I'm simulating the deformation of an unusually shaped pressure vessel. The deformed shape is somewhat complicated; is there a way to compute the change of volume enclosed in the model or otherwise get some kind of profile of the deformed surface?
Thanks so much!
Solved! Go to Solution.
Yes there is a way. The basic steps are to create a new model of the displaced shape ("Results Options > Other > Tools > Make FEM"), and then calculate the volume of the new model ("Analysis > Analysis > Weight and Center of Gravity").
Here are the details.
- Fill the tank with a new part, representing the volume of the tank, and give weak material properties for this volume. You will use this part to calculate the volume as it moves along with the tank walls, but you do not want it to affect the displacement of the tank.
- Perform the stress analysis as usual.
- In the Results environment, you must set the displacement scale factor to an absolute value of 1. ("Results Contours > Displacement > Show Displaced > Displaced Options", make sure "Show Displaced Model" is checked and "Scale Facotr > As an Absolute Value" is chosen and set to 1.)
- Hide all of the parts except for the volume part.
- Display the internal mesh since this is off by default. ("Results Options > View > Show Internal Mesh".)
- Export the displaced volume to a new model ("Results Options > Other > Tools > Make FEM")
- Open the new model, assign any material properties, and do "Analysis > Analysis > Check Model".
- Calculate the volume with "Analysis > Analysis > Weight and Center of Gravity".
You should calculate the original volume with the Weight and Center of Gravity calculator also.
John Holtz, P.E.
Senior User Experience Designer, Simulation
Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)