What is a Modal Analysis? What answers do we get out of it? How is it useful? What does it not tell us?
In this article, we’ll discuss where a modal analysis comes from, what it is and to some extent what it is not. We’ll also discuss why we do it, what we get out of it and how to use it.
Download a PDF version of this article
To answer these questions, we need to dig a bit into the mathematics of dynamic systems first – hopefully not too much for your taste.
Unfortunately the article is already overly long, so the examples are kept to only those required to illustrate a concept. If time permits, a future blog will discuss practical examples and uses of modal analysis.
The RealEigenvalue Problem
In this section, we’ll derive the equation used to solve for mode shapes and frequencies. In the process, we’ll also try to describe why it happens (in mathematical terms). This isn’t too important – feel free to skip to the following sections as we’ll discuss the results of this in more intuitive terms later.
The discrete dynamic equation used in FEA is the following:
Where is the mass matrix, is the damping matrix and the stiffness matrix. All three matrices are constant in linear dynamics.
, and are respectively the acceleration vector, velocity vector and the displacement vector. is the loadvector. All three vectors vary as a function of time.
If we neglect damping for the moment, the equation becomes:
We can neglect damping for a large class of problems because the amount of damping for most structures is well below 10%, which means slow damping of vibrations in the system.
Let’s say we have resultsvectors and which is a solution to the dynamic equation such that:
Let’s say we also have a second set of vectors and which is a valid result of the dynamics equation in which the load vector is set to zero:
Then, summing the two equations yields:
This can be rewritten as:
In other words, () and () is also a valid solution of the undamped dynamic equation. As long as and are both zero, there is obviously no problem. This is called the trivial solution.
On the other hand, if there is a nonzero set of vectors and , then there are multiple possible solutions to the dynamic equation. Spoiler: As it turns out, there are multiple solutions to the dynamics equation. Only one of the solutions is valid, though – the initial conditions determine which one.
Solutions to the equation
Have the form
Where is a constant vector, and represents the timeresponse which is simply a sine wave. is the radial frequency of the sine wave. is obtained by differentiating twice.
Using this, we obtain:
Dividing by results in the eigenvalue equation:
In which is the eigenvalue and the eigenvector. Discussing ways to solve this equation is unimportant in the context of this article.
The solution to this equation is the vector with a corresponding frequency . These are very important and will be discussed extensively in this article.
The implications of the RealEigenvalue Problem
Stepping back a moment: We are trying to obtain nontrivial solutions (i.e. is not a zero vector) to the previous equation. If the matrix is positive definite (also called nonsingular or invertible), then the only solution for is the trivial solution.
The only way to obtain a nontrivial solution is to pick a value of which will make singular. Once we find such a value for , the next step is to find a corresponding vector that matches . Notice that we say “a” vector instead of “the” vector. If we scale by any real number, the scaled is still a solution to the eigenvalue problem.
For this reason, it is more convenient to think of as a “shape”. It is also why it is called a “mode shape”. It is the shape that the structure oscillates within at frequency . Said in less technical terms: If we deform the structure statically into the modeshape, then set it free, it will oscillate between the initial deformed shape and the negative of the initial deformed shape at a frequency . True  Over time it will dampen out, but for low amounts of damping it will slowly decay in amplitude.
Another important point to remember is that there are multiple modes for a structure. Each mode shape occurs at a very specific frequency called the natural frequency of the mode in question. It is entirely possible for a structure to have multiple modes at the same frequency. An example is a beam with a symmetrical crosssection, clamped at one end: The first two bending mode shapes will be at the same frequency. However, the modeshape will be in different planes.
Note also that, because our system is linear, the superposition principal holds: Each mode’s behavior can be solved separately. The total displacement due to all modes being present will be the sum of the results due to each mode. Each mode shape oscillates at the natural frequency of that mode. In other words, multiple modes, each at their own natural frequency will be present in the results.
Lastly, since the eigenvalue problem only has real values in all the matrices and constants, the displacement vector of the mode shape is also real. A real mode shape implies that the motion of all locations in the Finite Element model is either perfectly in phase (0° relative phase) or perfectly out of phase (180° relative phase).
What a mode is
A mode is a combination of a deformed shape in which the structure will exchange kineticenergy and stainenergy continuously, and the natural frequency at which the mode shape occurs. If only one mode is present:
 In the undeformed state, the velocity at every point will be at its maximum. At this time, the kinetic energy is at its peak and the strain energy is zero
 At the maximum deformed state, the instantaneous velocity is zero. The kinetic energy at this point is zero while the strain energy is at a maximum
Said another way: If we deform a structure into any of its mode shapes and release it, it will oscillate continuously from the initial shape to the negative of the initial shape and back again, and at the natural frequency of the mode in question.
Remember that (without damping) we need zero external load to keep the oscillation going at constant amplitude. Therefore, a load applied at the natural frequency of the mode would cause additional motion for the mode, increasing the level of the oscillation. All the energy available from the load is absorbed into the structure. If there is no damping, the oscillation will grow to infinity, or rather until failure. With damping, the oscillation will grow to the point where the damping will remove exactly the same amount of energy from the system as the amount of energy being added by the excitation load. This can (and often does) lead to failure due to the relatively large oscillations that can result from a relatively small excitation force.
If the structure is deformed into a linear combination of mode shapes and released, each mode will be present in the resulting deformation over time. Furthermore, each mode will still oscillate at its own natural frequency. Below is an example of two mode shapes animated over time, as well as the combination of the two.
In summary:
 A mode is a shape with a corresponding natural frequency at which the structure will absorb all the available energy supplied by an excitation
 A mode is a property of a structure since it is calculated without any load applied to the structure
What a mode is not:
As mentioned before, a mode has a shape, not a displacement. By this we mean that the magnitude of the mode shape is arbitrary. The aforementioned is however not the whole truth  There are a number of standard ways to scale the modes. Even so, this is still a scale factor chosen for mathematical reasons, not to try and represent anything real for the model. So from this perspective, the scale factor for each mode is still arbitrary.
There is a problem with a mode shape: A shape looks like a displacement. After all, both a displacement vector and a shape vector imply deformation of the structure. This means that it is entirely possible for the Finite Element solver to calculate all standard results for the mode shape. In other words, we can ask for stress or strain for each mode. These should be referred to as stress or strain shapes as they correspond to the mode shape.
These values are useless though. Wait. What?!? Yes, the values are nearly useless. Granted, the distribution is useful even if the values are useless. To see why: A mode is a shape, not a deformation. If you want, think of it as a displacement with a random scalefactor applied. The stress reported for each mode would be the stress you would obtain if the displacement of the structure is exactly the same as that of the displacement shape.
Think of it this way: If the maximum reported stress was 9 MPa, what is the stress state of the model? We don’t know yet – we have not applied any loads yet so why would we know what the stress in the structure is? The stress level would reach this value if (and only if) we deform the structure to the exact deformation level that the modeshape has calculated, but the scale factor for the mode has been arbitrary.
As mentioned, the stress distribution is correct, even if the exact values are meaningless. We only need one measurement point to find the behavior of the complete structure if it oscillates at one frequency only.
Let’s use an example to illustrate the point. In figure 6, we have the stress plot of the first mode of a structure. Notice that the peak stress is 25 GPa. The matching deformation is 716mm. Note the excessive deformation due to the arbitrary scale factor applied by the solver.
If the real structure is oscillating at this first mode and we measure the peak deflection to be 1mm (instead of 716), we should scale both the deformation and stress by 1/716. This results in a maximum stress of 34.9 MPa and the stress distribution (and displacement distribution) as shown in figure 7.
