[Julian121]

Dear all,

I am simulating the flapping motion of a wing using Fluent to calculate lift and drag coefficients. I have used a UDF code and dynamic mesh to simulate the flapping motion.

I am simulating a rigid wing which has pitch and roll rotations and have defined four boundary conditions:
1- Pressure far field
2- Wall
3- Wall-solid
4- Interior-solid

I am defining the x,y,z components of the airflow using pressure far field boundary and assume that the flow is static and the wing moves.

What force direction should I use to calculate lift force?
Do I have to run the solution at steady first and then transient?

I would appreciate if anyone help me with this.

[cfd seeker]

Originally Posted by Julian121

Dear all,

I am simulating the flapping motion of a wing using Fluent to calculate lift and drag coefficients. I have used a UDF code and dynamic mesh to simulate the flapping motion.

I am simulating a rigid wing which has pitch and roll rotations and have defined four boundary conditions:
1- Pressure far field
2- Wall
3- Wall-solid
4- Interior-solid

I am defining the x,y,z components of the airflow using pressure far field boundary and assume that the flow is static and the wing moves.

What force direction should I use to calculate lift force?
Do I have to run the solution at steady first and then transient?

I would appreciate if anyone help me with this.

lift coefficient depends on angle of attack....in monitor panel give values of the cos and sine components at which you performing your analysis and run steady solution solution for static case without UDF so that flow develops and then switch to transient case and hook UDF to simulate flapping motion

[Touré]

I totally agree with cfd seeker. If you want to automate it, you can use parameters to change the angle but I wouldn't recommend that. The process would be:
1. Create a new project
2. Choose an angle alpha
3. Check the force Fy on Y-axis
Redo the process for several alpha until you get a curve or Lift versus alpha. It's better to do one alpha per project so that if it crash you wont loose all your other simulation.
For example, if you want to simulate alpha = 20, you can load a previous solution data of alpha = 10 so that the computing will be less difficult for the software to converge to the solution.
To find Fy (figure 1), go to Report -> forces ; Fy = Lift (Fx= Drag)
If you really want to use your UDF, you must save the data for the several times with Autosave (figure 2). Then, you will check the alpha and the corresponding Fy for each saved time data .

[Julian121]

Since I am simulating flapping motion of a wing and not a static airfoil, the lift force varies at different wing positions. How can I plot the lift force over time?
If I use Forces option in Fluent, it only gives lift at a particular wing position and not total lift over time.

[Touré]

Fluent loads only the flow-field data of one time step and not all of them but maybe you can do this in FLUENT

Report -> forces -> Save Output Parameter

You will see the Parameter set at the bottom of the project (see figure).
Double click on it to check the values

[Julian121]

Thank you for your reply. As the direction of lift changes during the wing motion, how can I define the direction of lift force while the direction changes at each wing position?

[Touré]

Maybe you're talking about the projection of the Lift. The Drag (Fx) and Lift (Fy) which are orthogonal never change direction. The lift is always on the same direction as the gravity (vertical) and the drag is horizontal even if you wing moves. I don't think that FLUENT gives the projection of the Lift on the new position of you axis when they rotate and I don't think that you really need to compute it. I suggest simply Excel or Matlab to compute the projected Lift forces if you really want them by multiplying the Lift with cos(alpha) or sin(alpha) .

[cfd seeker]

Originally Posted by Julian121

Since I am simulating flapping motion of a wing and not a static airfoil, the lift force varies at different wing positions. How can I plot the lift force over time?
If I use Forces option in Fluent, it only gives lift at a particular wing position and not total lift over time.

I guess you are talking about the variation of lift as the wing flaps with time....its simple just go to Monitors and put the sine and cos components of angle of attack and also check plot and print tabs.....by this way you will get the variation of lift with time as it goes from positive to negative until a cyclic behavior which shows convergence of your problem....

[Touré]

Monitors -> Create (Lift)

[Julian121]

Originally Posted by Touré

Monitors -> Create (Lift)

I started the simulation and solved the problem in steady-state first. However, when I change the steady state to transient problem, the mesh quality decreases and I get an error:


Static mesh:
Minimum Orthogonal Quality = 0.6

After clicking on the preview motion:
Minimum Orthogonal Quality = 0.00000e+00

Warning: non-positive volumes exist.

Primitive Error at Node 0: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 1: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 2: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 3: Update-Dynamic-Mesh failed. Negative cell volume detected.

Error: Update-Dynamic-Mesh failed. Negative cell volume detected.
Error Object: #f

Any idea what I should do?

