[androm]

Hello,

I am trying to do heave mode for airfoil using the dynamic mesh method in CFX. I have tried several boundary and setup but my result could not approach the test data. The topology is c_grid, the inlet and the outlet, I used the wall boundary condition with specified displacement and y component equation is amplitude *sin(2*pi*f*t)and the upper and lower boundary, I used opening with the specified displacement and y component is the same equation as the other boundary, the airfoil boundary is rigid body with no slip wall. the front and back of the domain is symmetric.

The paper that I used to compare my result with is using the whole grid as rigid body. However, in my case, I used only the airfoil as rigid body. How do I specify the whole domain and the airfoil as rigid body and allow it to do the motion? can anyone help me with that?

Thanks In advance,

Andrew Metry

[Opaque]

ANSYS CFX does not support mesh motion on inlet/outlet or opening unless the motion of the mesh is completely tangential. Your experience may vary.

To move all the mesh as a whole, create a sub-domain, and impose the mesh motion you want on the sub-domain.

[androm]

Thank you for your reply.

In the case of subdomain, I will not be able to use the mesh as structure mesh, I have to use unstructure one. Is there a way to use the structure mesh with the subdomain option?

When you said subdomain, you mean that I use the interface like the one in chapter 32 in the CFX tutorial or you meant that I use the subdomain option in the insert bar of the domain default, and I select the inner domain and give it the motion?

In other words, I know that since there is two domain, there should be interface but my confusion is whether I use the subdomain option in the insert bar of the domain default or not?

For any cases, do I use the wall boundary option for the inlet and outlet or use the inlet boundary for inlet and outlet boundary for outlet separately?

what is the best shape for the inner domain, cubic or cylinder, or C shape, as the outer domain will be C shape?

I am waiting for your kind reply.

Thanks in Advance,
Andrew Metry

[Opaque]

I meant subdomain in the ANSYS CFX sense, that is, it is a region of the mesh (structured/unstructured) to which you can certain physics. In this case, mesh motion.

Definitely, a circular mesh (2D view) around the airfoil will avoid the numerical issue at inlet/outlet/opening. There is no need of changing the boundary type if the motion is tangential to the boundary definition.

Hope the above helps

[ghorrocks]

Looking at your fundamental setup - why are you modelling this as a CFD/rigid body simulation? A MUCH easier way of doing it is to model a series of angle of attacks in steady state to give you a lift/drag versus AOA curve, then do a quick ODE solver outside of CFX to model the motion using your simulated AOA curve (python/matlab/wahtever). Is this approach suitable for your case?

[androm]

I appologize, I did not see yours messages yesterday.

I need to do it using CFD, since the test data is using CFD software, and the reason is to encounter the viscous effect of the flow. For ODE, there is some test data about it but it is without including the viscous effect. The motion that I am doing is not changing the AOA, and the AOA is constant, however, the airfoil itself should move up and down to produce the full motion that I am studying.


For the CFX, I have tried the mesh deformation but it limits me to increase the number of layer around the airfoil as when I increase the number of layer, I got an errors like negative volume or so and even if I increase the time step and increase the stiffness, the error still come out but later in the solver and it is not reasonable to increase the time step more since the result is the same as the one I got without increasing the number of layer around the airfoil, which is not near the test data. After that, I was thinking that the rigid body option may solve this issue.

Until now the only way that works with the rigid body option is to make the inlet and outlet as wall boundary, if I used the inlet and the outlet as inlet boundary and outlet boundary I will get an error finmes. However, I think the answer may not be the same as the test data, I will leave it to run, and see after that the result. May I ask you question when the result is out and wrong?

Thanks for your replies.
Andrew Metry

[ghorrocks]

Negative volume errors are a FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

Can you explain what motion you are expecting? If the motion is not AOA then what is it?

[androm]

The motion is called plunging motion which is moving the airfoil up and down with a hormonic motion. In my case, I am using the sinusoidal hormonic motion. In this motion, the frequency and amplitude of the motion are constant for running one case (using one value for frequency and one value for amplitude), for next case, I change the frequency and amplitude and after finishing all cases, I take this data and study it.