In summary:
 A mode is not a displacement at a certain natural frequency  rather it is a shape
 A mode is not the structural response due to an input loading since it is calculated without any load
 The results of a modal analysis, such as displacement, stress, strain and velocity, are not representative of the stress in the structure under dynamic loading: This is because the relative values between any two (or more) points in the structure have meaning, not the numerical values of any of the results.
What is modal analysis used for?
Finally time to get practical. The purpose of a modal analysis is to find the shapes and frequencies at which the structure will amplify the effect of a load. In this section we’ll list some examples of why we may need this information and how to use the answers.
Finding loose components
In static analysis, the structure has to be constrained in such a way that any load in any direction can be countered by a reaction force or moment. If the structure is underconstrained, a static analysis will report an error. The reasons for being underconstrained can be anything from a missing constraint to having a part that isn’t attached to the rest of the structure.
Finding these problems is easy with a modal analysis: The analysis will report a 0 Hz (i.e. static) mode for each unconstrained direction. They will not be exactly 0 Hz for two reasons: Numerical roundoff during the solution process can cause a very low stiffness to ground, and also because the Eigensolution is an iterative process. The frequencies will be very low though – usually significantly less than 0.001 Hz. These zeroHertz modes are often referred to as “rigidbodymodes” or “strainless modes”. This is because the structure (or a part of the structure) translates or rotates in such a way that no stress results. In other words, it moves in some direction as if it was rigid.
The displacement shape for these modes should provide enough information about which component(s) may be loose or which constraints are missing.
If a single component has no constraints, then the model will have six rigid body modes. They correspond to the component translating respectively in X, Y and Z and Rotating about X, Y and Z. Notice that the modes is unlikely to be aligned with the global coordinate system as a linear combination of rigid body modes is also valid as a rigid body mode.
Deciding which rotational speeds are dangerous
If we have a structure that is rotating, any unbalanced mass will cause a sinusoidal load. If this coincides with a natural frequency, excessive motion will result.
To be honest, an extension to the dynamics equations are required if we want to look at rotating shafts as this starts to form part of rotordynamics. In rotordynamics, the natural frequencies are a function of the speed it is spinning at.
On the other hand, if we want to look at blades attached to the shaft or the load transferred to the casing at speeds well below the first rotordynamic shaft mode, then we need to perform a modal analysis on the blade or casing to find the rotor speeds that match natural frequencies of these.
We are sometimes forced to operate a shaft at a speed above the first (or even later) mode of a structure. If we slowly spin up the shaft, this mode (or modes) will be excited significantly. By slowly accelerating to a point somewhat before a mode, then accelerating quickly to a speed higher than the mode, that mode will not have time to reach steady state. This will drastically reduce the vibration level.
Finding out where to constrain or load a structure
Since real structures have damping, exciting them at their natural frequency will reach a steady state. Hopefully this steady state value is well before failure.
If we apply a known force at a natural frequency, the location where we apply it will determine the maximum displacement of the mode. If we apply it to the point of maximum motion in the direction of the applied load, the amount of energy we can add in a cycle is significantly more than if we apply it to a point with less motion. This will result in higher amplitude of motion for the same excitation level.
If we can apply it to a point on the model which has zero movement for a given mode, no energy will be added even if we excite at exactly the mode. Such points are called the “nodes” of a mode.
While sounding great, the nodes will in reality be at different locations for different modes. Finding a location where the displacement is relatively small for all modes is then a better choice than a node for a specific mode.
Finding out how to move a mode
If we have a mode at an inconvenient frequency, we may want to move the mode (or rather the frequency of the mode). The frequency can be increased or decreased based on the requirements of the structure.
For a single degree of freedom springmass, the natural frequency is equal to with the spring stiffness and the mass. Increasing the natural frequency requires an increase to or a decrease to .
Real systems do not have such a simple equation, but the same principal holds. Increasing the stiffness of the modeshape or decreasing the mass of the mode shape will increase the natural frequency of the mode. Bear in mind that adding stiffness also means adding mass. Therefore we need a way to increase stiffness faster than increasing mass, or reducing mass faster than reducing stiffness.
There are some tools to help us find the location where we should increase stiffness or decrease mass:
 The location(s) with the highest strain energy density is the locations that have the most impact on the stiffness of that mode. By adding stiffness in these locations in the direction in which the strain is greatest will add the most stiffness with the least amount of mass.
 The locations with the maximum kinetic energy density are those where changing the mass will have the greatest effect.
For a number of mode shapes, the location of maximum strain energy density and maximum kinetic energy density differ. For these, adding stiffness or reducing mass is relatively simple.
In the cases where they coincide, we need to add stiffness significantly faster than mass. An example of how this may be achieved is as follows: For a firstorder bending mode of a flat plate (see figure 8 below), doubling the plate thickness will double the mass, but increase the crosssectional inertia (and by implication the bending stiffness) to the 3^{rd} power. Another approach would be to add a diagonal rib to the plate as it would add less weight to the plate while adding even more bending stiffness than simply increasing the thickness would.
Note also that by comparing the different modes, it is often possible to selectively change the frequencies of modes by adding material to locations that will significantly stiffen up only specific mode shapes.
Modal dynamics (classical dynamics)
Modal methods are a way to drastically decrease the number of degrees of freedom solved in linear dynamics. Discussing the intricacies of modal dynamics is well outside the scope of this article. In short, it transforms the full dynamics system into a system that only allows motion that is a linear combination of the mode shapes used in the simplification. Instead of solving for every degree of freedom as a function of time, modal methods solve for a scale factor of each mode as a function of time.
In other words, we’re solving an approximate model. As approximations go, this is most likely the most efficient approximation in terms of accuracy vs. solution time for large models.
Conclusion
Virtually all analysis types solves for some form of response due to some type of load. A modal analysis is rather unique in this regard for at least the following reasons:
 A modal analysis solves an equation for which there is no applied load
 A modal analysis gives us specific information on the characteristics of the structure instead of reporting a response
What a modal analysis tells us is at which frequency the structure will absorb all the energy applied to it, and what the shape looks like which corresponds to this frequency.
While this seems to tell us very little, there are a range of uses for a modal analysis varying from finding mistakes in models up to providing information on how to change a structure in order to move a mode.
Finding out exactly how the structure will respond requires some other type of analysis though – A topic for another time.
Download a PDF version of this article
Resources
A modal analysis can be conducted using any of the software products from MSC Software:
And you can download a free student version here now.
For a list of other products we support, visit our Products page.
This is a very good article giving simultaneously the mathematical treatment & the intuitive concept of Modal Analysis simultaneously. Especially I found WHAT MODE IS NOT more helpful for conceptual understanding. THANKS. Do u have any such article specifically for Civil Engineering Structures.Can u please help out in conceptual understanding of MODAL MASS PARTICIPATION & MODE COMBINATIONS?. THANKS AGAIN. AMODH LUMAN
Thank you for the kind response.
I hope to be able to write followon articles soon. There are at least one on the way on the practical use of modes. Another on more indepth mathematics for modal analysis  As an example, for Civil Engineering, I'll have to add at least a section on Response Spectra methods. Another topic on the way is a series on Structural Dynamics  linear, nonlinear and modaldynamic.
I'd appreciate comments on specific topics anyone would like to be covered in such articles. For example, is anyone interested in "added mass" methods for submersed structures, or simultaneous solution of fluidstructural modes in FEA?
Hi,
i found your article pretty interesting. I would like to ask you the following:
Do I need absolutely the force part in order to find out the Modes and the corresponding Eigenvalues ? In my opinion the Eigenvalue problem is a harmonic problem without a force? right?
