Learning Forum

[jil260]

I am doing a fluid-structure interaction simulation and want to know the natural frequency of the structure(cylinder) to do the analysis.

[peteroznewman]

Define the geometry: length, diameter, wall-thickness (or solid) for the cylinder.

Define the material: Young's Modulus, Poisson's Ratio, Density

Define the supports on each end of the beam:  Fixed, Simply Supported or Free (Cantilevered).

That completely defines the problem to compute the natural frequency.

[jil260]

10 meters long, 0.5m diameter, solid;

density:1120kg/m^3; poisson's ratio:0.48; it's a non-linear material (silicon rubber) ansys data does not show Young's modulus;

both end sides are fixed. Thank you.

[peteroznewman]

The range in Young's Modulus is huge!  If I take the Average value from this site, the first natural frequency is 1.2 Hz and the second is 3.2 Hz.

If you could narrow down the range of the modulus, that would be good.  Or if you have a physical sample, there are tests that could be performed.

Another factor is tension. A small amount of tension would greatly increase the natural frequency.

[jil260]

Here are more details all I have. How did you figure this out? Is there any application or formula?

[peteroznewman]

The slope of the blue line is the linear elastic property of Young's Modulus. Estimate the slope at a small strain, like at 0.1 and it would come out to about 1.8 MPa.  The value I used in the first model was 80 MPa so the natural frequency will drop significantly. The first natural frequency is now 0.18 Hz and mode 2 is 0.48 Hz.

[jil260]

Could you please tell me how to calculate this? I may change the geometry or materials in the later simulations.

[peteroznewman]

In Workbench, double click on Modal.

Open Engineering Data, create a New Material, drag the Density Property onto it and enter the data. Drag the Isotropic Elasticity property onto it and enter the Young's Modulus and Poisson's Ratio.

Open Geometry and create the cylinder in SpaceClaim, close SpaceClaim.

Open Model and apply a Fixed Support on each end.  Solve. 

Click on Solution Information, it will show you a table of natural frequencies.

The default mesh may be okay, you can enter a smaller element size to see if the results are consistent.

[jil260]

Is the natural frequency the same in water as in air since the former includes the effect of added mass?

[peteroznewman]

The natural frequency of the cantilever is a calculation based on its mass and stiffness so air or water are irrelevant.

If you excite vibrations in the cantilever, the surrounding fluid will have an effect on the damping of those vibrations.

Water will have high damping compared with vibrations in air.

[jil260]

May I ask why the frequencies of 1 and 2 (3-4,5-6) are so close? As you mentioned before, mode 2 is 0.48Hz, so it's the third one instead of the second listed above?

[peteroznewman]

A circular beam along the Z axis can vibrate sideways in the X direction, or it can vibrate sideways in the Y direction.  ANSYS finds both of those solutions. The exact solution is that it can vibrate sideways in any direction as mode 1.  The same goes for the higher modes, ANSYS finds the X and the Y vibrations which have the same modal frequency. You could call that pair mode 2 and the following pair mode 3, even though ANSYS is up to 6 modes.

[miel]

Just to make sure you don't get it wrong.

You need to include the effect of the added mass. You'll see that immediately when you write up the equations of motion for the beam and the fluid. The reason is that it affects the inertia term as the fluid force is proportional to the accelleration of the beam - so in other words, when you calculate the eigenfrequencies there will be a contribution from this.