[ghorrocks]

Then this is not a rigid body simulation but it is a moving mesh only simulation, because you know the position of the body at all times in advance.

If the moving mesh is not working for you then you have a few options:
* Add a remeshing step when the mesh quality deteriorates below a threshold
* Generate all the meshes before the simulation and store them as a series of mesh files. This is a moving mesh simulation, but instead of using the mesh displacement diffusion algorithm use a user fortran routine to read in your pre-generated meshes.

[androm]

Is this different from the mesh defromation?

I have tried the mesh deformation and I get result from it when I use not many layer around the airfoil, and the result is far from the test data. When I increase the number of layer around the airfoil, I get error either fatal overflow or negative volume, I have tried to increase the number of step to 5000, and I used the mesh stiffness, increase near small volume, and the model exponent is 200000, and the solver works for several number of time step and then spell out the error and it was negative volume, If I increased the number of step, it is time consuming and the result that appears is not near the test data. That is why, I thought may be the rigid body method solve this issue.

Do you mean that I generate the mesh for each displacement and read it by CFX_Pre as several cases?

[ghorrocks]

No. I gave two options:
* dynamic remeshing
* pre-generated meshes, read in via a user fortran routine.

If you want to look into dynamic remeshing have a look at the ANSYS customer site for examples.

If you want to look into pre-generated meshes it is a bit trickier. Many versions ago in CFX there was a user fortran example which did this. But it was removed from CFX installation many versions ago. I would recommend you talk to ANSYS support and see if the mesh deformation via user fortran example is available.

[androm]

Thank you, I will try to contact them but they take much time to respond, like 10 days or so. I will contact them and see If they have examples about dynamic remeshing or pre-generated meshes read in via a user fortran. I am not on customer portal, I have signed up but I think this is expensive service like $2000 or so.

Do you know the name of the topic to this examples?

[ghorrocks]

For the dynamic remeshing search for dynamic remeshing.

The customer portal and support is for paid customers. It has lots of good support information and examples - and that is why it is worth paying for it.

You are doing quite a difficult simulation so it is worth paying some money to get a good start on it. The free resources are only suitable for beginner level simulations, and your simulation is beyond a beginner simulation.

You can also try google and youtube, there are some useful resources there.

[androm]

Thank you for your replies. I will see when they reply to me with the price, if I can afford it now, I will buy but if not I will buy it in the future since I will need to advance myself using CFX.

I have question about the lift coefficient. The lift coefficient is the force in y direction, this force should include the pressure and shear effect. I have been using the following equation to get the lift coefficient; force_y()@Airfoil/q where q is 0.5*density*velocity^2*Area. However, I think this equation is not accurate since the force_y direction function in CFX only count the pressure, as I understand from previous post. I have came across function about how to get the force in x direction and y direction but I do not know if they are right. The equation is as follow, force_X = areaInt_X(Pressure)@Airfoil + areaInt(Wall Shear X)@Airfoil, and the same for y but changing the x to y, Is this equation correct to calculate the drag from it and the same for lift but changing the x to y?

[ghorrocks]

I think this equation is not accurate since the force_y direction function in CFX only count the pressure, as I understand from previous post.

No, my understanding is the force_x/y/z() function includes both pressure and shear components. But why listen to me? Do a test case with flow over an object and get the force and work out for yourself what is correct. Figuring it out for yourself is always the best approach.

[androm]

I was using the force in x or y direction to get cl and cd, I thought that the force include the pressure and shear components, yesterday, I was searching how does CFX caluclate the force in x direction or so? I saw two or three thread mentioned that the force is caluclated by PressureXNormal area, this defination is correct but this may ignore the factor of shear in calculating the force, In the study that I am doing I got one result equal to one of the test data which rely only on pressure force to calculate the lift and drag coefficient, but the other test data I cannot confirm, and when I read this posts, I doubted myself about the defination of force, so I wanted to take second opinion about what I understand. I will give a try to confirm that the force_x/y/z() function includes both pressure and shear components. Thank you very much for your replies.