Thank you!
Mohammad
Hi Mohammad,
"Do I need absolutely the force part in order to find out the Modes and the corresponding Eigenvalues ?"
Rather the opposite: A modal analysis ignores any force applied.
"In my opinion the Eigenvalue problem is a harmonic problem without a force"
Yes. A modal analysis solves with a zero load. A mode is a characteristic of the system rather than a response due to some inputload.
The moment you want to include a load in a calculation, you need to run a "response" type analysis. By this I mean an analysis that reports an output due to some input. Examples include transient analysis where you solve the response as a function of time. Or frequencyresponse where you calculate the steadystate response as a function of frequency.
Best regards,
Gerrit
Thank you very much for the article. Very well explained the concepts. Could you also tell us a bit about the Postprocessing of the results maybe.
Very good and clear explanation.
A very good article, thank you for this effort :). In case you have time, elaboration on using modal kinetic energy for determining optimal sensor (e.g. accelerometers) locations would be quite handy..
Can we apply modal analysis to ball bearings to know a failure.?????? And...where to fix the bearing..... If possible
You can analyse a small subset of bearing failure at best. If the shaft is standing still, performing a modalanalysis and comparing the results with a measurement using a modalhammer may work.
Most bearing problems are diagnosed using measurement techniques instead of analyses. In these methods, you look at harmonics of the shaft speed as well as ballbearing speeds and their harmonics. A harmonic is a response due to an input load, and doesn't have anything to do with the frequencies of the modes – the harmonics occur at multiples of the shaft speed, not multiples of naturalfrequencies.
A modal analysis gives a system characteristic, not a response to some input load. The measurement is a response due to an input load and will have most of its content at frequencies away from modes.
Furthermore, the harmonics measured are due to nonlinear behaviour of the bearing, while modal analysis only looks at linear behaviour only.
In short, performing modal analysis is not a good fit for predicting bearing problems.
Hello Gerrit, Very nice article on Modal analysis. Is there any way to link failure mode of a rotating shaft/system (rotor of a motor) due to its vibration level and natural frequency/mode shape. Just imagine that the rotor has various loading patterns (say electro magnetic forces, un balanced forces, eccentricity etc) and when it runs for a long period, due to structural degradation (may be due to fatigue, fracture etc) and just would like to know is there any way I can correlate with mode shape info of the rotor? I understand that by looking at the mode shape one should avoid reaching the operating frequency near to that. I wonder if the operating frequency is not matching with natural frequency but close to it then is there any prediction of failure mode possible?
Hi Nair. Yes it is possible. This is done by modelling various levels of damage to the structure to see how it impacts the natural frequencies and modeshapes. For some structures, the natural frequencies can change by a very small fraction when comparing the "perfect" structure and nearfailure components. This result in nontrivial measurement to detect damage based on the natural frequency. The modeshapes for these structures sometimes changes by a greater amount. In these cases, measuring shapechange may be a better indicator of damage than frequency change.
There are complications though (aren't there always?). One complication is that you may be forced to do measure inuse vibration levels. If the vibration level changes due to any reason (imbalance, magnetic changes etc.), the vibration measured will change. Furthermore, predicting the amount of vibration due to each source is often difficult. Therefore, a method is needed that is not too dependent on input load magnitude.
Other complications include rotordynamics and bearings: The rotordynamic terms in the equation of motion are the cause of the natural frequency and modeshape change of a shaft as a function of its spinning speed. Bearings have their own vibrationlevels and vibration changes that can be measured to detect bearing damage. If not careful, these vibrations levels and frequencies can look like part failure.
I found ur article is very important and i learnt from u thank u for this article.
I make a modal analysis on a radial turbine blade and i want to know how can i show the banding mode shape in FEA because the six mode i have is torsion.
thank u in advance.
Hi Amr. I need more info to give a good answer, so I'll try and provide some basic pointers that may help:
Are you including stressstiffening due to spinning the blade? Depending on how fast you're spinning, the bending mode may be significantly higher than the torsion modes. Even so, 6 torsion modes for a single blade before any bending modes would be extreme  check the radial load is correct.
If it's for rotor with multiple blades, 6 torsion modes are only the start of the torsion modes. In this case you'll have large numbers of modes at nearly the same frequency and looking nearly the same (one per blade).
What kind of elements are you using? Shells or solids? For solid elements: If you're using Tetrahedral (Tet) or Pentahedral (Penta) elements, please ensure that you're using second order (or higher) elements. First order Tet elements are extremely stiff in bending  you need a very fine mesh through the thickness before they start giving soso answers. To put it into perspective: I expect that one element through the thickness of a firstorder Hexahedral (Hex) element or a secondorder Tetelement to be more accurate than a firstorder Tetmesh with three elements through the thickness! Penta elements are mixed: In some directions they're as good as a Hex, in others as bad as a Tet, so "always" use secondorder Penta and Tetelements.
Please check your constraints to ensure you're not applying any constraint to the bladepart of the model (only the root or the shaft if that's modelled)
If the model is a single blade, correctly constrained and meshed fine enough for the element type you're using, then increasing the number of modes requested should yield the bending mode pretty early on.
If it is a fullmodel, then you'd need to request at least one more mode than the number of blades (assuming the second mode for each blade is bending). Otherwise, even more would be required. This is a very expensive way to model as it would require a large number of elements and a large number of modes.
Thank u very match i have edited my constraints and increasin the number of modes and i found the bending mode shape. I am thankful for ur help.
What a great article. You nailed them mode shapes. You effectively answered all the questions i had on mode shapes. I am doing a simulation of deformation in a motor/generator support frames and thought it would be wise to understand mode shapes first. Thank you neighbor. From Namibia, thank you.
Good Read..
Really it is nice to understand ....
very much helpful to understand basic
This is very well written. And great illustrations, too. Thank you.
Great Job! Modes was a misery to me, but now i have good knowledge of it. Thanks alot!
Hi there. Thanks alot for this superb article. I had alot of queries regarding modal analysis and the interpretation of the results. This article has helped me alot in this regard.
Very well explained! Great work. Congratulations.
Dear Mr. Visser
I'm a begineer using Ansys.
And now, i trying to perform a modal analysis of prestressed concrete beam with ansys R15.0 APDL. I read section "modal analysis guide" on "Structural analysis guide" file. And i understand is there are three situations:
1. To perform a basic analysis (static structural analysis) that must be a linear analysis. So, i understand that i must model a structure and then, i will create a force and apply it in model (certainly, value of the force is equal to prestressed force). and then, i obtain a result that have prestrain on a result file. and i perform modal analysis on it (i mean is result file).
2. I read some papers that discribled how to model a reinfored concrete beam. And have known they used two elements to model: solid65 for concrete, link8 or link10 for steel reinforcement. So, is this a nonlinear problem because of contact between solid5 and link8 (link10)? If so, we must perform a "linear pertubation analysis" (via modal analysis guide)
And the end, that is situation that has a large  deflection.
In situation 2, I have some problems such as:
+ Does material for concrete (solid65) must be a non  linear (via some papers) ?
+ When i use solid5 for concrete, link180 for prestressed steel using option initial state, do i only perform a modal analysis without basic analysis that be replaced by using force step option. (my first force step is doing prestressing in model).
Best Regard.
Thank you so much.
thanks a lot, very clear information
Very fine Article. Thanks a lot.
Thank you, very useful.
OK. Very good.
"Scale Factor " is that called "tọa độ dạng dao động" in Vietnamese.
So how can we solve "function scale factor of time". Can i use Newmark, Wilson or HHT Methods to solve it?
Not in a modal analysis directly.
