## Interpretation & Importance of Mass Participation in Modal Analysis

We often come across the dynamics or vibration problems in most of the product development across all industries.  We have gained enough knowledge through the degree of Bachelors or Masters, with an example of the famous engineer disastrous design of “Tacoma Narrows Bridge-1940”, that considering the dynamics effects in design is quite critical.  Generally, a dynamics problem is categorized into linear or nonlinear dynamics. This blog is related to the linear dynamics and nonlinear dynamics will be discussed in length in another blog. The most commonly heard terminology which we stumble upon in the design of such vibrating products is “natural frequencies“, “resonance“, “eigenmodes” etc. We have many linear dynamics simulation techniques such as “Harmonic Analysis“, “Random Vibration“, “Response Spectrum“, “Transient Analysis“, “Acoustic Analysis“, etc based on the loading it undergoes and also on the output we are interested in. But all these dynamics simulations start with the first step called “Modal Analysis“.

# Modal Analysis

What makes something unique is an identity of its own, right? What if I say natural frequency is the identity of a body? Let’s see why. Assume you are imparting energy (striking) to a body. What will happen is obvious, the body will start to vibrate. But the vibrational frequency will be in its natural frequencies. It doesn’t matter how much or where you give the energy it will always vibrate in its natural frequencies, period.  This is why the base of any dynamic analysis is said to be modal analysis as it shows its identity or behavior.

The modal analysis calculates natural frequencies and mode shapes of the designed model. It’s the only analysis that doesn’t require any input excitation or loads, which also makes sense, as mentioned before natural frequencies are independent of the excitation loads. Natural frequency depends only on two things mass and stiffness.

### Why do we need to do the modal analysis?

Yes, we can find natural frequencies, and mode shapes through modal analysis but why to do it? Let me explain that through an example, when you ride a motorcycle, sometimes you might have experienced vibration in your handle. Some bikes have too much vibration that, you can’t even use your rear mirror. This is because the handle’s natural frequency is matching with engines RPM.

Structure borne noise: A structure makes peak noise when it’s vibrating in its natural frequency.

Whirling of shafts: To find the critical RPM of a shaft so that, crossing the critical speed will be done with precautions to avoid resonance.

Avoiding resonance is always preferred, thus shifting or modifying natural frequency can help to control, above mentioned issue. Natural frequency depends on only two parameters, modifying them will help to design a dynamic body part.

As an engineer, I always go in search of the physical meaning rather than proving by an equation. But at times equations are unavoidable.

Now let us see how we can get the natural frequency of a system.

Excitation force Equation of any dynamic system can be represented as

Every natural frequency is associated with each mode shape and mode shape represents the displacement behavior. There is enough material on the internet which explains mode shape. Right now, let’s concentrate on the “Mass Participation Factor” other important information from modal analysis, which would assist us in the simulation of other linear dynamic simulations.  What is mass participation in general? Consider a 3 massed system as shown below.

The figure shown above is a mode of the system. Here masses participating in the X direction are M1 and M2  and thus total mass participation is M1 +M2.  The only difference in FEA is that instead of lumped masses, the system will be discretized by elements.

Now let’s see ANSYS modal Analysis. Here I’m taking a cantilever beam, with 0.8478 kg. Having a cross-section of 3*60*600.

As you can see from the participation factor calculation. I have solved the first 12 natural frequencies. In this table, ANSYS solver calculates only frequency and Participation factor ie 1st and 4th column. Every other column is calculated from these two values. Let’s look at the most important column one by one.

As you can see this ratio is in direct comparison with total mass, which gives a better clarity on how much of the total mass participation is extracted. In other words, the sum of the effective masses in each direction should equal the total mass of the structure. But clearly, this depends on the number of extracted modes.

The same logic is for rotational mass participation. But here you might get ratios bigger than 1. Then, there can be confusion as mass participating is more than the total mass of the system? The answer is, participation factors for rotational DOFs are calculated about the global origin (0,0,0). The calculated effective mass essentially contains a moment arm (effective mass multiplied by the distance from centroid). Thus, the effective mass for the rotational DOFs can be greater than the actual mass and the participation factors can be greater than 1.0.

Ideally, the ratio of effective mass to total mass can be useful for determining whether or not a sufficient number of modes have been extracted for the “Mode Superposition” for further analysis. Modal superposition is a solution technique for all linear dynamic analyses. Any dynamic response can be calculated as the sum of the mode shapes, that are weighted with some scaling factor (modal coefficient). Also, the time step of the transient simulation is calculated based on the most influential mode in the modal analysis.

Modal analysis is usually done without considering any force or working environment. This assumption is taken by considering mass and stiffness to be constant. But at times this doesn’t work, like a pressurized vessel or pipe. As compressive or tensile force changes the stiffness. In such cases, we have to do a prestressed Modal Analysis.

In some cases, like rotating shafts with motors, turbines, the natural frequency will not match with the working condition. This is because, for different RPM, stiffness also changes,(Centrifugal force changes). In these cases, we need to consider the rotational speed of the shaft. In ANSYS Modal Analysis (Rotodynamic Analysis) rotational speed with Coriolis effect can be directly given to find the critical speed of the shaft.

Modal analysis is a prerequisite for all linear dynamics analyses like Harmonic, Random vibration, and Response spectrum analysis. Hence Modal Analysis plays a huge role wherever you are trying to find out vibration characteristics of a design. Thereby it is relevant for most industries like Rotating machines, construction, automobile, Machine tool, agricultural equipment, and Mining.

