
"First, don't panic," suggests David Dearth, a consulting analyst and president of Applied Analysis Technology, ([email protected]) Huntington Beach, Calif. "You can solve dynamicresponseanalyses problems from harmonic excitation. All you need is a little background and a few sample problems with known solutions," he says.
First of all, a modal analysis differs from a dynamicresponse analysis in that vibration modes are for resonant frequencies, like ones extracted experimentally with a hammer tap. They don't involve quantitative deflections, despite what animations show. Dynamicresponse analyses ask for nondimensional deflections (mode shapes) and compute stresses from vibration inputs that might come, for example, from an outofbalance motor.
Most FEA programs that do dynamicresponse analyses use base excitation. "The technique essentially ‘shakes' a digital model as if it were fastened to a shaker table. In other words, base excitation exposes models to inertia loading at specified ‘g' levels," he adds. The program then matches freevibration frequencies (resonances) from a table of frequencies (and mode shapes) corresponding to the input frequencies. When freevibration frequencies come close to the input or excitation frequency, the program computes a possible response (amplification) to the external excitation. "In many cases, you'd like to find the response of a structure to variable excitation, frequencies, and ‘g' levels, and at different structure locations. Solving those problems calls for more comprehensive FEA programs, such as MSC/Nastran," says Dearth.
Dynamicresponse analysis can be difficult to address without a solid foundation in resonant vibrations. "Resonant vibration or RV problems involve obtaining the natural frequencies and associated mode shapes," says Dearth. "RV frequencies are also called freevibration frequencies. Such frequencies are useful when they fall near the range of what external vibration designs might experience in their service life."
When FEA models are processed for modal analyses, the solution includes a table of resonant (free) vibration frequencies. "There is a corresponding mode shape for each frequency in the table. This shape, stored in a displacement output file, is sometimes called a load case or solution set depending on the software. The program might also generate an output file containing stresses for each mode shape. The table and associated mode shapes will also contain coupled modes," explains Dearth.
Animation routines in most software show an FEA model's shape at each resonant frequency. "Unfortunately, novice analysts mistakenly think they have completed a response analyses after viewing animated resonantmode shapes because they see results for stress and deflection." But the magnitude of deflected shapes from resonantvibration analyses give only an indication of how the structure will deform when subjected to external excitations at the same frequency as the one under display. The shapes are good, but the magnitudes are not. "These displacement and stress results are simply reference information," he says.
The big issues become: How to relate physical observations from the lab to approximations from virtual testing with FEA techniques? And how do you simulate physical testing using computer analyses?
"The key to relating displacement mode shapes is that one must process a dynamic response in addition to the resonantvibration analyses," says Dearth. "To simulate harmonic dynamic response, process the FEA model for an external excitation force at the resonant frequency associated with a deflected mode shape. The dynamicresponse analyses determines the precise magnitude of displacements and stresses at a particular resonantvibration frequency to an external excitation," he adds.
Dynamicresponse analyses, unlike resonantvibration analyses, subject FEA models to external loading, usually in terms of gravitational acceleration, or "gs," at a specific resonant frequency (or by a sinusoidal input forcing function). The software uses reference results from the table of resonantvibration frequencies to assess the response of the component structure or assembly to given inputs. Running
the analyses then gives meaning to the magnitude of the displacements and stresses. Finally, during environmental testing, when designs carry inertia loading at a specified acceleration and frequency input, designers can predict the stresses and how much the actual part or assembly will deflect.
The problem most novice FEA analysts still face is: How do you know you have performed all necessary tasks to generate the correct response to the vibration excitation? In a word — experience. "And that comes from solving several sample problems," says Dearth. He suggests testing your skill with the beam on the previous page. It lets readers do a quick sanity check with only pencil, paper, and calculator. "If readers cannot solve simple problems by hand, then how can they solve problems using a computer?" he asks. "Remember, the same hoops one must jump through to solve simple FEA models are the same for real problems solved by a computer. The only difference is usually the complexity of the geometry."
The problem here, A simply supported beam, has a uniform cross section and a concentrated midspan weight. "It can be solved in four steps," explains Dearth.
Estimate the fundamental mode of vibration. Using equations from engineering books, estimate the model's fundamental, or first, natural frequency. "Check two cases," suggests Dearth. "In case A, consider only the concentrated weight and neglect the beam weight. In case B, include the beam's distributed weight with the concentrated weight. Remember, handbook formulas are for uncoupled modes of vibration. Handbooks can't give analysts coupled modes of vibration with components of bending, torsion, axial modes, and account for complex geometry. FEA programs, however, do provide this information. The cookbook approach works if you can make intelligent, simplifying assumptions that will make complex geometry fit into one of the cookbook solutions," he says.
Estimate peak static stresses and deflections. Using similar handbook equations, estimate the peak static stresses and deflections for case A and B. Set the staticload case at 1g inertia loading in the direction of input excitation. Referring to the model, let the staticload case condition be N_{z }= ±1 g .
Estimate peak stresses and deflections due to dynamic response at harmonic input. Using the first resonantvibrationfrequency mode shape for this simple beam model, make simplifying assumptions to estimate the response due to sinusoidal input, base excitation using a singledegreeoffreedom
spring analogy. For light damping C/C_{c }< 0.05, about 5% critical damping. The magnitude Q of the input amplification is Q = 1/(2 ). For example, at 5% damping Q 1/(2 0.5) = 10. In other words, the amplification of input excitation at the first resonant frequency is approximately 10:1 for the case of a 5% damping ratio. Therefore, for a 1g input excitation at the first harmonic (resonant) frequency, with 5% overall structural damping, peak stresses and deflections at dynamic response will be about 10 times greater than for the 1g static condition.
Process the FEA model for the dynamic response at the harmonic input. Develop an FE model of the beam and ensure that it correctly approximates the static stress, static deflections, and resonant vibration frequencies for Cases A and B.
Process the dynamic response due to harmonic excitation for cases A and B and compare results.
The Summary results, presented in the December FE Update column, will include the difference between manual estimates and an FEA model of the beam, processed with MSC.Nastran. The table compares manual estimates for the fundamental resonant vibration frequencies to FEAgenerated figures, along with static stresses and deflections.