However, what you suggest is exactly what a modaltransient analysis does: It transforms the dynamics equation from the physical (Movement in X, Y and Z per node) domain to the modal domain (deformation being limited to the sum of modeshapes, each scaled by some factor which we solve for). It then solves (timeintegrates) the transientdynamics equation on the modal system using any of the same methods used in directtransient calculations (Newmark beta, Generalized alpha, HHT etc.).
This is a much smaller system to timeintegrate. The number of Degrees of Freedom (DOF) to solve is equal to the number of modes solved, instead of the total number of DOF in the model. It is therefore orders of magnitude faster to timeintegrate in the modal domain. Finally, the scale factors just solved for can be written out directly, or alternatively backsubstituted into the transformation equation to get nodal displacement results (and stresses etc.)
You can also extract the relevant data and do the timeintegration using your favorite method in other software (Octave, Matlab, Scilab, Python NumPy, etc.)
On a side note, it is also possible to measure them on a physical structure: Measure the response on a real structure due to (possibly unknown) load input at enough locations so that you can find the contribution from each mode at each of these locations. Then solve for the modal contribution (i.e. the "mode scale factor") from each mode at every point in time. There's more involved to accurately do this. To name some complications: You need more locations measured than modes for validation and error estimation. Additionally the FEA model needs to really accurately represent the sample that was tested. But it is done in real life.
Thank you so much.
When i use mode superposition method to solve a problem that is a moving load transports above a simple supported beam (for example).
u(t) = PHI*neta(t) (1)
When:
u(t) is response that we need find
PHI is mode shapes matrix
So, Is neta(t) function scale factor of time as you defined above?
And, Do i have to solve two problem?:
First problem: Modal analysis (or solve a eigen problem) to find mode shapes matrix and frequencies. (equation 1)
Second problem: solve function scale factor of time problem to find scale factors for each corresponding to mode shape.
And, then, responses (deformation, stress, and so on..) that i'm finding are sum of responses according to mode shape.
etc:
u(t) = neta1(t)*phi1+neta2(t)*phi2+....neta(m)*phi m
Of cause m is much smaller than N (N la degree of free of Structure) because influence of high frequency modes into response is much smaller than low frequency modes
Here, i use matlab to solve.
So, I mean when i use Newmark, Wilson or HHT methods to find function scale factor of time (that is neta(t)) for each corresponding to mode shape. Is this right or wrong when i use mode superposition method?
That is my meaning.
Yes, that sounds right. There are some intermediate steps and refinements you didn't mention, so I'll go throught the whole process below. It is easiest to explain in matrix equation terms, especially if you plan to use Matlab for the timeintegration.
I plan to write a blog post about this topic at some point. Below are the short version. Apologies in advance for not using typeset equations.
Step 1: Modal analysis
Solve the modes of the equation
[M]{U''(t)} + [K]{U(t)} = {F(t}
where [] indicate a matrix and {} a vector. ' being first derivative and '' the second derivative.
Since the scale of the modes reported is arbitrary, we can pick any initial scale factor. A really convenient mode shape is one where we scale each mode so that the following equation holds:
transpose{phi} * [M] * {phi} = 1
(In Nastran, Massscaling is one of the default options. Other software may have this option too)
Step 2: Set up modeshape matrices
We then assemble these into the matrix containing all the modes we've solved for
[PHI] = [{phi_1} {phi_2} ... {phi_m}]
where {phi_i} is the i'th mode shape. Note that [PHI] is an n x m sized matrix, where "n" is the number of DOF in your original model and "m" is the number of modes we use
Step 3: Convert from the spatialdomain to the modal domain
{U(t)} = {phi_1}*q_1(t) + {phi_2}*q_2(t) + ... + {phi_m}*q_m(t)
with q_i(t) being the scale factor for mode i [same as your "neta(t)"]
Written in Matrix terms, this becomes
{U}(t) = [PHI]*{q(t)}
with {q(t)} the vector of scalefactors at time t. (The scale factors are sometimes called modal displacements of the modal coordinates)
Since [PHI] is not time dependent, it the time derivative of [PHI]*{q(t)} is simply [PHI]*{q'(t)}, and [PHI]*{q''(t)} for the second derivative.
To solve the transient problem, we now replace {U(t)} in the following equation with [PHI]*{q(t)}
[M]{U''(t)} + [C]{U'(t)} + [K]{U(t)} = F(T)
becomes
[M][PHI]{q''(t)} + [C][PHI]{q'(t)} + [K]{q(t)} = {F(t)}
premultiply this with the transpose of [PHI], [PHI_t] for short:
[PHI_t][M][PHI]{q''(t)} + [PHI_t][C][PHI]{q'(t)} + [PHI_t][K][PHI]{q(t)} = [PHI_t]{F(t)}
Since [PHI], [M], [C] and [K] are fixed, we can solve the matrixmultiply parts before solving the full equation. Define the following:
Modal mass matrix: [Mm] = [PHI_t][M][PHI]
Modal damping matrix: [Cm] = [PHI_t][C][PHI]
Modal stiffness matrix: [Km] = [PHI_t][M][PHI]
then substitute into the above:
[Mm]{q''(t)} + [Cm]{q'(t)} + [Km]{q(t)} = [PHI_t]{F(t)}
** We can solve {Fm(t)} = [PHI_t]{F(t)} before hand, but it may end up being too much data. It can be solved over time as needed. Whichever is easiest
This equation is exactly the same as our initial transient equation, but the matrix sizes and meanings differ:
[Mm], [Cm] and [Km] are of size m x m. q(t) is the modal displacements (vector of mode scale factors)
Interesting notes on the last equation:
A property of modes are that they are massorthogonal. Meaning:
transpose({phi_i}) [M] {phi} = 0 if i and j differ. It is "1" if it is the same mode because we have applied "mass scaling" before.
This means that [Mm] is the identity matrix (all offdiagonal terms is zero, all ondiagonal terms are "1")
K is also diagonal: The term on the diagonal at position i,i in the matrix is the square of the natural frequency (in radians per sec.) of the i'th mode.
This means we don't need to even calculate [PHI_t] [M] [PHI] or [Phi_t] [K] [PHI] since the first is the identity matrix and the second I only need the natural frequencies.
Damping is more complex. Without damping, since [Mm] and [Km] are diagonal, the equations are decoupled and each mode can be solved independently.
If we want "modal" damping (i.e. specifying the damping ration of each mode explicitly), we can specify the diagonal of the [Cm] matrix very easily to reach the required damping ration because the system is decoupled (it consists of "m" 1DOF equations)
If we use "proportional" damping ([C] = a*[K] + b*M], a and b being scalars defining the relationship between [C], [K] and [M]), then C is still diagonal and the system still decoupled. If [C] explicitly contained damper elements, we have to then find [Cm] from [PHI_t] [C] [PHI]
Step 4:
Timeintegrate
[Mm]{q''(t)} + [Cm]{q'(t)} + [Km]{q(t)} = [Phi_t] * {F(t)}
Step 5:
To find the displacements and stresses of the structure at time t, backsubstitute the modal displacement vector {q(t)} into
{U(t)} = [PHI]{q(t)}
and for any other component such as "stress in X direction":
{Component(t)} = [PHI_component]{q(t)}
where {Component(t)} is the result component we are interested in (e.g. "stress in x direction") and [PHI_component] is the matrix containing the components (e.g. stress in x direction") for each mode. Using the "stress in x direction" example with "Sx" the stress in the x direction:
{Sx(t)} = [{Sx_mode1} {Sx_mode2} ... {Sx_modem}] * {q(t)}
I hope the above is readable and without typographical errors..
