Learning Forum

[kimkarimi9574]

Hi there!

Does Anybody know how I can get the amplitude of vibration for each mode shape in a 3D problem in ANSYS modal?

Thanks in advance!

[Akshay Maniyar]

After the solution is complete, you can review the mode shapes for each frequency.
Step 1: Select the Solution branch of the outline
Step 2: Select the Frequency column of the Tabular Data
Step 3: Right-mouse-button, Create Mode Shape Results
Step 4: Evaluate Results
Thanks amaniyar

[kimkarimi9574]

Thank you very much for your answer! Which one of deformations (directional or total) is the amplitude?

[Akshay Maniyar]

In aModal Analysis(and other eigenvalue-based analyses such as buckling), the solution consists of a deformed shape scaled by an arbitrary factor. The actual magnitudes of the deformations and any derived quantities, such as strains and stresses, are therefore meaningless. Displacements, stresses, strains, etc. reported with mode shapes are ÔÇ£relativeÔÇØ and do not reflect the actual magnitudes.
Can you explain what you want to calculate from modal analysis?
Thanks Amaniyar

[kimkarimi9574]

I want to calculate peak displacement of a fluid conveying rubber pipe. I applyed all the required settings but the final results of deformations are considerably greater than experimental results. So, I want to make sure I'm considering the right output as amplitude.

[Akshay Maniyar]

Why are you doing modal analysis? From the image you shared, I am not able to figure out it.
Amodal analysisdetermines the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component. It can also serve as a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic analysis, or a spectrum analysis.

Thanks Amaniyar

[kimkarimi9574]

Because I'm trying to validate a paper and the given results are peak displacement and natural frequencies, so I guessed the best fit would be modal analysis.
The first picture was problem description and this picture is the result.
Thank you so much for your help!
Best wishes Kim

[kimkarimi9574]

This is the paper

[peteroznewman]

Hi A harmonic response analysis will compute the displacement amplitude of the pipe for a specific harmonic input. In Figure 5 shown above, the pinned supports have a lateral sinusoidal displacement amplitude of 0.012 m

[kimkarimi9574]

In harmonic response, I don't know how to set the sinusodial displacement. Because it doesn't have function option. Could you please tell me how I can do so?
Thank you very much!

[Erik Kostson]

You just need to add the displacement there - so say 0.001 m in Y or whatever you have and that will be sinusoidal since it is a harmonic (sinusoidal loads/boundary conditions are assumed) analysis.
As a side and something that might be relevant.
If you are looking into the effect of the fluid conveyed in the pipe on the pipe vibration (Coriolis effect - so exerted pressure from fluid flow on the pipe wall during vibration), we need to use a coupled vibroacoustic analysis (Harmonic acoustic system with fluid as acoustic and pipe as structural region) with mean flow effect (convective acoustic equation is used with - see BF,,VMEN command for mean flow).

Not sure if this helps.
Erik

[peteroznewman]

that's awesome!

[kimkarimi9574]

Thanks a million, guys for your help! I could finally gain the correct answer, using your guidance. I appreciate it