Learning Forum

[SaurabhG]

What would be the best way to simulate the model for vibrational analysis of a PCB given that the I have the empirical data from the vibration bench with known frequencies and velocities as outputs.n

[peteroznewman]

nIt depends on the questions you want the model to answer. Below describes the simplest model.nCreate a surface model of the outline of the PCB. Cut out of that surface the holes that support the PCB and the outline of any large components. Fill in the holes of the large components with new surfaces. That allows you to assign a material and thickness to the PCB board while assigning a different material and thickness to the large components, which are much stiffer than the PCB. Use the Share button in SpaceClaim to have the mesh connect the component edges to the PBC edges.nAdjust the density of each large component so the mass equals the measured (or published) mass of that component. nDon't bother to represent all the tiny components, simply adjust the density of the PCB until the total mass of the model equals the measured mass of the populated board, smearing the mass of the tiny components across the whole PCB.nAdd Fixed Supports to the support holes.nRun a Modal analysis. You should see the measured frequencies show up in the simulation results.n

[SaurabhG]

Thankyou for your reply . I did reach this stage of analysis. Rephrasing my question to be precise. I have an actual data that is collected from the vibrational test bench which was excited at 2g velocity and frequencies ranging 20 Hz to 2000 Hz sweep. I want to know what should be my inputs for FEA analysis so as to replicate this empirical test to get similar results to know exact stress points on the PCB for further design evaluations. Appreciate your help. Thanks. n

[peteroznewman]

nIt would have saved me some time if you had asked the question more precisely in the beginning.n2g is an acceleration, not a velocity. Please be more precise about the inputs to your experiment.nShow the results from your experiment.n

[SaurabhG]

Thankyou for your help and correcting me. I apologize for not being specific earlier. Following is the experiment,nn

[peteroznewman]

nThe experimental data should have provided data on Damping in the PCB. You need to know that.nDid you slice up the surface of the pcb to put a vertex at each of the 10 locations on the PCB? Do that.nUse a Modal Analysis and reply with the Mass Participation table for modes up to 3000 Hz.nDrag a Harmonic Response and drop it on the Solution cell of the Modal Analysis.nOpen the Model, add an Inertial Load of Acceleration. What axis is normal to the PCB? Assuming it is the Y axis, use 2*9806.6 mm/s^2 for the acceleration in the Y component.nUnder Analysis Settings, Damping Controls, enter the Damping measured in the experiment. The simulation results are strongly dependent on the correct value of damping. nSet the Start and End Frequency for the sweep to 20 - 2500 Hz. Turn on User Defined Frequencies and enter all the specific frequencies that are listed in your table plus some extras.nInsert a Frequency Response on each of the the 10 points, Type = Directional Acceleration. Orientation = Y axis.nRepeat but use Type = Directional Velocity.n

[SaurabhG]

Thankyou for your response. nI am getting following mass participation:nAlso, the experimental system did not use any external damping values. There was direct input at the base. All the damping may have been from fixtures if at all any. Apparently it may be safe to assume damping between 1 - 5.nI did try harmonic response analysis as per your instructions with damping ratio 1 - 5, but I am not getting results close to empirical data. nPlease let me know if possible which parameters need to be tweaked. nThan you. n

[peteroznewman]

nYou need many more modes than two. You want to see the cumulative mass participation above 90% for all directions.nThe shaker table instrumentation can measure internal damping in the structure. I'm not talking about external damping.n