Yes, you are right. Because as you know, there are many formulations in steps when use mode superposition method. And it isn't too convinient to write on here.
Yes, you are so enthusiastic.
And about theory of mode superposition method, you can find very easy when you search on Google, So i only write main content. So sorry.
And on the same occasions, could you answer a my question?
How many methods are used to determine frequencies and mode shapes (or eigenvalues and eigenvectors) in vibration? How do they catalog ?
When i search on Google, i found a book that is "Mechanical Vibration" 5th edition by Singiresu S. Rao. In it, i find some methods as:
1. Rayleigh's method
2. Holzer's method
3. Dunkerly's method
4. Standard matrix iteration method
But, as you know, in ansys, there are many methods such as:
BlockLanzcos, PCG LAnzcos, supernode, and so on...
So, what is that mean?
There may be more types today, but there used to be two main classes  those known as transformation methods and the tracking methods. Lanczos (in all it's forms) have been (and still is) an efficient method as it combines the best of the two types. It is my method of choice in Nastran and Marc. One of the best books on FEM is the one by Bathe (Finite Element Procedures)  it has some methods and implementations as well.
There are some extreme refinements to the existing methods such as breaking up the model into large numbers of smaller models, solving them, then assembling these again. This allows massively parallel modalextraction to be done (and done efficiently).
To be fair, I don't really care too much about how each method works internally (yes, I have coded some myself). What is important to me is in usage terms: Does the method work reliably and is it efficient? Some of the other methods are only efficient if you try to extract all (or most) modes of a model. For a 100 DOF model it is no problem to extract all modes, but for most realworld models we extract a very small fraction of the modes in a system. Lanczos is good with these. As to blockLanczos, PCG Lanczos etc.  you will have to read the Ansys documentation to see what they do differently and (hopefully) what their strong and weak points are. If not, test them.
Yes, I read guide of Ansys on Modal analysis when i tried to perform a modal analysis of a prestressed concrete beam. But, In there, it only provide for us information without detail. They only tell us scope, capacity of these methods.
Again, Thank you so much, Mr Visser.
Still; what is the contributing mass in each mode , in mechanic ?
I'm not sure what the question is here. Do you want to know how to calculate it or what the meaning of the contributing mass is?
Hello ,
I am confused at these two serperate statements "A mode is a shape with a corresponding natural frequency at which the structure will absorb all the available energy supplied by an excitation
A mode is a property of a structure since it is calculated without any load applied to the structure" .
How can a component vibrate without an external load applied to it? By external load it is force, how can the structure undergo any changes without force? If the structure absorbs available energy, should it come from a force?

Actually the two statements complement each other: The purpose of the modal analysis is to determine the frequencies at which energy will be absorbed when you apply a load (force or moment) or enforced motion to it. It does not determine what the response of the structure will be due to the excitation though.
It may be easier to understand if we look at how to measure the frequencies (and shapes) of modes. We add a number of strain gauges, accelerometers or any other sensors that can measure displacement directly or indirectly. Before any load is applied, there will be no response. Then we excite it with a wideband signal long enough to ensure that all the modes are excited nicely. Then we take away the excitation and start measuring. In other words, while the measurement takes place, there is no excitation although the structure is vibrating.
At this point, the ONLY frequencies in the measurement will be at the natural frequencies, even though we had excited all frequencies initially. The measurements relative to each other is used to determine the mode shape associated to teach frequency.
If the initial excitation duration or magnitude is changed, the same discrete frequencies will appear and the shapes will be the same even if the magnitude of the vibration differs.
Hello. Gerrit Visser.
Do you understand on mode superposition method in "frequency domain"? Could you explain to me about theory of it? Or, where can i find theory of it ?
Thank you so much.
Are you talking about frequency response? If so, there is nothing special to the process: Do the transformation to the modalspace as you would for a modaltransient analysis, then perform the frequency response calculation exactly as you would on the full system.
Yes, i found that i need. thank you so much.
So much information, presented in simple way. Thank you so much. Please provide links to find other related articles by you.
Very good explanation and comments added by Mr Visser were really useful.
Very wellwritten article!
Hi Mr. Visser,
I'm very interested in this blog. Unfortunately, the figures here are not properly displayed. I can only view the text.
Can you send me a PDF copy, or something equivalent, of this article? Or is it possible to fix the figure problem of this post?
Thank you in advance.
Best regards,
Ding
Hi Ding
Thank you for letting us know.
We have emailed you a pdf version of the article.
I hope it works better that way.
Thank you so much for your quick reply!!! I have received the email.
It seems a glitch of my network. Everything works perfectly right now.... : )
Thank you again!
Excellent article!
I found it while searching for qfactor calculation methods alternative to the classical "3dB", which yields some difficulties in case of coupled modes or 'very close' modes.
Would you happen to have any suggestions or pointers to this subject?
Is it possible to print a pdf/printerfriendly version off this article?
Thanks.
Regards.
Gilberto
Hi Gilberto,
Thanks for the feedback.
The article is about Real Eigenvalues of undamped modes of the basic equation of motion as used in FEA. In this case, the modes are per definition uncoupled and have zero damping (q=infinite).
If damping is included or any nonlinear behavior exists, the modes can couple (to name some sources). This is however totally outside the scope of this article and would unfortunately need a complete blogarticle on it's own.
Regarding your question "Would you happen to have any suggestions or pointers to this subject?": Are you looking for analysis techniques or measurement techniques for coupled modes?
We'll send a pdf version to you.
Best regards,
Gerrit
Hello Gerrit,
Thank you for your reply and the pdf.
I am looking for measurement techniques.
I need to measure qfactor from an FRF bode plot. Sometimes there are coupled modes where the peak amplitude @3dB is actually a compound of both modes. In those cases, the resulting qfactor is biased at best, when not at all wrong.
To solve such cases, I imagined interpolating both peaks to 'guess' their shape if they were not coupled. Unfortunately, more often than not they are so close that I only have a limited number of points in the plot in between peaks to use for interpolation, which again does not help in calculating a 'good' qfactor.
I hope you can give me a suggestion.
Regards.
Gilberto
Do you mean that we can perform modal analysis without applying external load in our models in Ansys?
thank you very much
Eamon
Hi Eamon,
Yes, definitely. Constraints will be used. Loads will not be used  At least not directly: In a preloaded modal the loads can be used to update the tangent stiffness matrix before the modal part of the analysis takes place.
[If the loads are not used in a preload calculation but the modes change due to an applied load, then the modes that have changed are not modes  they're "static correction shapes" for use in subsequent modaltransient or modalfrequency response analysis. Nastran calls these additional modes "residual vectors", but they are not modes of the system.]
Best regards,
Gerrit
Hello Gerrit, Great article! Would like to print it out, would you mind sending me a PDF version of this article? Thank you!
Best regards,
Tom
Hello Gerrit,
I am a mechanical engineer. I am studing on vibration shaker for master. I produced a vibration shaker for modal analysis. If it is possible, could you send me your article PDF? And, can I get some advice about this topic from you.
Best regards,
Yunus Emre
Hi Yunus,
Apologies for the late response. There's now a link at the top to download a PDF.
What advice were you looking for?
Best regards,
Gerrit
Hello Gerrit.
Really a brilliant piece of work.
Just had a small doubt .
The frequencies that you obtain by solving the equation kmw^2=0 correspond to the frequency per each degree of freedom or each node or any other parameter .
And, what should be the order of the matrices [K] and [M] and how are they defined ?
Thanks
Hi Vivek,
Thank you.
