<?xml version='1.0' encoding='UTF-8' ?>
<!DOCTYPE html
  SYSTEM "about:legacy-compat">
<html xmlns:mml = "http://www.w3.org/1998/Math/MathML" lang = "en"><head><meta charset = "UTF-8"/><meta name = "copyright" content = "(C) Copyright 2020"/><meta name = "DC.rights.owner" content = "(C) Copyright 2020"/><meta name = "DC.type" content = "concept"/><meta name = "abstract" content = "Frequency responses can be obtained in several ways in Abaqus. They are discussed within this section."/><meta name = "description" content = "Frequency responses can be obtained in several ways in Abaqus. They are discussed within this section."/><meta name = "DC.format" content = "HTML5"/><meta name = "DC.identifier" content = "tso-c-usr-solver-abaqus-freqspec"/><meta name = "DC.language" content = "en"/><link rel = "stylesheet" type = "text/css" href = "../DSDocUI_XML34.css"/><title>Frequency Spectrum</title>
<script type = "text/javascript" src = "../DSDocUI_Highlight34.js">
  	/* */
  	</script><script type = "text/javascript" src = "../MathJax/MathJax.js?config=DS-default,local/local">
  		/* */
  		</script></head><body onLoad = "highlightSearchTerms();" id = "tso-c-usr-solver-abaqus-freqspec">
<a name = "hj-top"> </a><table class = "table1" id = "table11"><tr><td><table class = "DocHeader"><tr><td class = "DocHeader1" colspan = "2"><h1>Frequency Spectrum</h1></td></tr><tr><td class = "DocHeader4" colspan = "2"/></tr><tr><td class = "DocHeader3" colspan = "2"><table class = "DocThemeIntro" id = "table12"><tr><td class = "Intro1Only"><p class = "header"><p class = "abstract"> 
<span class = "shortdesc"> Frequency responses can be obtained in several ways in 
<span class = "ph">Abaqus</span>.
They are discussed within this section.
</span>
 
</p>
<p>This page discusses: </p><ul><li><a href = "#tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-limitations" id = "toc_rg" title = "">Limitations</a></li><li><a href = "#tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-options" id = "toc_rg" title = "">Options in Context of Frequency Response</a></li><li><a href = "#tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-damping" id = "toc_rg" title = "">Damping</a></li></ul>
</p></td></tr></table></td></tr></table>


 
 
<div class = "body conbody"> 

<div class = "section" id = "tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-limitations"><h2 class = "title sectiontitle">Limitations</h2> 
 
<p>Currently frequency responses are allowed only for sizing
optimization.</p> 
</div>
 

<div class = "section" id = "tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-options"><p><map name = "FPMap1"><area href = "#hj-top" title = "Back to Top" shape = "rect" coords = "416, 0, 435, 10"/></map><span class = "itemsprite"/></p><h2 class = "title sectiontitle">Options in Context of Frequency Response</h2> 
 
<p>The following lists which options can be applied in frequency response optimization using <span class = "ph">Tosca Structure</span> and <span class = "ph">Abaqus</span>:</p> 
<ul class = "ul"> 
<li class = "li">The following types of analysis are supported in 
<span class = "ph">Abaqus</span>:
       
<ul class = "ul"> 
<li class = "li"><code class = "ph codeph">*STEADY STATE DYNAMICS, DIRECT</code></li> 
<li class = "li"><code class = "ph codeph">*STEADY STATE DYNAMICS, SUBSPACE PROJECTION</code></li> 
<li class = "li"><code class = "ph codeph">*STEADY STATE DYNAMICS</code></li> 
</ul> (The modal superposition is used in 
<span class = "ph">Abaqus</span>
when <code class = "ph codeph">DIRECT</code> or <code class = "ph codeph">SUBSPACE PROJECTION</code> is not defined.) </li> 
<li class = "li">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 
<span class = "ph">Abaqus</span>:
       
