Performing Modal Analysis in Ansys Mechanical

[Music] hello everyone in this anses how to video we will show you how to perform one of the most fundamental linear dynamics analysis modal analysis the need to determine the natural frequencies of a structure can apply to many areas of engineering some examples include tacoma nervous bridge blade disc or valve body considering the dynamics effect in design is quite critical in this video we will focus on free vibrations or modal analysis of the mechanical systems let's go [Music] model analysis provides valuable insights to the dynamics characteristics of the structure it is a linear analysis that doesn't utilize any excitations or loads mode frequencies are dependent only on two things stiffness and mass model analysis provides engineers with information regarding how the design may respond to different types of dynamics loading and can be used for example to avoid resonant vibrations that can be harmful to the structure that is why the modal analysis is the most fundamental of all dynamic analysis it is the basis of all other linear dynamics analysis such as harmonic response spectrum or random vibration let's see how we can calculate natural frequencies and mode shapes the linear equation of motion for free undone vibration is mass matrix time acceleration plus stiffness matrix times displacement where m is the mass matrix and k is the stiffness matrix if we assume harmonic motion the displacement and acceleration vectors can be expressed by these two equations substituting displacement and acceleration back into the equation of motion we can get the eigenvalue problem solving for the first part of this equation gives the natural frequencies omega and solving for the second part of this equation gives the mode shapes v the eigenvalues are the square of the natural circular frequency of the structure omega and eigenvectors are the corresponding mode shapes v in the example of the simple vibrating beam fix on the both ends if the beam displays a mode shape of half of the sine wave it would be vibrating in modes one or two if the beam displays a mode shape of a full sine wave it would be vibrating in mmo 3. natural frequencies f i can be then calculated as f i equals omega i over 2 pi cycles per second the eigenvectors represent the mode shapes obtained when the structure is vibrating and frequency applied the participation factor and effective mass obtained from a modal analysis can give an idea how the design will respond to different types of dynamic loading participation factor measures the amount of mass moving in each direction for each mode and it can be calculated by this equation where d is the unit displacement spectrum in each of the global cartesian directions and rotation about each of the axes in ansys mechanical the participation factors for each direction is reported under solution information or by looking at a solar output a high value of the participation factor in a direction indicates that mode will likely be excited by forces in that direction some modes may contribute more than others depending on the mode shape and participation factor value if for example we know which mode may be excited in a particular direction that can help in design assessment since we know what the frequency and mode shape is thus by looking at the ratios we can identify the modes that can contribute a lot to the structure response if excited in a particular direction the effective mass is a measure of how much mass is associated with each mode when we use the default mass normalized approach the effective mass is equal participation factor squared ideally the sum of the effective masses in each direction should equal to the total mass of the structure but that will depend on the number of modes extracted and how the structure is constrained the ratio of effective mass to total mass can be useful for determining whether or not a sufficient number of modes have been extracted the material near the supports is generally less likely to move so effective mass will be smaller than actual mass of a structure based on how much material is located near fixed supports in the example we can see that about 73 of mass is associated with modes 1 2 and 6 which means that these modes are going to be excited by forces in x direction of the cartesian coordinate system let's go and see how we can do model analysis in ansys mechanical in this demo we will show you model analysis of the metal frame and how to get model frequencies and mode shapes additionally we will look at the participation factor and effective mass and see the effect of number of extracted modes on these quantities insert modal analysis system on the project page import geometry check material structural steel is assigned material by default insert mesh sizing under mesh and set the sizing to 0.05 meters geometry is suitable for sweep mesh and we want to ensure that there are at least two elements to the thickness of the frame for the better accuracy insert fixed support and scope it to the entire perimeter of the frame under analysis settings we can specify a maximum number of modes to find and under limit search to range we can specify the frequency range in this example the number of modes to extract will be the default number 6 and the default frequency range will be used next solve the model once you get a solution the table of most numbers and frequencies is available right click and select all right click and create mode shapes notice that 6 total deformation results are inserted in outline tree automatically right mouse click on the solution and evaluate all results click on the total deformation this is mode 1. the tabular data shows corresponding natural frequencies let's look closer into the participation factors and effective mass click on the solution information and under solution output select participation factor summary to see participation factor and effective mass tables the participation factor is used to determine how much of the mass of the certain mode is moving in the same direction as the excitation a high value in a direction indicates that the mode will be excited by forces in that direction participation factors are available in all six directions as we mentioned previously in this case for example mode 5 is mode that is making a meaningful contribution to the response in x direction and will be excited by forces in that direction let's look at the effective mass effective mass is giving the amount of mass moving in a certain direction for a given mode the value is higher for the more prominent modes in this example if you look at the ratio of effective mass to total mass about 13 percent of overall mass is moving in the direction of the mode 5 which is x direction the sum of the effective mass is a good indicator is enough modes are extracted the effective mass in each direction should add up to overall mass of a structure but that would depend on how the structure is constrained let's see what happens if we extract 200 modes under analysis settings set maximum number of modes to find to 200. next solve the model next see the participation factor and effective mass in the participation factor summary more prominent modes can be identified by the higher value of the effective mass as we can see about 63 percent of overall mass is moving in x direction comparing to the previous case where only 13 of the mass was moving in x direction we can see a higher percentage of the actual mass moving in x direction when 200 modes are extracted but it is still not 100 of the actual mass why in this model there is the fixed support around the perimeter of the frame so the material near the fixed constraint won't move and effective mass will be smaller than the actual mass this concludes the demo now let's summarize what we learned in this video model analysis calculates natural frequencies and mode shapes of the structure participation factor shows the most prominent modes in a certain direction that will be excited by forces in that direction the effective mass can be useful for confirming that enough modes have been extracting for further analysis such as harmonic response spectrum or random vibration i hope that you find this video informative please share the video post your comments and subscribe to this channel to stay updated don't forget to visit courses.ansys.com to discover more useful courses you

Channel: Ansys Learning

Views: 17,443

Rating: 4.9597988 out of 5

Keywords:

Id: CGpNf1Zi9AI

Length: 11min 15sec (675 seconds)

Published: Fri Nov 20 2020