I'm not sure of what the questions mean though. You're solving the eigenvalue problem which is the matrix equation
([K]  omega^2 *[M]) * {U} = {0}
with [ ] indicating a square matrix and { } a vector. The full [K] and [M] is used when solving this to fund omega. So each "omega" is the natural frequency for all DOF simultaneously (i.e. the {U} vector is for all DOF at the same time).
[M] and [K] are simply the mass and stiffness matrices respectively. Again, I'm unsure what you mean by the "order" of these or "how they are defined". They are defined by the FEA solver that sets up the system mass and stiffness matrix.
Best regards,
Gerrit
Hi Getrit,
Thanks for this article. Let me ask you a doubt. How can we excite an n th mode frequency and corresponding mode shape of a system?
Hi Joseph,
Exciting only one mode is (nearly) impossible. However, if you don't care about exciting other modes as well, then exciting a specific mode isn't difficult. Applying a load at any location that does not have zero motion in the direction of the applied load at the frequency of the mode will excite it. Applying an impulse load (e.g. hitting it with a hammer) instead of a sinewave will also excite it due to the wideband input.
The best locations to excite the mode will in general be at those locations that moves the most for the modeshape in question.
Be careful of measuring a mode shape while an excitation is applied: The shape will be the sum of the mode excited combined with the response due to the applied load.
Best regards,
Gerrit
Awesome article! I was looking for a brief overview on modal analysis..and this is perfect!
Dear Joseph.
I have a problem. Could you explain to me?
Now, i have been reading a book "modal testing: theory and practice" by Prof D.J.Ewin. And in this book, Prof D.J.Ewin wrote:" those (structures) with extremely light damping, for which measurements at resonance are inaccurate and difficult to obtain".
And, i understood that, when perform a modal testing for extremely light damping structures, results that obtained from measurements are inaccurate and of course is difficult to obtain these results.
Yes, Of course, may be i understood wrong meaning of this sentence. But, oppositely, if i understood right, so why is it difficult to obtain modal parameters when measure extremely light damping structures and those results is inaccurate?
Thank you so much.
Hi,
When the author talks about the "measurements at resonance", my guess is that he is referring to using a frequency response measurement to determine the modes (frequencies and shape) as well as the damping ratios. The intent of a frequencyresponse measures is to measure the steady state response due to an input load at the frequency of interest. Measuring steady state response for lowly damped modes is more difficult as explained below.
When exciting a structure at a natural frequency, the structure does not reach steadystate response instantaneously. The response amplitude increases with an exponential decay to the steady state value. The lower the damping of a mode, the longer it takes to reach steady state.
If you use the measured frequency response to determine the natural frequencies and mode shapes, it is very easy to get lowlydamped modes wrong in both frequency and measured damping ratio. This is especially true with a sinesweep input when the frequency is ramped too quickly: The response has not yet reached steady state by the time you're past the natural frequency. Past the natural frequency, the response is still increasing because it still hasn't reached steady state at this higher frequency. The natural frequency is therefore overpredicted and the shape of the peak (which determines damping ratio) is wrong.
If you are interested purely in the natural frequencies and modeshapes but not damping ratio measurement, it would probably be most accurate to only start measurement of the vibration after the input is stopped (i.e. after hitting with the hammer or switching off the shaker). This is because all frequencies present in the input is present in the output while an input exists. If no input is present when measuring, the only frequencies present should be those of the modes. A frequency response of this would most likely have very sharp peaks (the modes) and approach the noisefloor everywhere else.
Best regards,
Gerrit
Can you explain me what happens in a 3D modal analysis problem?
Hi,
I'm not sure what the question is as the whole article is for 3D analyses [although it would apply asis for 2D and 1D structures as well].
The process for (from the FEAsolver's perspective) modal analysis is to set up the stiffness matrix, set up the mass matrix, then solve the eigenvalue problem to find the eigenvalues (in turn used to find the natural frequencies) and the corresponding eigenvectors (the modeshapes)
From the FEA analysis perspective, you build the mesh. Then apply material properties (the material must have an elastic modulus and density at a minimum), and geometric properties (such as thickness for shell elements). Add constraints as needed. Set up the analysis to run modal and run the model.
Best regards,
Gerrit
When performing a rotor dynamic analysis (Modal analysis) using ANSYS Workbench on a shaft resting on anisotropic bearings, how can I add radial forces acting on the shaft? Does performing a prestressed modal analysis accurately represent this load case?
Hi,
Firstly, I don't know Ansys so I can't comment on the details of how to implement it. That said, to take it into account from the mathematical perspective, you would have to preload the structure so that you get the stressstiffened stiffness matrix, then use that in the rotordynamic calculation.
As you know, the difference between a modal/transient/frequency response and a rotordynamic modal/transient/frequency response is the inclusion of the gyroscopic terms. The modes you're interested are the shaft's the whirl modes. I don't think a radial force will impact these modes. An axial load may as it will stiffen the bending modes, in turn impacting the higher frequency (bendingtype) whirl modes.
If the radial force you are talking about is the centrifugal force on the blades of a turbine, the stress will stiffen the blades, thereby causing an increase in the frequencies of the modes. However, these are not rotordynamic modes and is usually calculated in a standard modal analysis to determine the blades' bending and torsion modes.
On the other hand, if it is a side load such as for a Vbelt, then it should not impact the rotordyamic modes. It will have an impact on the response of the spinning shaft, but a modal analysis is not about the response of the structure. A frequency response or transient response with the rotordynamic terms included will be requried to calculate this response.
Best regards,
Gerrit
Hello Sir,
This was a really helpful article. I don't know much of the mathematics behind the modal analysis, and rather than going into deep study of it I want to apply it directly on the structure and check whether it is safe or not using ANSYS Modal Analysis. How can I check that?
As of my knowledge, To perform Modal analysis, I am fixing some points that would be constrained by use of fasteners and finding different Natural frequencies for different modes. From the obtained values of frequencies, how can I check that my structure will be safe or not?
I know the frequency range of the load under which this structure will be loaded.
Hi,
Modal analysis does not tell you whether a structure is safe or not. It simply shows you some dynamic characteristics of the structure.
Since there are no loads in a modal analysis, the stresses doesn't tell you anything directly.
To find out whether the structure is "safe", you will have to run an analysis that includes the input loading (magnitude and frequency content). Depending on the load type, you have the choice of a frequencyresponse analysis, a frequency response analysis combined with a PSD of the input loading, a response spectra (also called shockspectra) or a fullon transient analysis.
In short, the purpose of a frequency response is to look at the behavior of the structure if a load is applied onefrequency at a time. The answer as the stressstate etc. and is reported per frequency. This is useful only if you apply the load one frequency at a time (for example a shaft spinning up and having an imbalance  at any point the excitation is at a single frequency).
A PSD is for those cases with random vibration and uses the frequency response together with the input PSD to calculate an RMS stress which is then used in a statistical calculation to determine if failure will occur.
A Response/Shock spectrum is to determine the worst stressstate due to a shortduration input such as an earthquake or elastic impact.
A transient analysis is the most expensive to solve as it performs a timeintegration of the equation of motion. The input load is specified as a function of time. This makes it the most general type of transient analysis. However, the longer the timestep, the longer the analysis takes to complete. Additionally, the higher the maximum frequency to capture, the smaller the timestep has to be. To get an idea of the amount of data generated, look at typical strain measurements: They can easily run for hours and have a sampling rate that can easily exceed 1kHz. An hour at 1kHz means there are 3.6 million timesteps to be solved for in a transient analysis!
Best regards,
Gerrit
Hello Gerrit, Few very fundamental questions I wanted to ask..