[cfd seeker]

Originally Posted by Julian121

I started the simulation and solved the problem in steady-state first. However, when I change the steady state to transient problem, the mesh quality decreases and I get an error:


Static mesh:
Minimum Orthogonal Quality = 0.6

After clicking on the preview motion:
Minimum Orthogonal Quality = 0.00000e+00

Warning: non-positive volumes exist.

Primitive Error at Node 0: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 1: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 2: Update-Dynamic-Mesh failed. Negative cell volume detected.

Primitive Error at Node 3: Update-Dynamic-Mesh failed. Negative cell volume detected.

Error: Update-Dynamic-Mesh failed. Negative cell volume detected.
Error Object: #f

Any idea what I should do?

negative volumes are appearing during re-meshing process....decrease your time step size.........

[Julian121]

Originally Posted by cfd seeker

negative volumes are appearing during re-meshing process....decrease your time step size.........

I have reduced the time step to 0.0001 but still does not work.

[cfd seeker]

Originally Posted by Julian121

I have reduced the time step to 0.0001 but still does not work.

try step size of 0.000001....what are your flow conditions?

[Touré]

It's maybe because of a coarse mesh. Maybe you need very small elements in the zone where you have your movement (trailing edge) at the beginning of the simulation. The dynamic mesh destroys the quality of your meshing, so do your best at the beginning.

[Julian121]

Originally Posted by Touré

It's maybe because of a coarse mesh. Maybe you need very small elements in the zone where you have your movement (trailing edge) at the beginning of the simulation. The dynamic mesh destroys the quality of your meshing, so do your best at the beginning.

I refined the mesh at the trailing edge but it did not work. Still, I get that error. I do not understand why Minimum Orthogonal Quality changes during the simulation. When the time step is 0.0001 the simulation goes up to 20 while the time step is 0.00001 it goes to 228 and then stops.

Is the error because of the mesh? I have tried tri/quad coarse/fine mesh but still does not work.

[Touré]

Did you select "Remesh" when you have selected "Dynamic Mesh" ?
Use "Previewing the Dynamic Mesh" button, so that you see what is going on before running your simulation.
The "Minimum Orthogonal Quality" should change because the cells on the boundary of your airfoil moves making their angles to change also.

[Julian121]

Originally Posted by Touré

Did you select "Remesh" when you have selected "Dynamic Mesh" ?
Use "Previewing the Dynamic Mesh" button, so that you see what is going on before running your simulation.
The "Minimum Orthogonal Quality" should change because the cells on the boundary of your airfoil moves making their angles to change also.

Thank you very much Touré for your help.

I have got five zones in dynamic mesh zones: interior-solid, pressure_far_field, solid (fluid), wall and wall_solid

Which zone should be stationary or deforming? Should all of them be deforming except the wall-solid which does rigid body?

When I set every zone to stationary except the solid(fluid) to deforming and wall_solid to rigid body, I don't get any negative cell error.

[Touré]

You 've got it.
Stationary is for the boundaries that are not moving like your far-field and the two symmetrical boundaries
Deforming is for a deforming boundary or zone such as your fluid
Rigid body is your airfoil and you have to link it with your motion after compiling the code.c file
Did you use "Peview Mesh Motion" before doing the computation?
Keep going

[Julian121]

Originally Posted by Touré

You 've got it.
Stationary is for the boundaries that are not moving like your far-field and the two symmetrical boundaries
Deforming is for a deforming boundary or zone such as your fluid
Rigid body is your airfoil and you have to link it with your motion after compiling the code.c file
Did you use "Peview Mesh Motion" before doing the computation?
Keep going

The problem still exists! When interior-solid is stationary, the minimum orthogonal quality remains constant and the error does not appear. However, when interior-solid is stationary, no motion is seen by using "preview motion".

What is the difference between solid (fluid) and interior-solid zones? Should it be deforming? When I change interior-solid to deforming, the error appear again.

The wing tips remain in the domain during the movement of the wing.

[Julian121]

Originally Posted by Touré

You 've got it.
Stationary is for the boundaries that are not moving like your far-field and the two symmetrical boundaries
Deforming is for a deforming boundary or zone such as your fluid
Rigid body is your airfoil and you have to link it with your motion after compiling the code.c file
Did you use "Peview Mesh Motion" before doing the computation?
Keep going

The lift coefficient curve shows that it varies between 0.75 to 0.76 which seems to be wrong. Should not it go to minus value during downstroke? I have attached a screenshot of the lift curve. Do I have to do the calculation through "Run calculation", as when I preview the motion the lift curve starts drawing?