[Mid Grove]

Dear all

I’m researching a propulsion mechanism in fluid using an oscillating fin. I’m trying to simulate a 2 - way FSI simulation (2D) of an oscillating flexible fin. The objective is to achieve the thrust force generated by oscillating the fin.

This approach is similar to Tutorial No. 23 Oscillating Plate.

The flexible fin system consists of some materials as shown in the attached image. And the fin has been modeled as solid body in DM. The fluid domain is rectangular cuboid.
The setup conditions of Mechanical ADPL and CFX were as follows.

< Mechanical ADPL >
Analysis Settings
-Step End Time: 6s,
-Auto Time Stepping: On
-Define by: Sub Steps
-Initial Sub Step: 1
-Minimum Sub Step: 1
-Maximum Sub Step: 10

Remote Displacement
Scope
-Coordinate System: Global Coordinate System
(The z-axis is the same as the rotational axis)
Definition
-Rotation Z: 4.e0*atan(1.e0))/6*sin(2*(4.e0*atan(1.e0))/3*time

<CFX>
Total Time: 6s, Time step: 0.001s
Coupling Data Transfer Control
-Under Relaxn. Fac.: 0.3
-Convergence Target: 1e-5

I received the error message that the fatal error occurred when requesting Total Mesh Displacement for FF when simulation time = 0.256s. FF is FSI interface. And also the image of mesh deformation right before the error message had occurred (simulation time = 0.255s) was attached.

I estimate that this error was caused by less-accuracy mesh of structure. I next created finer mesh of structure and simulated. However, the same error message as the above occurred. Therefore, I stopped the simulation right before the error message had occurred. By the simulation results, the gap between the interface of structure (Mechanical ADPL) and that of fluid (CFX) was occurred. This is first question: Why does the gap between those interfaces occurred?

I created some mesh of structure and fluid using ANSYS Meshing for improving the accuracy of the mesh and simulated using those meshes. The tendency for the mesh deformation for each time step decreased by fining of the mesh was observed from those results.
Next question: How is the mesh set to improve both the value of mesh deformation for each time step and the mesh accuracy?

Any help will be very much appreciated. Thanks in advance.


Mid Grove

[Vinzent]

hi,
try different meshstiffnesses. the gap region (connection) should be softer than the surrounding.
vinzent

[brunoc]

Use a fixed timestep for the structural side of your simulation. The timescale for the fluid simulation is probably smaller anyway. Then play with the mesh stiffness on CFX. Use the option where stiffness if bigger near walls or boundary conditions.

[stumpy]

As bruno said get rid of the auto timestepping in ANSYS and just use 1 substep. Your under relaxation factor of 0.3 is also very small. This means CFX only gets 30% of the change in displacement from ANSYS each coupling iteration, so you'll need a lot of coupling iterations to get the meshes to match up.

[bbhv]

have you checked your scaling?
especially when you import the geometry from another software.
i experienced it once, the design modeller scaled the model automatically.
so, make sure they are the same in the structural and fluid models.

[Mid Grove]

Thanks all.
I tried simulations in some different conditions. In the results, it succeeded by setting up as follows.
< Mechanical ADPL>
Analysis Setting
-Step End Time: 6s
-Auto Time Stepping: Off
-Define by: Substeps
-Number of substeps; 1
<CFX>
Total Time: 6s, Time step: 0.01s
Mesh stiffness: 1000[m^5 s^-1] / (max (0.1[mm], wall distance)^3
Under relaxation factor: 0.30 (minimum iteration: 3, maximum iteration: 30)
Convergence Target: 0.01
And crushing of a mesh was prevented by making a sliding interface in the fluid around a fin. But, Computational time is too long and is troubled.
Please teach me how to decrease computational time? Computational time has taken no less than 12 days.

[stumpy]

Use an under relaxation of 0.75 or higher, so fewer coupling iterations are needed. If this is unstable, then use an under relaxation factor of 1 then add a 'mass flux pressure coefficient' on the FSI boundary on the Source tab. If you have access to the ANSYS Customer Portal then you can see how this works by searching for "FSI" in the knowledge resource section (it's the first hit).

[Mid Grove]

Thanks stumpy.
I'm sorry I have much slower response.
Using the mass flux coefficient, calculation is finished in two days.