1. What exactly is the physics behind 'Natural Frequencies' of solid structures (Please don't start explaining, strings and harmonics)? I mean, why free vibrations happen only at these particular frequencies (Can it not vibrate at other frequencies)?
2. What is the physical significance of multiple modes, that too simultaneously?
3. What is the difference between FreeFree Modal Analysis (after excluding first 6 rigid body modes) and normal Constrained Modal Analysis?
Hi Puneet,
1. The physics of modal analysis is the same for all types of models (springs & mass, Beam, Shell, Solid etc.): It is the solution to the undamped equation of motion when the applied load is exactly zero. We're trying to find a shape and frequency combination that allows this equation to be true for all time values.
In other words, the whole article was written for all types of structures (including solids).There is no difference between solid structures, beam structures and simple springmass systems as far as modal analysis for finite element analysis is concerned: The equations are exactly the same. The solution method is exactly the same.
The only differences between solid models and others is that the stiffness matrix and mass matrix is set up for a solid mesh instead of a beam mesh or a springmass model. This has nothing to do with modal analysis as static analysis also needs a stiffness matrix and mass matrix, and the modal stiffness matrix and mass matrix is exactly the same as for a static analysis. You can read up on static analysis to answer your question.
For the second part of the question about free vibrations: Forced vibrations can cause vibration at any frequency because we can apply a load at any frequency. Free vibrations on the other hand can only occur at specific frequencies for a very simple reason. The undamped equation of motion for free vibration (no force applied) says [M]{u''(t)} + [K]{u(t)} = 0 and must be true for all time values. This is only possible if [M]{u''} = [K]{u}. In other words, acceleration "forces" perfectly balance "stiffness" forces. At frequencies that are not natural frequencies, there is no possible {u} that can satisfy this equation.
2. Multiple modes at the same frequency or multiple modes happening simultaneously?
Multiple modes at one frequency usually occurs for symmetric structures which will have the same "shape" but different directions.
Multiple modes simultaneously present in a structure is easy to explain as well: If you bend a structure into a linear combination of its first and second mode shape, both frequencies will be present and you will be able to extract the motion due to mode 1 and mode 2 at any point in time. After subtracting the deformed shape due to the two modes, no additional deformation will be left, so no other "modes" or "deformed shapes" will be excited. However, two mode shapes present in a structure has nothing to do with a modal analysis as we are only trying to find the mode shapes and frequencies. We are not attempting to find the vibration over time. Modes are extracted separately and independently.
3. The modes for a constrained structure will be different to the modes of the same structure which is unconstrained. This is true even if we're neglecting the first 6 rigidbode modes for the free structure  in other words, comparing the strainmodes (non rigid body modes). Both the shapes and the frequencies will differ because the stiffness matrix changes: Constraints adds infinite stiffness to ground which result in some rows & columns from the stiffness matrix and mass matrix to be removed. In other words, to find the modes of a real structure, you have to model the constraints placed on the real structure.
Please run a modal analysis (of a solid structure if you want) and look at the difference in the shape and frequencies. It should be readily apparent why the shapes differ. After looking at the change in shape, it should then be apparent why the frequencies differ too.
Best regards,
Gerrit
Very well explained Gerrit.
But in my 2nd part, I intended to ask something else. Simultaneous multiple modes, I meant at different frequencies. Let me frame it in other way. Structure is excited at two frequencies (corresponding to mode1 and 2) simultaneously. Now suppose, the location of Node for mode1 is same a location of antinode for mode2. Physically, how the system is going to superimpose these two and vibrate??
Hi Puneet,
It sounds like you're back to forced vibration again ("structure is excited") which has nothing to do with modal analysis. This is a transient analysis and is pretty time and diskconsuming.
From the analysis perspective:
If there is no excitation but both modes are present (i.e. we deformed the structure into a combination of the two modes then released it to oscillate), then you need to know how the magnitude and phase for each of the two modes. You can then manually scale the two modes with the relevant scale factors at the point in time you're interested in. The scale factor for the two modes are simply cos(omega_1 * t + phase_1) and cos(omega_2 * t + phase_2).
If there is excitation, and the excitation is only at the two natural frequencies, then you can't solve an undamped system: The response will increase linearly over time and reach infinity when excited at the modes. If you have damping, you can excite it at the modes and reach a limit magnitude (and phase) even when exciting at the natural frequencies. This magnitude and phase is calculated in a frequencyresponse analysis. This can again be used like the previous paragraph mentions to find the response at a point in time  instead of modeshape you use the displacement or stressresult of the frequency response calculation (which will be similar to a mode shape, but not exactly the same due to the influence of the excitation changing the shape slightly)
For a real structure (and a transient analysis):
If the excitation location is at the node for mode 1 and the antinode for mode 2, mode 1 will not be excited while mode 2 will be excited. The amplitude of mode 2 will grow over time and in theory reach infinity if there is no damping. With damping, we will again reach a steady state oscillation.
If the excitation is not at a node for either mode, then both modes will be excited. (The argument about damping will hold again). The amount of excitation for each mode depends on how well the load represents the mode. Again this can be found from a frequency response analysis.
If we extract the response at the two frequencies from the timesignal (measurement or transient analysis), the steady state response will match the results from a frequency response analysis at the two frequencies again.
In short, there is an interesting complication when we think of the timedomain of a system for which we have frequencydomain results: The two are not directly compatible. To convert from timedomain to frequency domain requires something like a Fourier transform. To convert from frequency to time, every frequency point "i" needs to be scaled by a cos(omega_i * t + phase_i) term and summed.
Best regards,
Gerrit
Thanks a lot Gerrit 🙂
Hello Gerrit,
Thank you for a very wellwritten article.
I have a question I want to answer and I was glad you touched on it.
You stated that:
"If a single component has no constraints, then the model will have six rigid body modes. They correspond to the component translating respectively in X, Y and Z and Rotating about X, Y and Z. Notice that the modes is unlikely to be aligned with the global coordinate system as a linear combination of rigid body modes is also valid as a rigid body mode."
If a model is unconstrained, then sweeping a range of frequencies should excite the 6 rigid body modes in pure xyz translation and rotation. In a model I'm working on, the modes however are about seemingly random axes, and most have two components to their motionthus as you stated, not aligned with the global coordinate system.
Is this simply a function of the way the model has been built (i.e additional coordinate systems)? Or is there something else going on?
Thanks again!
Hi Zach,
The reason for the "random" rigid body modes (RBM) is not due to coordinate systems. Any six rigid body modes that are massorthogonal is a valid vector set for the rigid body motion. The basis vectors chosen is (nearly) random, so picking pure translations and rotations is extremely unlikely.
There is nothing wrong with these modes though  they are perfectly valid and will allow any rigid body motion you want to apply to the body (pure translation or rotation included) if you have the correct scale factors for the RBMs.
Your statement "If a model is unconstrained, then sweeping a range of frequencies should excite the 6 rigid body modes in pure xyz translation and rotation." is incorrect: Rigid body modes occur at zero Hz  i.e. a constant load applied. The location and direction where the load is applied will determine whether the resulting motion is pure translation, pure rotation, or some combination motion.
In other words, for every rigid body motion you want to measure or calculate from running a transient analysis (not modal analysis!), you have to apply a load in either a different location or a different direction. For pure, translations you have to apply the load in such a way that the equivalent force acts through the center of gravity of the body. A "gravity" type load will be most accurate for this.
