Understanding mode shapes

[jacob_poulsenYNQP9]

Hi

I´m fairly new to Nastran(2022) an vibration analysis as a whole, and I´m having some trouble understanding the mode shapes output from both modal and direct frequency response analysis. 

To start simple, I modelled a cantilever beam, and used the Normal Modes analysis to find the first 4 mode shapes and frequencies - they looked as expected, and the natural frequencies align with what I calculate analytically. 

In order to determine the stresses and displacements at a sinusoidal acceleration excitation of 1G at the base of the beam, I setup a Modal Frequency Response analysis, and while I get somewhat realistic results in terms of displacements, the deformation plots at the natural frequencies look non-physical:

 

I looks as if the sign-error, as the deformation is opposite that of the mode shapes(at some parts of the beam). I know it doesn´t impact the results in this particular analysis, as the displacements and stresses are both zero at the sharp bends, but it looks incorrect, and I´d like to know whether it´s my simulation setup or my understanding that is off?

I also setup a Direct Frequency Response analysis and excited the beam at it´s 4 first natural frequencies with a sinusoidal load of 1G, and the results was equal to that of the Modal Frequency Response analysis.

Thanks in advance, 
Jacob

EDIT: Please ignore the dynamic setup of the Direct Frequency Response analysis. I was simply trying to investigate what happened if I excited the beam at its natural frequency without damping - it went to infinity as expected. 

[John_Holtz · Accepted solution]

Hi Jacob. Welcome to the Inventor Nastran forum.

See if the description in this article is the explanation for your result: Nastran In-CAD: displacements not in direction of load in Frequency Response analysis. 

Essentially, the result at some forcing frequency is the combined contribution from all the natural frequencies. In order to combine the different natural frequencies an SRSS (square root sum of the squares) is used which makes all the displacements positive.

John

[jacob_poulsenYNQP9]

Hi John

Thank you very much!

That makes really good sense, I had a feeling it had something to do with the summation.
I´m wondering how I should handle the dynamics options when looking at the stresses though. If I want to determine the maximum stresses in the slender rod at its 1st natural freq., should I choose 'Phase' and look at 'Magnitude' or should I choose 'Real' and look at 'Real' - I have a feeling it´s the last option?

Thanks again, 
Jacob

[John_Holtz]

Hi Jacob,

I agree that looking at the "Real and Imaginary" results is easier to understand from a physical point of view. For example, the Solid Z-Normal stress shows tension on the top and compression on the bottom due to bending, as expected. The "Magnitude and Phase" results are positive on the top and bottom become of how the results are combined from the multiple modes.

However, the "Real and Imaginary" results need to be combined manually to get the total stress. That is going to take work, especially for stress results like the von Mises or Principal stresses. The von Mises stress due to multiple results is not the sum of the von Mises from the individual results. The Solid X, Solid Y, Solid Z, Solid XY, Solid YZ, Solid ZX are the sum of the two results, then the von Mises is calculated from those 6 results. Not fun.

John

[jacob_poulsenYNQP9]

Okay, that sounds tedious - Just to make sure I understand correctly, this summation is not required when looking at the Von Mises stresses from the "Magnitude and Phase" results? 

- Jacob

[John_Holtz]

Correct.

• The magnitude results is based on the total amplitude, so nothing more needs to be done. The phase result is an angle (degrees if I remember correctly, but it could be radians also).
• The real and imaginary results are both components that need to be combined to give the total amplitude.

John

[jacob_poulsenYNQP9]

Perfect, your help is much appreciated John!