Why does the prestress from Static analysis does not add up to the stress in Random Vibration analys
PSD stresses are statistical and reported as standard deviations from a zero mean (always positive numbers). These stresses take into account stiffening effects of a pre-stress analysis, but are themselves simply statistical deviations from a zero mean.
On a component-by-component basis you can add or subtract PSD stress values to component values from your pre-stress to find the 'worst case' max/min stress that can occur in that component. This can be thought of as rigidly shifting the stress distribution reported by the PSD run away from its zero mean.
You cannot simply use the Von Mises Equivalent Stress equation to calculate PSD equivalent stresses, as that algebraic equation is not mathematically suited for statistical values. If you want to Superpose Random Vibe Stress with Static Structural then there are a couple of points for your consideration on this issue:
The default output from a Random Vibration analysis will be 1-sigma values (i.e., standard deviations about a zero mean). Therefore, we have a Gaussian distribution of stress at each node. If you have pre-stressed the modal analysis, then the effect of the static loading is accounted for in the stiffness that is used to determine the natural frequencies. This consequently filters down into the PSD analysis.
You could add/subtract the 1-sigma component value (i.e., Normal Stress in X, Y, and Z) at each node to/from the static analysis to get a sense for the 1-sigma variation of the component stresses about that mean value. This would be the same as rigidly shifting the Gaussian distribution from zero mean to be centered about the static condition. There will not be a way to directly plot contours like this in ANSYS Mechanical. However, I can think of one possible workaround:
Right Click on the PSD result and select Export. This will give you a text file containing stress at each node. It will also contain the X, Y, and Z coordinates of the nodes if you have specified this on Tools > Options > Mechanical > Export > Include Node Location.
Repeat this process for the Static result
Add and subtract appropriately to get the min/max values in Excel
Save separate Text files with the Node locations and Min/Max values
Read in the Text Files using External Data in ANSYS Workbench. Make sure to specify the appropriate column data, especially Stress (and units!)
Link the External Data cell to the Setup of a duplicate Static Structural
Right Click on the Imported Load folder in ANSYS Mechanical and specify 'Initial Stress'
Specify 'Apply To' > Corner Nodes and 'Component' > Desired Component
ANSYS Mechanical will then try to map the stress to the duplicated mesh. The result should be an Imported Initial Stress that really is the combination of your static and PSD results.