Engineering Simulation opens up a huge range of possibilities. Since CAEsimulation requires more than just software, we at CADFEM help our customers to adopt simulation for success in every phase of product development, thereby enabling them to realize their product promise.

Please feel free to connect with us at marketing@cadfem.in or +91-9849998435, for a quick Demo on this Product.

Author Bio:

Mr. Vineesh Vijayan, Application Engineer

Mr. Vineesh Vijayan has done his Master of Technology in Machine Design. With good expertise in Structural Simulation currently, he is contributing his efforts to CADFEM India as an Application Engineer.

## Demystifying Modal Analysis (Part I)

In this article, I will discuss about modal analysis – a topic that is standard, however I’ll strive to demystify it using a simple example and FAQs.

###### Motivation for Modal Analysis

As a mechanical engineer, life is always interesting because I can correlate the knowledge gained from books to real life scenarios. As a student, my professor gave a real example of a bridge failure due to marching soldiers. What followed was a very interesting lecture about dynamics. Until then, I never understood the power of the words such as dynamics, vibration and resonance. Of course, the example provided food for my thoughts to study more about how a bridge could fail due to lesser dynamic load compared to a heavier static load.

For those of you who are curious, the bridge was England’s Broughton Suspension Bridge that failed in 1831 due to the soldiers marching in step. The marching steps of the soldiers resonated with the natural frequency of the bridge. This caused the bridge to break apart and threw dozens of men into the water. Due to this catastrophic effect, the British Army issued orders that soldiers while crossing a suspension bridge must ‘break step’ and not march in unison.

Such failure has given rise to more emphasis on analyzing the structure (mechanical or civil) for dynamic loads if it undergoes any sort of vibrations. Traditionally test equipment have been used to experimentally monitor vibrations in new designs; this is costly however. We apply finite element analysis (FEA) to solve such problems. FEA solvers have evolved and today’s solvers are powerful not only in statics but in dynamics too. ###### Modal Analysis: Getting Down to the Basics

In any dynamic/vibration analysis, the first step is to identify the dynamic characteristics of the structure. This is done through a simple analysis called Modal Analysis. Results from a Modal Analysis give us an insight of how the structure would respond to vibration/dynamic load by identifying the natural frequencies and mode shapes of the structure.

Modal Analysis is based on the reduced form of dynamic equation. As there is no external force acting and neglected damping, the equation is modified to: I have skipped the derivation part of natural frequency as it is easily available in textbooks. Natural frequency is substituted back into the equation to find out the respective mode shapes. These natural frequencies are the eigen values whereas the respective mode shapes are its eigen vectors. Natural frequencies & mode shapes in combination are called as modes.

Eigen vectors represent only the shape of deformation, but not the absolute value. That’s the reason it is called as mode shape. It is the shape the structure takes while oscillating at a respective frequency. Important point to remember is the structure has multiple modes and each mode  has a specific mode shape. If any load is applied with same frequency as natural frequency in the same direction as mode shape, then there will be increase in magnitude of oscillation. With no further damping, the scenario will lead to a failure due to a phenomena called resonance. To avoid this phenomena in dynamics, calculating the modes carries great importance.

Having said that, questions will certainly arise. In my opinion, these are the most commonly asked questions in support calls by customers using ANSYS.

• Why do frequencies from simulation don’t match the test results?
• Why are deformation and stresses in modal analysis very high?

From equation (3), it is clear that natural frequency of structure depends on its stiffness and mass. In order to accurately capture frequencies in FEA, the following points are important for you:

• You need to capture mass of the structure and connecting/ignored members accurately.
• Your mesh can be coarse, but enough refinement so that you can accurately capture the stiffness of the structure. If you are interested in the local modes in slender members, then you’ll need to perform local mesh refinement.
• You need to define appropriate boundary conditions in forced modal analysis in order to capture realistic frequencies.
• You need to accurately model the contact between different bodies in an assembly since they affect the stiffness of the structure drastically.

For the second question, a lot of confusion exists when the modes extracted in modal analysis show deformation magnitude. In Equation (2), you will see that no external load is applied on structure. This will make you wonder where these values come from? Let’s have a look with an example of simple cantilever beam.

Fig. 1 shows its extracted mode shape 1 & stress shape 1 from modal analysis. I observe deformation to be as high as 253 mm and stress as 4,914 MPa which is far greater than the ultimate strength of Steel i.e. 500 MPa. You may wonder, why did we get these high values?

This happens because the FEA solver returns the mode shape (not the deformation magnitudes) as output. By this, I mean that magnitude of the mode shape is arbitrary (as seen in Fig. 1). The high value is because of a scale factor that’s chosen for mathematical reasons and does not represent anything real for the model. However this value helps us in relative measurement. Let’s take the example of the first mode. Maximum deformation occurs at the free end compared to any other location. This changes with the change in mode.

Since we have deformation, you can compute corresponding stresses and strains. Once again, these are relative values. If you ask the FEA solver for stresses & strains, it will use the same scaled deformation magnitudes and calculates stresses & strains. They are referred to as stress shape & strain shape (not to be confused with stress state or strain state) because no loads are applied. The magnitude of stresses and strains are useless but their distributions are useful to find hot-spots in the respective modes.

###### Conclusion

Modal analysis offer much more than just the frequencies and mode shapes. This analysis is primarily the stepping stone for linear dynamics studies to calculate the actual deformation due to different kinds of dynamics loads. Modal analysis has many secondary applications which I will discuss in my next blog.