Modal analysis - Input and boundary conditions given?

[k.udhay]

TL;DR Summary

In modal analysis, why is there no force excitation given as input? If there is no input how can the software or method predict a vibration mode?

My understanding in modal analysis is very limited. All I know is it helps to find a specific mode of vibration and the natural frequency corresponding to it.

While I was discussing about this with my NVH team colleague, he told me that there is no force input or excitation input given to a modal analysis. I also saw a modal analysis report and it gave a lot of different modes with corresponding natural frequency, without indication any direction or magnitude of load input.

These are my questions:
Assuming modal analysis of a simple shaft is to be carried out,

1. What are the typical boundary conditions given (For example, radially two ends fixed, rotary motion constrained etc.)?
2. If there is no force input given, why should a shaft vibrate and how is it captured as a mode?

Because I am unclear, I am unable to put more specific questions. Perhaps with your answers, I can think of more questions and I can work on finding the answers too. Thanks.

 

[jrmichler]

Modal analysis has two meanings:
1) Measuring the modal frequencies and shapes using accelerometers.
2) Calculating modal frequencies and shapes using FEA.

You are apparently asking about #2, calculating modal frequencies and shapes. The FEA software calculates these from the mass and stiffness matrices. The calculation is exactly similar to calculating the natural frequency of a simple spring - mass system, except the FEA model has many masses and springs.

Since you are calculating ratios of masses to spring constants, there is no need to apply a force. The actual calculation involves calculating eigenvalues and eigenvectors, which is a fairly simple matrix calculation.

Given the above, you should be able to use search terms modal analysis, FEA modal analysis, FEA modal eigenvalue eigenvector to learn more. If it seems like a lot of work, note that modal analysis is a full semester course at the senior level in a mechanical engineering curriculum.

 

[k.udhay]

Thank you

Modal analysis has two meanings:
1) Measuring the modal frequencies and shapes using accelerometers.
2) Calculating modal frequencies and shapes using FEA.

You are apparently asking about #2, calculating modal frequencies and shapes. The FEA software calculates these from the mass and stiffness matrices. The calculation is exactly similar to calculating the natural frequency of a simple spring - mass system, except the FEA model has many masses and springs.

Since you are calculating ratios of masses to spring constants, there is no need to apply a force. The actual calculation involves calculating eigenvalues and eigenvectors, which is a fairly simple matrix calculation.

Given the above, you should be able to use search terms modal analysis, FEA modal analysis, FEA modal eigenvalue eigenvector to learn more. If it seems like a lot of work, note that modal analysis is a full semester course at the senior level in a mechanical engineering curriculum.

Thank you for the detailed reply. I will indeed learn more from online resources.

My basic question is in a simple spring mass system, we at least have a directional constraint assumed in the calculation. For example, spring is assumed to vibrate along its axis. But on a random physical component, how is the direction of vibration assumed?

 

[FEAnalyst]

Modal analysis, understood as eigenfrequency extraction procedure, solves the following equation: $$(K- \lambda M)q=0$$ where: K - stiffness matrix, $\lambda$ - eigenvalue, M - mass matrix, q - eigenvector.
The right side is zero because the force vector is ignored in this type of analysis. The equation is a typical eigenvalue problem known from linear algebra.
When it comes to boundary conditions, they should represent real life constraints of the system as closely as possible. In case of modal analysis you don’t have to worry about underconstraint like you would have to in case of static simulation (modal analysis can be performed even without any boundary conditions at all). For shafts just apply proper restraints in place pf bearings.

 

[k.udhay]

Modal analysis, understood as eigenfrequency extraction procedure, solves the following equation: $$(K- \lambda M)q=0$$ where: K - stiffness matrix, $\lambda$ - eigenvalue, M - mass matrix, q - eigenvector.
The right side is zero because the force vector is ignored in this type of analysis. The equation is a typical eigenvalue problem known from linear algebra.
When it comes to boundary conditions, they should represent real life constraints of the system as closely as possible. In case of modal analysis you don’t have to worry about underconstraint like you would have to in case of static simulation (modal analysis can be performed even without any boundary conditions at all). For shafts just apply proper restraints in place pf bearings.

Thank you! I will try to understand with the help of this equation now.

 

[Dr.D]

What JRMichler said in post #2 was a bit too narrow. Modal Analysis can also refer to the classical modal response calculation which seems to come closest to what the OP had in mind.

For an undamped MDOF system, the eigen problem comes down to
[K-omega^2*M]{phi}={0}
where
omega is the natural frequency
{phi} is the mode vector

If the full set of mode vectors is available, they can be used as columns in the modal matrix, [Phi]=[{phi1}|{phi2}|...|{phi_n}]

The modal matrix is the basis for the modal transformation of the equations of motion, resulting in two diagonal matrices for the coefficients in the equations of motion,
[MM]=[Phi]^t[M][Phi] = Modal Mass matrix
[KK]=[Phi]^t[K][Phi] = Modal Stiffness matrix
Because they are diagonal, the equations of motion are separated and can be solved one by one.

If we return to the original problem with forcing, written in matrix form,
[M]{xdd}+[K]{x}={F(t)}
where xdd is x double dot
Applying the modal transformation gives
[MM]{ydd}+[KK]{y}=[Phi]^t{F(t)}
where {y(t)} = modal response vector
That addresses where the forcing functions go right there.

The ICs can be transformed through the modal transformation in the same way. After the response is calculated in the modal coordinate space, it must then be transformed back to the physical coordinates to get the final solution.

 

[jack action]

he told me that there is no force input or excitation input given to a modal analysis.

I don't totally agree with that. In modal analysis you assume a harmonic motion. This sets a constraint on the possible answers:

To represent the free-vibration solutions of the structure harmonic motion is assumed, so that ${[{\ddot {U}}]}$ is taken to equal ${\lambda [ U]}$, [...]

For more info:

• Simple harmonic motion
• Complex harmonic motion

 

[Dr.D]

@jack action

In modal analysis you assume a harmonic motion. This sets a constraint on the possible answers:

The free vibration (unforced) is assumed to be harmonic because that is the correct solution of the homogeneous differential equations of motion. This is only the beginning, and it does not constrain the motion with forcing. The forced response calculation is as I indicated in #6, and {F(t)} can be any time function.