<ul class = "ul"> 
<li class = "li">For <code class = "ph codeph">DIRECT</code> and analysis <code class = "ph codeph">SUBSPACE PROJECTION</code>: 
<ul class = "ul"> 
<li class = "li"><code class = "ph codeph">INTERVAL=RANGE</code> is allowed (default for <code class = "ph codeph">DIRECT</code>).</li> 
<li class = "li"><code class = "ph codeph">INTERVAL=EIGENFREQUENCY</code> is not allowed (default for <code class = "ph codeph">SUBSPACE PROJECTION</code>).</li> 
</ul> 
</li> 
<li class = "li">Modal analysis: 
<ul class = "ul"> 
<li class = "li"><code class = "ph codeph">INTERVAL=RANGE</code> is allowed.</li> 
<li class = "li"><code class = "ph codeph">INTERVAL=EIGENFREQUENCY</code> is allowed.</li> 
</ul> 
</li> 
</ul> 
<p><table class = "Remark" id = "table132"><tr><td class = "Remark"><span class = "run-in.warning">Warning:
				</span><span class = "notecontent"><code class = "ph codeph">INTERVAL=EIGENFREQUENCY</code>
should be used with caution because eigenvalues change during optimization.
</span></td></tr></table>
</p>
<p><table class = "Remark" id = "table132"><tr><td class = "Remark"><span class = "run-in.important">Important:
				</span><span class = "notecontent">It is strongly recommended that <span class = "ph">load cases</span>
in <code class = "ph codeph">*STEADY STATE DYNAMICS, DIRECT</code> are defined in
<span class = "ph">Abaqus</span> using the command 
<code class = "ph codeph">*LOADCASE</code>. Using <code class = "ph codeph">*LOADCASE</code> leads to a significant reduction of
the CPU-time for the optimization executions.</span></td></tr></table>

</p>
</li> 
<li class = "li">When <code class = "ph codeph">*STEADY STATE DYNAMICS, DIRECT</code> is applied, all
requests that <span class = "ph">Tosca Structure</span>
requires from <span class = "ph">Abaqus</span>
for the optimization are not available from the <code class = "ph codeph">*STEP</code> containing 
<code class = "ph codeph">*STEADY STATE DYNAMICS, DIRECT</code>. However, these can
be requested in the eigenfrequency extraction analysis. Consequently, an
eigenfrequency extraction (modal analysis) should always be applied before the 
<code class = "ph codeph">STEADY STATE DYNAMICS, DIRECT</code> analysis. This can be
done without much CPU effort by defining the following as the first 
<code class = "ph codeph">*STEP</code> in the <span class = "ph">Abaqus</span> finite element input file: 
<pre class = "codeblock">
<code class = "ph codeph">
*STEP
*FREQUENCY, EIGENSOLVER=LANCZOS, NORMALIZATION=MASS
1, 0.0, ,
*END STEP
</code>
</pre> 
</li> 
<li class = "li">Only pure linear frequency responses are supported. Thus, no
prestress (stress stiffening) before the frequency is allowed.</li> 
<li class = "li">The normalization option 
<code class = "ph codeph">MASS</code> will be used by default. It will be set
automatically regardless of the original option.</li> 
<li class = "li">Prescribed displacements, velocities, and accelerations for 
<span class = "ph">Abaqus</span>
are supported in frequency response using the command 
<code class = "ph codeph">*BOUNDARY</code> including one or several of the following
arguments: 
<pre class = "codeblock">
<code class = "ph codeph">
TYPE=DISPLACEMENT
TYPE=VELOCITY
TYPE=ACCELERATION
</code>
</pre> 
Other types of prescribed displacements, velocities, and
accelerations for <span class = "ph">Abaqus</span> are not supported for frequency response. </li> 
<li class = "li">The geometric nonlinearities and the incompatible, modified, and hybrid elements are not
     supported as design elements (<code class = "ph codeph">DV_TOPO</code>) for frequency response. Elements, which
     are allowed as design elements (<code class = "ph codeph">DV_TOPO</code>) in frequency response, are marked
     with an ’F’ in the table of supported element types ( <a class = "xref" href = "tso-c-usr-solver-abaqus-elements.htm#tso-c-usr-solver-abaqus-elements" title = "The analysis model can contain arbitrary element types, but not all element types can be used in the design area. In addition, for the definition of restriction areas only certain element types are permitted. All other elements in the analysis model are considered as dummy elements in the optimization; for example, the elements not changed during the optimization process.">Supported Element Types</a>), but all other elements are allowed outside the design area. </li> 
</ul> 
</div>
 

<div class = "section" id = "tso-c-usr-solver-abaqus-freqspec__tso-c-usr-solver-abaqus-freqspec-damping"><p><map name = "FPMap1"><area href = "#hj-top" title = "Back to Top" shape = "rect" coords = "416, 0, 435, 10"/></map><span class = "itemsprite"/></p><h2 class = "title sectiontitle">Damping</h2> 
 
