Learning Forum

[peteroznewman]

Aerospace structures often have a minimum first natural frequency requirement, as well as a maximum mass requirement. Suppose a modal analysis of the inital design predicts that the first natural frequency is below the minimum requirement and the mass of the inital design is at the maximum. The structure needs a design iteration. 

Structures are made up of components. Some components need to get stiffer, which usually adds mass, while other components need to reduce mass. A Modal Energy Analysis is the recommended method to choose which component to focus the redesign effort on.  This consists of computing the Strain Energy and Kinetic Energy in each component. The component with the highest Strain Energy in Mode 1 is the redesign candidate to increase stiffness and accept some additonal mass.  The component with the highest Kinetic Energy in Mode 1 is the redesign candidate to reduce mass. The analysis provides a weighted ranking of the importance of each component for its contribution to the Strain Energy and Kinetic Energy for each mode. If two components have a similar contribution, both can be examined for potential redesign. 

A simple tutorial example shows a structure with four bodies (components).

In Mechanical, if we turn on Volume and Energy Output, we can plot the Strain energy in each element using a User Defined Result and type in the expression ENERGYPOTENTIAL which will show where the highest strain energy is, but it doesn't sum up all the elements in each body.

APDL code in a Command object is used in the Solution branch of the outline to sum the energies in each body and write that data to a text file. The script requires that each solid body be named Body1, Body2, Body3, etc. The APDL code will access each body by name.

Here is the APDL code:

/sys,del energy.out
*cfopen,energy,out
*vwrite,'MODE', 'SENE', 'KENE', 'BODY'
 (A,A,A,A)
*cfclos
resume

*do,iii,1,4,1
cmsel,s,body%iii%

*do,jjj,1,6
  set,1,jjj
  etab,sene,sene
  etab,kene,kene
  ssum
  *get,sene1,ssum,,ITEM,sene
  *get,kene1,ssum,,ITEM,kene
  *cfopen,energy,out,,APPEND
  *vwrite,jjj,sene1,kene1,iii
  (F4.0,2E12.4,F5.0)
  *cfclose
*enddo
*enddo

I used Excel to plot the data in the text file that this code produces.

The results tell you what to do, increase the stiffness of Body 2 and 1, reduce the mass of Body 3 and 4. You may not have needed this method to tell you that, because this is such a simple structure. But when the design has a realistic amount of complexity, it may not be obvious which component is the largest contributor to Strain Energy and Kinetic Energy.

This tutorial serves as an introduction to the topic since it only deals with the strain energy in solid elements. If a structural model includes spring elements, the strain energy in those must be included. An excellent article provides the APDL code to account for the energy in other types of elements.

I made two videos that shows how to use the APDL code and how to use Excel to plot those graphs. They are in the replies below. Here is a link to the ANSYS2022 R2 archive.

[peteroznewman]

https://www.youtube.com/watch?v=sFNGXjlnIFQ

[peteroznewman]

https://www.youtube.com/watch?v=2xJWO3F6i7c