Frequency Spectrum

Limitations

Currently frequency responses are allowed only for sizing optimization.

Options in Context of Frequency Response

The following lists which options can be applied in frequency response optimization using Tosca Structure and Abaqus:

• The following types of analysis are supported in Abaqus:
  • *STEADY STATE DYNAMICS, DIRECT
  • *STEADY STATE DYNAMICS, SUBSPACE PROJECTION
  • *STEADY STATE DYNAMICS
  (The modal superposition is used in Abaqus when DIRECT or SUBSPACE PROJECTION is not defined.)
• The excitation frequencies should always stay constant during the optimization iterations. Consequently, the locations of the excitation frequencies determined from the eigenfrequencies (an option in modal analysis) are prohibited. The following ways of defining excitation frequencies exist in Abaqus:
  • For DIRECT and analysis SUBSPACE PROJECTION:
    • INTERVAL=RANGE is allowed (default for DIRECT).
    • INTERVAL=EIGENFREQUENCY is not allowed (default for SUBSPACE PROJECTION).
  • Modal analysis:
    • INTERVAL=RANGE is allowed.
    • INTERVAL=EIGENFREQUENCY is allowed.

  Warning: INTERVAL=EIGENFREQUENCY should be used with caution because eigenvalues change during optimization.

  Important: It is strongly recommended that load cases in *STEADY STATE DYNAMICS, DIRECT are defined in Abaqus using the command *LOADCASE. Using *LOADCASE leads to a significant reduction of the CPU-time for the optimization executions.

• When *STEADY STATE DYNAMICS, DIRECT is applied, all requests that Tosca Structure requires from Abaqus for the optimization are not available from the *STEP containing *STEADY STATE DYNAMICS, DIRECT. However, these can be requested in the eigenfrequency extraction analysis. Consequently, an eigenfrequency extraction (modal analysis) should always be applied before the STEADY STATE DYNAMICS, DIRECT analysis. This can be done without much CPU effort by defining the following as the first *STEP in the Abaqus finite element input file:

  
  *STEP
  *FREQUENCY, EIGENSOLVER=LANCZOS, NORMALIZATION=MASS
  1, 0.0, ,
  *END STEP
  
  

• Only pure linear frequency responses are supported. Thus, no prestress (stress stiffening) before the frequency is allowed.
• The normalization option MASS will be used by default. It will be set automatically regardless of the original option.
• Prescribed displacements, velocities, and accelerations for Abaqus are supported in frequency response using the command *BOUNDARY including one or several of the following arguments:

  
  TYPE=DISPLACEMENT
  TYPE=VELOCITY
  TYPE=ACCELERATION
  
  

  Other types of prescribed displacements, velocities, and accelerations for Abaqus are not supported for frequency response.
• The geometric nonlinearities and the incompatible, modified, and hybrid elements are not supported as design elements (DV_TOPO) for frequency response. Elements, which are allowed as design elements (DV_TOPO) in frequency response, are marked with an ’F’ in the table of supported element types ( Supported Element Types), but all other elements are allowed outside the design area.

Damping

The following lists the options to deal with dumping:

• For DIRECT and analysis SUBSPACE PROJECTION:
  • Raleigh damping (viscous damping) defined by *DAMPING, ALPHA=$\alpha$ and *DAMPING, BETA=$\beta$. These should also be defined using OPT_PARAM for the design elements:

    
    OPT_PARAM 
     ... 
     DAMP_VISCOUS_MASS  = $\alpha$ 
     DAMP_VISCOUS_STIFF = $\beta$ 
     ...
    END_
    
    

  • Structural damping defined by *DAMPING, STRUCTURAL=${\beta }_{\mathrm{\Omega }}$ in the *MATERIAL command is supported. The damping should also be defined using OPT_PARAM for the design elements yielding:

    
    OPT_PARAM 
     ... 
     DAMP_STRUCTURAL_STIFF = ${\beta }_{\mathrm{\Omega }}$
     ...
    END_
    
    

    Even though several different materials with different Young modulus and density can be applied in the design area, the structural damping of all elements in the design area must be the same.
• For modal superposition procedures:
  • Critical damping defined using *MODAL DAMPING, MODAL DIRECT depending on the eigenfrequencies is not allowed. During the designing the eigenfrequencies change significantly and, thus, the modal damping will also change significantly.
  • Rayleigh damping (viscous damping) defined using *MODAL DAMPING, RAYLEIGH, DEFINITION=FREQUENCY RANGE is allowed when all modes are included and all modes have the same damping. For example:

    1e-20,$\alpha$,$\beta$

    1e+20,$\alpha$,$\beta$

    where $\alpha$ and $\beta$ must be the same in the two lines ensuring that the Rayleigh damping is constant in the entire range. The damping should also be defined using OPT_PARAM for the design elements:

    
    OPT_PARAM 
     ... 
     DAMP_VISCOUS_MASS  = $\alpha$
     DAMP_VISCOUS_STIFF = $\beta$
     ...
    END_
    
    

    DEFINITION=MODE NUMBERS can also be applied if all modes are included with the same damping and defined in OPT_PARAM.
  • Structural damping defined using *MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE is allowed when all modes are included and all modes have the same damping. For example:

    1e-20,${\beta }_{\mathrm{\Omega }}$

    1e+20, ${\beta }_{\mathrm{\Omega }}$

    where ${\beta }_{\mathrm{\Omega }}$ must be the same in the two lines ensuring that the structural damping is constant in the entire range. The damping should also be defined using OPT_PARAM for the design elements:

    
    OPT_PARAM 
     ... 
     DAMP_STRUCTURAL_STIFF = ${\beta }_{\mathrm{\Omega }}$
     ...
    END_
    
    

  • The DEFINITION=MODE NUMBERS call also be applied if all modes are included with the same damping and defined in OPT_PARAM.

  Important: Use the SIM architecture of the solver to take the present structural damping effect into account.