Back to the question on these "random" RBMs: The only reason we would like to see pure translation and pure rotation modes is that it looks pretty. From the mathematics perspective as well as from the physics (i.e. dynamics) perspective of the body, there is no reason to want "pure" RBMs
If you really want "pure modes" for visual purposes, you can obtain them in Nastran. To calculate them, then you have to "guide" Nastran by specifying "SUPORT" cards (yes, single "p" in "suport"). The "suport" card is used to define a reference coordinate system for the rigid body modes. You can read up on it in the Nastran Dynamics Guide in "Chapter 3: Real Eigenvalue Analysis" in the section "Suport Entry". For other software, you will need to contact your local support to find out how to get them.
Best regards,
Gerrit
Suppose if I run a natural frequency analysis for 25 mode shapes in order to calculate DAF for performing pseudo static analysis for blast load. Which time period shall I pick up for calculating the DAF?
Hi abc,
I assume the blast load is for a blast in a pipesystem (I had to look it up just to see that DAF (Dynamic Amplification Factors) in Blast was used for pipes in the chemical industry...). Unfortunately I can't comment with any level of certainty as I have not been exposed to this industry's methods.
What I saw in published papers seem to refer to blast duration as the one period used, and 1/f (for each natural frequency) for the other set of periods. The code of practice you use should explain how to determine the blast period to use and whether you should combine it with one mode only (the worst one?) or with all modes calculated.
Best regards,
Gerrit
Hi Gerrit,
Thank you for your very well written article.
I was confused when you state " With damping, the oscillation will grow to the point where the damping will remove exactly the same amount of energy from the system as the amount of energy being added by the excitation load."
Perhaps I missed something, but why can the oscillation not keep growing past this point?
Thank you!
Ari
Hi Ari,
Forced vibrations are outside the scope of the article as it is the response of the system due to a load, and not just a mode. This is why I didn't include the mathematics behind forced vibrations. Unfortunately this can cause confusion, so I'll try and clear it up in a hopefully relatively simple (nonequation) explanation first.
If the oscillation magnitude is greater than the steady state oscillation for a damped system, then the damper would remove more energy than the applied load can add to the system in a cycle. The resulting reduction in energy results in smaller oscillation for the next cycle. As the oscillation reduces, so does the damping energy removed from the system. The oscillation reduces until the added (due to the load) and removed (due to damping) energy is the same per cycle at which point steady state is achieved.
If you search for "forced damped vibration equation" you'll come across a lot of websites that derives the equation of motion for a damped system. The "magnification factor" described on these pages is the ratio between the maximum displacement due to a static load and the amplitude if the same load is applied at some frequency. Just for reference, this ratio is
1/sqrt( (1(w/wn)^2)^2 + 2*(zeta*w/wn)^2 )
where w is the frequency (rad/s) that the load is applied at, wn is the natural frequency (rad/s) and zeta is the damping ratio.
From this, if the damping ratio is zero and w=wn, then both terms in the squareroot becomes zero. 1/0 means the response is infinite for the case of no damping and the load applied at the natural frequency.
On the other hand, if the damping ratio is greater than zero, then the second term in the squareroot will be positive for all frequencies greater than 0 rad/s. The first value will be zero (at the natural frequency) or positive (for all other frequencies). Therefore, the magnification factor is one divided by a positive nonzero number, independent of the frequency. This means that the magnification if finite if the system is damped at all frequencies.
Most websites you'll find will plot the magnification factor as a function of frequency for different damping ratios.
Best regards,
Gerrit
Thank you!
Very informative, thanks Gerrit. My concern now is on the identification of these points, do our FEA packages explicitly distinguish these points?
Hi Elias,
If your reference to "these points" is referring to the natural frequencies and mode shapes, then yes. If you run a modal analysis the results are the modeshapes and corresponding natural frequencies.
Best regards,
Gerrit
Hello
I am getting negative eigen Values in one of the modal analysis. What does it mean?
Hi,
Without more info on the analysis type, software you use and the eigenvalue extraction method, I can only provide some generic pointers to what the problem may be.
Is it a realmodal or complex modal calculation? Real is the most common and is used for undamped symmetrical systems.
Complex modes can have complex natural frequencies which can be stable or unstable. A negative eigenvalue is therefore possible in a complexmodal calculation.
For a real modes, it should in theory not be possible to get negative eigenvalues, but there are a couple of reasons for negative values to sometimes appear:
 Small negative values may possibly occur due to roundoff errors in the calculations of the eigenvalue equation. This will in all likelyhood refer to rigid body modes as it should have been "exactly" zero.
 Badly conditioned stiffness or mass matrix can also cause roundoff errors which cause lots of havoc with all analysis types, including modes
 A singular massmatrix can cause infinite modes which will appear as either large positive or negative values
Best regards,
Gerrit
Hello Gerrit,
Can you please explain Participation factors, Ratio and effective mass for a modal analysis. I would like to know its significance also.
Hi Vishnu,
You can easily get the equations for these on the web, so I'll rather concentrate on the physical meaning here.
The modal effective mass for each mode is reported separately for each of the 6 directions of motion (3 Translations, 3 rotations). The modal effective mass is effectively the amount of mass participating when a basemotion is enforced in a specific direction at the mode's natural frequency. If we add add the modal effective mass of all modes of the structure for one direction at a time, then the total modal effective mass will be the same as the mass (or inertia for rotations) of the structure.
Modal effective mass fraction is obtained when we divide the modal effective mass by the mass (inertia for rotations) of the structure. The sum of the mass fractions for each direction adds up to 1. In other words, modal effective mass fraction is the "normalized" modal effective mass.
Mode participation factors are seldom directly useful: They are mostly used as an intermediate step to calculate the modal effective mass.
The modal effective mass fraction is an indirect indication of how well a mode can be excited by basemotion. If we have a mode with a modal effective mass fraction of 0.9, then this mode is the dominant mode in this direction. The sum of all other modes in this direction is 0.1 (or 10% of the mass).
Another useful example is if we have a mode where the motion of all nodes in the model is in the purely in the Xdirection. Intuitively it should be obvious that we can't excite this mode by applying a sinusoidal baseexcitation in the Y direction at the mode's natural frequency. If we calculate the modal effective mass fraction for such a mode, we will find that only the Xdirection will have a nonzero modal effective mass fraction.
Therefore the use of the modal effective massfraction is to determine which modes are important in a specific direction. We can use this in a modaltransient or modalfrequency response analysis to determine whether we have enough modes to represent the response of the system as well as to determine which modes we can ignore. The idea is that we should have a cumulative mass fraction in the direction we apply the base motion of as close to one as is reasonable.
Any number I report here will be controversial  please don't take my numbers as being "reasonable", it is only intended as a relative example. For quickanddirty analysis, we may be happy with a total fraction of 0.9. In general we are shooting for a fraction of at least 0.95 or even 0.99. Please find out in your company / industry what the recommended target modal effective mass fraction is when running modal methods.
Best regards,
Gerrit
There is a line in the article which says "It is entirely possible for a structure to have multiple modes at the same frequency. However, the modeshape will be in different planes." I am confused what could be the reason for the same or there are some references to prove.
When you have a perfect double symmetrical structure, e.q. a square plate, it's first mode(s) can be about either of it's bending axes (e.g. X or Y in the Z plane). In FEA analyses it will show up as two mode shape results at the same frequency. In reality though, any minute imperfection or instability will determine which of the two shapes will appear. They can not present themselves at the same time offcourse.
Hi there would you mind stating which blog platform you're working
with? I'm going to start my own blog in the near future but I'm having a difficult time making a decision between BlogEngine/Wordpress/B2evolution and Drupal.
The reason I ask is because your design and
style seems different then most blogs and I'm looking for something
completely unique. P.S My apologies for getting offtopic but I had to ask!
No problem. We use WordPress for the content and Oxygen for the styling.