[Mehmet D.]

Thank you for your quick response. Air density is 1.225 kg/m^3. Contour plot can be seen below

[Rob]

So, no velocity/momentum transfer to the liquid. Can you check it's an interior between the two zones? 

[Mehmet D.]

I’m not entirely sure I understand your instructions regarding ensuring "it's an interior between the two zones." Could you please explain in more detail what steps I should take to achieve this?

[Rob]

You have a very sharp free surface effect which is visible in the velocity result: can you confirm there isn't a wall at the free surface position? 

[Mehmet D.]

After verifying the setup, I confirmed that there is no wall at the free surface position. I reviewed the boundary conditions (shown below) and displayed each one to ensure accuracy, confirming the absence of a wall at the free surface

 

[Rob]

Hmm, if you plot the pressure on the free surface how is it looking? Ie is there enough pressure to cause any deflection? 

[Mehmet D.]

Pressure distribution along the free surface can be seen below. I draw a line along the free surface and plotted the pressure along it

 

[Mehmet D.]

When reviewing similar studies, I noticed that they commonly use a 'velocity inlet' boundary condition, indicating they did not use 'Open Channel Flow.' Additionally, they set the upper boundary condition as 'pressure outlet,' whereas I have it set as 'symmetry.' When I attempted to replicate their setup, I encountered a 'reverse flow at pressure outlet' error. Extending the distance of the 'pressure outlet' did not resolve the issue. I also tried combining the 'pressure outlet' with 'Open Channel Flow,' but the error persisted. I don't believe the distance of the pressure outlet is the cause, as no errors occur when I set the upper boundary to 'symmetry.' I should contibue with "Oepn channel Flow" or I should close it and continue with "velocity inlet" BC ?

[Rob]

OK, and if you use the pressure calculation of dP = rho.g.h how much free surface deflection would you expect with around 30Pa of pressure? 

Open channel is the better option here, but you do need to set the water and air velocity to mimic the flight speed. The problem then is preventing a hydraulic jump as water tends not to want to move overly quickly. You may also trigger air speed derrived waves if you're not careful. 

[Mehmet D.]

Rho = 998.2 kg/m^3, g = 9.81 m/s^2, 30 Pa ==> h = 3.06 10^-3 m. This deflection is so small. I set the velocity water and air same because as I see, I don't have another chance when I use "Pressure inlet" BC.  

 

[Rob]

Open channel has a velocity option, think you need to turn on waves but check the manual. 

[Mehmet D.]

You meant I should open "Open Channel Flow Wave BC" ? When I open it, It is not needed to open "Open Channel Flow, right ?

[Rob]

Have a play, I tend to finish up with both options selected and then don't set a wave type. I no longer have 2021 installed and from memory the panel has changed compared to 2024. 

[Mehmet D.]

I followed your instructions and began the simulation. Initially, I set both the "Open Channel Flow" and "Open Channel Wave BC" with a "Velocity Inlet" boundary condition (BC). By doing this, I realized that I might have disregarded the "Open Channel Flow" since it should actually have a "Pressure Inlet" BC. I also tried the reverse setup.

 

In both configurations, the pressure differential (dP) was minimal and almost identical when I set the upper boundary condition as "Symmetry". I then attempted to change the upper boundary condition to "Pressure Outlet". Interestingly, although the iterations proceeded normally, I encountered a reverse flow error and observed unusual (wrong) velocity contours, as shown below.

 

I wonder what is the reason of this situation, everything is same just I changed upper BC. dP value is also strange but at least it's big. I believe that if I can solve this problem, I'll start to get logical free surface elevation.

[Mehmet D.]

"Have a play, I tend to finish up with both options selected and then don't set a wave type. I no longer have 2021 installed and from memory the panel has changed compared to 2024." 

 

I'm not sure I understand this part. Did you try solving the same problem in the 2024 version and succeed? If so, how did you achieve it? I believe if you succeeded, I should be able to as well. While there may be improvements between the 2021 and 2024 versions of ANSYS, the ability to obtain wave elevation shouldn't be version-dependent.

 

In my case, this time my U∞ is 2.193 m/s, h/c = 1 and the leading edge of the foil is located at 0.

 

[Rob]

No, it's that the panel options may be slightly different, I've not tried running airfoil models like this as I tend to look at ship hulls or weir type features with this sort of model. 

[Mehmet D.]

I managed to deform the free surface, but I encountered an error: 'Reversed flow on 1035 faces of pressure-outlet 8.' The Pressure Outlet-8 is the upper boundary condition. The maximum aspect ratio is around 600, and the maximum skewness is approximately 0.55. When I examine the velocity contour, I don't observe any reverse flow, as I expect to see a region with reduced velocity. I also plotted the streamlines but couldn't identify any issues.

 

I am using the Volume of Fluid (VOF) method with the 'Open Channel Flow' model. Additionally, I have updated my Fluent version to Fluent 2023R1.

 

How can I resolve this problem?

[Rob]

Reverse flow isn't an error, it's a warning. Given the flow is probably more-or-less aligned with the boundary there's a good chance the mass of back flow is fairly low: have a look at the velocity vector plots. Also, have a look at the backflow options in the panel (hint, preventing backflow needs to be used with caution, so don't just look at that). 

[Mehmet D.]

The oscillation in continuity has begun to decrease. The average CFL value on the foil is around 1, and the average y+ is approximately 1. Despite increasing the maximum iterations per time step, the issue remains unresolved. I employed the 'implicit' VOF method. Would it be better to use 'explicit' VOF for my case? If so, will switching to 'explicit' now cause my analysis to diverge, or will it stabilize after some time? The discretization methods I used are detailed in the attached document. Do you have any suggestions?

 

 

[Mehmet D.]

 

I also reduced under-relaxiation factor. Default momentum was 0.3 –> 0.22, Default pressure was 0.8–>0.6, default vof was 0.5--> 0.4

 

[Rob]

Not sure you need the transition model for turbulence, that may not be helping here. 

Explicit is better for free surface resolution, but given the domain scale I'd stick with Implicit as it may require a much smaller timestep.