Featured Case StudyThe Norsea Gas Terminal in Northern Germany plays a vital role in the connection of pipeline systems coming from the North Sea to the natural gas distribution network throughout Germany. Built in...Stay
- ANSYS Software
Featured Case StudyRelying on ANSYS Composite PrepPost helped EADS Innovation Works to develop lightweight composites in aircraft design. ANSYS Composite PrepPost provided simple pre- and post-processing of composite...Stay
- Resource Library
- News &
Thermo-Mechanical Analysis Methods for Printed Circuit Boards Part 3: Vibration Analysis
In previous blog entries, Mike Kuron discussed modeling techniques for the board, and thermal analysis of electronic components. In this third installment, I will address structural analysis of PCBs in terms of assessing their ability to survive vibratory load environments.
PCBs are used in most electronic products to mechanically support and electrically connect chips, capacitors, resistors, or other electronic components via soldered joints. Since many of these products will experience loading environments that include vibration loading, it is vital to determine the structural integrity of the PCB and its components due to these loads. This determination is often achieved using a random vibration finite element analysis.
The steps to perform a random vibration analysis of a PCB can be divided into three parts:
1. Create the finite element model including representations of PCB, stand-offs, and board components.
2. Perform a power spectral density (PSD) random vibration analysis.
3. Evaluate the PCB and component integrity based on the PSD response.
The main highlights, and some common practices, for performing these tasks will be briefly described.
PCBs can be very complex structures, usually consisting of a stack of layers of FR4 glass epoxy and copper foil, with vias connecting conductors between different layers. As described in Part 1 of this series, there are several approaches to modeling the board, and any of these approaches can be used in a random vibration analysis. However, the mapped material approach represents the best mix of accuracy and efficiency. This material mapping requires a fine, three-dimensional mesh to model the distribution of all of the details in the board. The mapping is automated in some codes, such as ANSYS Mechanical. An example is shown in Figure 1, above.
Stand-offs are the columns that connect the board to the underlying structure. The board is typically screwed down to the stand-offs. It is typical to model the stand-offs with solid elements. The screws can be modeled with a simplified connection, such as stiff beams. The key is the ability to extract axial and shear forces at these support locations.
Depending on the structure to which the PCB attaches, the opposite end of the stand-offs can be either fixed, or they can be connected to the underlying structure which, at least partly, is included in the finite element model. The approach taken depends on the flexibility of the underlying structure.
Since there can be a large number of components on the board, it is typical to identify a few critical components that will be modeled with solid elements. Critical components are those with large mass or stiffness, or a large footprint. The less critical components are modeled using discreet mass elements, and the remaining components not included in the model. However, since this is a dynamic analysis, the mass properties must be accurately represented. Therefore, the mass of the missing components can be accounted for by increasing the density of the PCB, so that it has the correct mass and center of gravity. The details of the attachment of the critical components to the board are generally not modeled, unless very high accuracy is necessary. They are generally considered rigidly attached to the board. Figure 2 shows a critical component modeled explicitly, and other components represented by point masses.
Figure 2: Components Modeled Explicitly and with Point Masses
Random Vibration Analysis
If a mode superposition approach is used, the analysis procedure starts with a modal analysis to determine the natural frequencies and mode shapes, as well as to supply the dynamic characteristics of the structure to the PSD analysis. The frequency range for mode extraction should be approximately twice the highest frequency for the applied excitation in the subsequent PSD analysis.
The participation factor calculation from the modal analysis should be reviewed to ensure that the ratio of the effective mass to the total mass is close to one in each direction of subsequent excitation (X, Y and Z). A general guideline is to assume that values greater than 0.90 are considered adequate for most applications. Mode shapes should be reviewed to verify expected response.
The PSD input in terms of frequency versus load must be defined. In most cases, the loading is described in terms of a base acceleration. International and company standards exist that represent the vibration requirement the structure must meet. Verification of the loading units should always be made. An example of a standard PSD input spectrum taken from International Standard IEC 60068-2-64 is shown in Figure 3. This standard was developed to evaluate harmonic loading generated by rotating, pulsating or oscillating forces that occur in ships, aircraft, land vehicles, rotorcraft and space applications or caused by machinery and seismic phenomena.
Damping plays a critical role in the response and it is important to define accurate values for the damping ratio, which may be a function of frequency. If damping is not known, a low value will produce conservative results.
Figure 3: PSD Spectrum Input
Evaluation of Structural Integrity
Since the PSD analysis predicts the random vibration response of the structure, the results will be in terms of probability of occurrence. It is typical to use 3-sigma probabilistic response for all PSD result quantities. 3-sigma represents a 99.7% probability that the result will be at or below this value if the loading is described by a normal (Gaussian) distribution.
The weakest link and most likely failure that would be expected in PCBs subjected to vibration loads would be the connection of the components to the board. If these fail, the operational electrical function of the board will be compromised. A popular electronic component life prediction method is by Steinberg, which states that components can be expected to achieve a fatigue life of approximately 20 million stress reversals in a random vibration environment if the displacement at the center of a perimeter-supported board is limited to the value Z:
B = length of PCB edge parallel to component (inch)
L = length of electronic component (inch)
h = height or thickness of PCB (inch)
C = constant for different types of electronic components
r = relative position factor
Constant C is a factor based on the type of electronic component being evaluated, with the table below containing values to use in the expression for Z.
Constant r is the relative position factor, defined as follows:
r = 1.0 represents the center location.
r = 0.707 represents a location toward the center of an edge.
r = 0.5 represents a corner location.
Once Z is calculated, the 3-sigma displacement at the center of the board can be obtained and compared to Z to assess the fatigue life. If the 3-sigma displacement is less than Z, the component is expected to achieve at least 20 million cycles.
This approach to component prediction is very basic, and there are others which introduce more complexity and accuracy. Which one is used depends on the level of accuracy and safety margins required. In any case, Z can be used to help identify the candidate components for more detailed modeling efforts.
If the mapped material approach was used to model the board, 3-sigma stresses can be extracted directly from the board and compared with endurance limits for board materials to assess fatigue life of the board itself. A relatively fine mesh along with the mapped material properties will provide a reasonable prediction of the nominal stresses in the board layers, since the mapping can be used to determine areas of FR4 and copper as opposed to a smeared or lumped property approach. Figure 4 contains a stress contour of a board. The maximum stress location can be compared to the material map to determine the material in which this stress exists.
Figure 4: Stress Contour of Layer of Board
3-sigma axial and shear forces can also be extracted at the stand-off connections and compared to the axial and shear capability of the screws to evaluate the response at these connection points.
If you would like to discuss how you perform vibration analysis of your PCBs, please add a comment below. Look for Part 4 of this series on shock analysis of PCBs, coming soon!
 Steinberg, D. S., Vibration Analysis for Electronic Equipment, 2nd Edition, John Wiley & Sons, Inc., (1988), Eqn. 8.50.
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Peter Barrett
- Engineering Consulting
- ANSYS Software & Support
- ANSYS Training
- About Us
- News & Insights
1579 Straits Turnpike Suite 2B
Middlebury, CT 06762
- ANSYS Software