# Applying External vibration (shaker simulation)

• 630 Views
• Last Post 31 July 2019
• Topic Is Solved
HamzaBaqasah posted this 14 July 2019

Hello everyone,

I'm trying to simulate a cantilever beam that is fixed from one end and free from the other end.

From the fixed end, I want to apply a displacement at certain frequency (such as 30Hz at +/- 0.4 mm).

by harmonic analysis, what kind of load should I apply here? is it displacement? but then how can I adjust the frequency?

Appreciate your help as I'm recent user of ANSYS workbench.

Regards,

Hamza

peteroznewman posted this 15 July 2019

An efficient way to do this, if you can accept a linear model, is to create a Modal analysis and drop a Harmonic Response onto the Solution cell of the Modal. That will allow you to apply an Acceleration as a Base excitation on the Fixed Support. Just convert the displacement specification of +/-0.4 mm at 30 Hz to the equivalent 14.2 m/s^2 acceleration. In the Analysis Settings, specify the frequency range, for example 25 - 35 Hz with 10 steps.

An ANSYS 2019 R2 archive is attached.

Attached Files

• Liked by
HamzaBaqasah posted this 28 July 2019

Hi Peter,

I appreciate your support. The attached file is not working.

However, I applied what you explained above and I don't know why I'm not getting the results as amplitude.

The attached photo show what I did.

Regards,

Hamzah

peteroznewman posted this 29 July 2019

Pick a vertex on the geometry where you expect to see a significant response. In the Harmonic Response system, under the Solution Branch, insert a Frequency Response for Acceleration, Velocity or Displacement. That will generate an amplitude of response vs frequency plot.

• Liked by
HamzaBaqasah posted this 29 July 2019

Hi Peter,

Thanks for your reply I could find the amplitude but it's not reasonable may be due to my inputs.

Could you please the first image that shows my inputs in acceleration details? also, in the second image, the arrow is only directing to the top where my shaker is going up and down.

Best regards,

Hamza

peteroznewman posted this 29 July 2019

What is the displacement result?  What do you think is a reasonable value?

Please attach a .wbpz archive file of your project so I can take a closer look.

• Liked by
HamzaBaqasah posted this 29 July 2019

The amplitude value is very high compared to the length of the beam.

Second, the arrow is only directing towards the top. I don't know if it's okay since I want to simulate the shaker where it moves up and down.

The project file is attached.

HamzaBaqasah posted this 29 July 2019

Dear Peter,

I'm afraid my project file is too large to be uploaded in this website.

HamzaBaqasah posted this 29 July 2019

Dear Peter,

Thanks,

Hamzah

peteroznewman posted this 30 July 2019

The acceleration arrow direction is for up and down along that axis.

Your model has a mistake, the acceleration is 14.2 m/s^2  You typed 12.4 mm/s^2.
Insert a Frequency Response for Displacement of a vertex at the fixed end and you will see the 0.4 mm amplitude at 30 Hz.

The amplitude is high because you did not include any Damping in the model.
You have to enter some amount of damping, say Damping Ratio = 0.01 = 1%

With 0% Damping Ratio, there is a 267 mm displacement at the tip at 24 Hz.

With 1% Damping Ratio, there is a 48.7 mm displacement at the tip at 24 Hz.

With 2% Damping Ratio, there is a 24.7 mm displacement at the tip at 24 Hz.

Keep in mind that this is a linear analysis. When the deflections get too large, the small rotation assumption in the linear model is no longer valid. In that case, you have to perform a Full Transient and turn on Large Deflection in order to see the true deformation.

Also, Insert a Mesh Control Method called Multizone on the body.

Attached Files

• Liked by
HamzaBaqasah posted this 30 July 2019

Hi Peter,

Thanks for your help I appreciate that.

I just need to know the amplitude when running it at its natural frequency and I think this gives me an idea especially when I want to compare it with another same geometry but has higher crack depth.

another question is does phase angle effects the results? I have used 90 degrees. should it be 0?

Regards,

Hamzah

peteroznewman posted this 31 July 2019

In your case, since there is only one load, the phase angle is irrelevant, 0 and 90 give the same answer.

Phase angle matters when you have two or more loads and you want to specify if they are in sync or out of sync.

• Liked by
HamzaBaqasah posted this 31 July 2019

Thank you Peter. That was very helpful!