Help w/ PSD Analysis

[Stringmaker]

Hi everyone,
I'm Brian, first time poster long time reader. I've used Ansys and various other FEA codes a fair amount. Most of my background is static stress and thermal and good results have always been obtained easily in the past.

I've been tasked to do a spectral (random vibration analysis) of several circuit boards. So far I've modeled them CB with shell93 elements, fixed nodes where the board solders to the base, and am using lumped masses to imitate where wires solder into the board. I've ran through a tutorial in the Ansys documentation which uses a beam, single point response, in seismic displacement loading and have tried applying this example to my analysis without luck. My problem is that I get stresses and displacements that are on the order of 3-4 orders of magnitude higher than one would expect. I've double and triple checked material properties and have been beating my head trying to figure out why i'm receiving what appear to be bad results. Here's what I have and the procedure which I've been using:

PSD function is g^2/Hz acceleration on Y-axis vs. Frequency on X-axis.

Hz g^2/Hz
20 .013
30 .028
150 .028
300 .0014
1000 .0014
2000 .00035

Here's the procedure I've been using to do the analysis:
1) New Analysis: Modal analysis using Block Lanczos method, calc 25 modes and expand 25 modes, calc element results. Solve.
2) New Analysis: Spectrum analysis, Single Point Response
3) Settings: PSD, scale factor is 1, direction is 0, 0, 1
4) Graph frequencies and psd values. Solve
5) New Analysis: Modal, Expansion Pass
6) Solution -> Spectrum -> Single Point -> Expansion Pass
7) NMODES=25, FREQB=0, FREQE=2000, yes to calc elem results, SIGNIF=0.001
8) Solve
9) New Analysis: Spectrum, Single Point Response
10) Solution -> LSO -> Spectrum -> Single Point -> Mode Combine
11) SRSS Method, SIGNIF=0.001
12) Displacement is selected in the Mode Combinations Method dialog box
13) Solve
14) Read Input From -> select the .mcom file
15) In /Post1 there are three modes which have a signif equal to or higher than 0.001. They are 114 Hz, 607 Hz, and 1460 Hz.

When I select any one of these frequencies, read the results, and look at both nodal and element solutions for displacement and principal stresses this is when I get the weird results. If you could provide any sort of feedback I would be very grateful!

I know that 1 sigma stresses are typically used for evaluation in these types of analyses. Could I be looking at the wrong stress?

Thank you all!

-Brian

 

[Drej]

Although you've made an excellent attempt at trying to explain what you're doing/have done (well done!), it's pretty difficult still to understand where things are going wrong. This is no surprise as PSD is a pretty complicated type of analysis to carry out, especially in ANSYS. It is my guess, however, that you are becoming confused by the seismic/PSD approaches in the FE code. Stage (10) in your list shows:

10) Solution -> LSO -> Spectrum -> Single Point -> Mode Combine

For modal combination in PSD analyses you should use the PSDCOM command, accessed via:

Main Menu>Preprocessor>Loads>Load Step Opts>Spectrum>PSD>Mode Combine
or
Main Menu>Solution>Load Step Opts>Spectrum>PSD>Mode Combine

You should also not read in the mcom file, as this operation is carried out when you issue the PSDCOM command. Below is an extract from the help file:

6.7.3. Combine the Modes

Only the PSD mode combination method is valid in a random vibration analysis. This method triggers calculation of the one-sigma displacements, stresses, etc., in the structure. If you do not issue the PSDCOM command, the program does not calculate the one-sigma response of the structure.

Command(s): PSDCOM
GUI: Main Menu> Solution> Load Step Opts> Spectrum> PSD> Mode Combin

The SIGNIF and COMODE fields on the PSD mode combination method [PSDCOM] offer options to reduce the number of modes to be combined (see the description of PSDCOM command). If you want to exercise these options, it is prudent to print the modal covariance matrices in Obtain the Spectrum Solution to first investigate the relative contributions of the modes toward the final solution.

Have a good read though the whole of the section "Structural Guide> Chapter 6. Spectrum Analysis>
6.7. How to Do a Random Vibration (PSD) Analysis" which should point you in the right direction.

Also, take a look here at an example PSD input.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Stringmaker]

Thanks Drej! I'm on the road to success now. I saw this example before and went through the steps even to no avail. Apparently, at the time of my posting this the only thing I can think is that I wasn't reading the appropriate load step hence my weird results. The results I have now look much much better! Again...thank you!

Best,
-Brian