COMSOL 6.4 - Bracket — Frequency-Response Analysis

A frequency response analysis solves for the linear steady-state response of a structure when subjected to harmonic loads. The problem is solved in the frequency domain and you can prescribe a range of frequencies at which to compute the response.

In this example, you learn how to perform a frequency response analysis of a structure under only harmonic loads, and also how to perform a frequency response analysis of a prestressed structure.

It is recommended that you review the Introduction to the Structural Mechanics Module, which includes background information and discusses the bracket_basic.mph model relevant to this example.

•

In the Structural Mechanics Modeling chapter of the Structural Mechanics Module User’s Guide:

Frequency-Domain Analysis

Mode Superposition

Harmonic Perturbation

•

COMSOL Blog: Frequency Response of Mechanical Systems

Model Definition

This model is an extension of the model example described in the section “The Fundamentals: A Static Linear Analysis” in the Introduction to the Structural Mechanics Module.

The geometry is shown in Figure 1.

Figure 1: Bracket geometry.

You study two load cases. In the first case, a harmonic load in the X direction, with a total amplitude of 25 N, is applied to the boundaries of the bracket holes. The load is equally divided between the two arms.

The second load case consists of a combination of a static preload and the same harmonic perturbation.

An eigenfrequency analysis of this structure is performed in the tutorial Bracket — Eigenfrequency Analysis. It shows that the first natural frequency is about 114 Hz. For the prestressed case, the eigenfrequency solution shows that the first resonance frequency is about 105 Hz when the arm is under a compressive load, and about 128 Hz when the arm is under a tensile load. In order to capture the resonance peaks properly, you can refine the frequency stepping around these values.

Results and Discussion

An important property of frequency domain studies is that the results are complex-valued. During result evaluation, you must be careful about whether you present values at a certain phase angle, peak values of the cycle, or RMS values.

The default plot in a frequency-domain analysis shows the variable
<phys>.misesGp_peak. This is a special variable that, in each point, contains the maximum von Mises stress over the whole cycle. The standard von Mises stress variables contain the stress at the current phase angle. This may be far from the peak stress, if there are significant phase shifts. In Figure 2, the stress at the last computed frequency, 750 Hz is shown. More interesting is to study the results at 114 Hz at which the first natural frequency is located. This is shown in Figure 3. Here, the peak value is around 115 MPa, to be compared with 1 MPa in the previous case.

Figure 2: von Mises stress at 750 Hz.

Figure 3: von Mises stress at 114 Hz.

Figure 4 shows the root mean square (RMS) of the displacement at the tip of the arms of the bracket around the first resonance for both the pure harmonic load case and the combined harmonic and static load cases.

Figure 4: RMS of the displacement at the tip of the left (blue) and right (green) arms. The results without prestress are shown with solid lines, while dashed lines are used for a case with a combination of static and harmonic loads.

The curves show resonance peaks around 114 Hz for the unloaded structure in both bracket arms and a frequency shift for the loaded structure. These results are in agreement with the values predicted by the eigenfrequency solution. The curves for the left and right arms coincide as long as there is no prestress.

You can also verify that the deformation remains small even around the resonance frequency. Thus, the linearity assumption necessary for frequency-domain studies is fulfilled.

Figure 5 shows the phase of the x-displacement at the tips of both arms.

Figure 5: Phase of x-displacement at the tips of the arms.

Note the smooth transition where the displacement is in phase with the load at lower frequencies and in counterphase for higher frequencies. This is an effect of the damping, where a 5% loss factor is used. The solution for the prestressed case shows interesting properties, where the phase flips at different frequencies in each arm. This can be interpreted so that the two arms move synchronously for low and high frequencies, but against each other for intermediate frequencies.

In Figure 6 and Figure 7, the perturbation of the von Mises stress is shown at 107 Hz and 128 Hz. This result is the linearized deviation from the constant stress caused by the static preload, and thus the values can be both positive and negative. Each arm dominates the response in the vicinity of its own eigenfrequency.

Figure 6: Perturbation in von Mises stress at first eigenfrequency, 105 Hz.

Figure 7: Perturbation in von Mises stress at second eigenfrequency, 128 Hz.

It is possible to display the variation in time domain of any result by using the phase angle as parameter for graphs. In Figure 8, the variation of displacement in the direction of the load is shown at two frequencies close to the two first eigenfrequencies. Note that the horizontal axis has phase angle as unit. This is essentially a scaled time.

Figure 8: Displacement history at two locations and two frequencies.

Quantities that are linear functions of the solution will share the property of being time harmonic. This would, for example, be true for a single stress tensor component, but it is not true for equivalent stresses. This is illustrated in Figure 9, where the von Mises stress is shown for studies with and without prestress.

Figure 9: Various representations of the von Mises stress in a point at resonance frequency.

Since the von Mises stress by definition is always positive, the result for the study without prestress looks similar to the absolute value of a harmonic function. When the prestress is added, then the von Mises stress is fully harmonic, since it can vary around the static prestress while still being positive.

Figure 10 shows the RMS of the x-component of the velocity of the arm of the bracket over the whole solved frequency range for the analysis without prestress as a one-third octave band plot. The band centered at 630 Hz shows a local maximum related to the second flexural mode of the arms.

Figure 10: One-third octave band plot of the x-component of the velocity at the arm tip.

Notes About the COMSOL Implementation

For structural mechanics physics interfaces in COMSOL Multiphysics, there are six predefined study types available for frequency-response analysis: ; ; ; ; ; and ;

The modal analysis uses the modal solver to compute the frequency response. This analysis type speeds up the computation significantly when compared to the regular frequency-domain analysis if the number of frequencies is large. In this example, the modal solver is used in the first study, and the direct solver in the second study. This is purely for comparison. If the modal solver had been selected also for the second study, it would run more than 10 times faster.

Use the prestressed frequency-response analysis when a structure is subjected to both static and harmonic loads, and the stiffness induced by the static load case can affect the structural response to the harmonic load.

When working with results from a prestressed analysis, there are several options for how to evaluate the solution. You can, for example, choose to display the total solution or only the perturbation part. The five graphs in Figure 9 are created using the settings summarized in Table 1.

Table 1: Graph settings
Graph Legend	Study	Frequency	Variable	Expression Evaluated for	Compute Differential
Without prestress	Study 1	114 Hz	solid.mises	N/A	N/A
With prestress	Study 2	107 Hz	solid.mises	Total instantaneous solution	N/A
Static solution	Study 2	Any	solid.mises	Static solution	N/A
Perturbation from prestress	Study 2	107 Hz	solid.mises	Harmonic Perturbation	Yes
Peak value for perturbation	Study 2	107 Hz	solid.mises_peak	Harmonic perturbation	No