Knowledgebase
Knowledgebase:
Nastrran in CAD - How to setup a vibration fatigue
Posted by Florian Neumayr on 24 March 2020 04:42 PM

HOW TO - Nastran in CAD

Based on reoccurring questions in Kayako: How to setup a fatigue analysis and where to get the material data from?

ANSWER:

Static vs. Dynamic Fatigue

  • Static fatigue analysis explores the accumulation of damage in a part or assembly based on a single or sequence of stress states with a defined number of cycles for each. This can be accomplished outside of FEA for simple load scenarios
  • Finite Element based static fatigue in Autodesk Nastran In-CAD can factor in multi-axial effects of complex
  • However, when the load input is a PSD curve, static cases don’t exist, and a different approach is
  • Random Vibration Fatigue in Autodesk Nastran In-CAD can provide insight on this type of

Setup the Vibration Fatigue Analysis

20h vibration against gravity.

  1. Right click Analysis 1 and choose Edit
  2. Select the Vibration Fatigue analysis type
  3. Make sure Acceleration and Stress are turned on
  4. Click OK
  5. Double click Fatigue Setup 1 in the Model Tree
  6. Make sure the Stress Life approach and Maximum principal method are selected
  7. Enter 20 for the Event Duration
  8. Enter 3600 for the Time Conversion Factor (=3600 sec per hour)
  9. Click OK

Define the Fatigue Properties

  1. Right click Steel, Alloy in the Model Tree and select Edit
  2. Click the Fatigue button
  3. On the S-N tab, enter the following properties:
  4. B = 0.1
  5. Su = 72200
  6. No = 1000
  7. KF = 1
  8. Be = 0.001
  9. Se = 29000
  10. Click OK on both dialogs

For other material data, please refer to: https://www.matdat.com/ for example. A pro-user member ship might be required. Another website is: http://www.matweb.com/.

Define the Dynamic Setup for Example

  1. Right click Dynamic Setup 1 in the Model Tree and choose Edit
  2. Select the Vertical PSD curve
  3. Turn on the Frequency Range check box
  4. Specify 60 Hz as the Lowest Frequency and 1000 Hz as the Highest Frequency
  5. Enter 20 for the Number of Points in the Range
  6. Turn on the Spread around Modes check box and again specify a range from 60 to 1000 Hz spread over 10 points in the range
  7. Enter 5 for the Percentage Spread
  8. Click OK

 

Replace any existing Load with Gravity

  1. Add a standard gravity load in the Y direction (9.81 m/sec2 or 386.4 in/sec2)
  2. Click Run from the Ribbon to start the analysis

 

Review Fatigue Results

  1. Right click the Results in Model Tree and choose Edit
  2. Select RMS Output from the subcase list
  3. Select Fatigue and Shell Max Damage Bottom/Top from the Result Data menu


Comments (0)