<p>The following lists the options to deal with dumping:
</p> 
<ul class = "ul"> 
<li class = "li">For <code class = "ph codeph">DIRECT</code> and analysis <code class = "ph codeph">SUBSPACE PROJECTION</code>: 
<ul class = "ul"> 
<li class = "li">Raleigh damping (viscous damping) defined by 
<code class = "ph codeph">*DAMPING, ALPHA=<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span></code>
and 
<code class = "ph codeph">*DAMPING, BETA=<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span></code>.
These should also be defined using 
<code class = "ph codeph">OPT_PARAM</code> for the design elements:
<pre class = "codeblock">
<code class = "ph codeph">
OPT_PARAM 
 ... 
 DAMP_VISCOUS_MASS  = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span> 
 DAMP_VISCOUS_STIFF = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span> 
 ...
END_
</code>
</pre>
</li> 
<li class = "li">Structural damping defined by 
<code class = "ph codeph">*DAMPING, STRUCTURAL=<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span></code>
in the 
<code class = "ph codeph">*MATERIAL</code> command is supported. The damping
should also be defined using 
<code class = "ph codeph">OPT_PARAM</code> for the design elements yielding: 
<pre class = "codeblock">
<code class = "ph codeph">
OPT_PARAM 
 ... 
 DAMP_STRUCTURAL_STIFF = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span>
 ...
END_
</code>
</pre>
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. </li> 
</ul> </li> 
<li class = "li">For modal superposition procedures: 
<ul class = "ul"> 
<li class = "li">Critical damping defined using <code class = "ph codeph">*MODAL DAMPING, MODAL DIRECT</code> depending
on the eigenfrequencies is not allowed. During the designing the eigenfrequencies
change significantly and, thus, the modal damping will also change significantly. </li> 
<li class = "li">Rayleigh damping (viscous damping) defined using 
<code class = "ph codeph">*MODAL DAMPING, RAYLEIGH, DEFINITION=FREQUENCY
RANGE</code> is allowed when all modes are included and all modes have the
same damping. For example: 
<p><code class = "ph codeph">1e-20,<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span>,<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span></code></p> 
<p><code class = "ph codeph">1e+20,<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span>,<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span></code></p> 
where <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span>
and <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span>
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 
<code class = "ph codeph">OPT_PARAM</code> for the design elements: 
<pre class = "codeblock">
<code class = "ph codeph">
OPT_PARAM 
 ... 
 DAMP_VISCOUS_MASS  = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">α</mi></mrow></math></span>
 DAMP_VISCOUS_STIFF = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow></math></span>
 ...
END_
</code>
</pre>

<code class = "ph codeph">DEFINITION=MODE NUMBERS</code> can also be applied if
all modes are included with the same damping and defined in 
<code class = "ph codeph">OPT_PARAM</code>. </li> 
<li class = "li">Structural damping defined using 
<code class = "ph codeph">*MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY
RANGE</code> is allowed when all modes are included and all modes have the
same damping. For example: 
<p><code class = "ph codeph">1e-20,<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span></code></p> 
<p><code class = "ph codeph">1e+20,
<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span></code></p>
where 
<span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span>
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 
<code class = "ph codeph">OPT_PARAM</code> for the design elements: 
<pre class = "codeblock">
<code class = "ph codeph">
OPT_PARAM 
 ... 
 DAMP_STRUCTURAL_STIFF = <span class = "ph inlineequation"><math class = "- topic/foreign "><mrow class = "- topic/foreign "><msub class = "- topic/foreign "><mrow class = "- topic/foreign "><mi class = "- topic/foreign ">β</mi></mrow><mrow class = "- topic/foreign "><mi mathvariant = "normal" class = "- topic/foreign ">Ω</mi></mrow></msub></mrow></math></span>
 ...
END_
</code>
</pre>
</li> 
<li class = "li">The <code class = "ph codeph">DEFINITION=MODE NUMBERS</code> call also be applied if
all modes are included with the same damping and defined in 
<code class = "ph codeph">OPT_PARAM</code>.</li>
</ul> 
<p>
<table class = "Remark" id = "table132"><tr><td class = "Remark"><span class = "run-in.important">Important:
				</span><span class = "notecontent">Use the SIM architecture of the solver to take the present structural damping effect into account.</span></td></tr></table>

</p>
</li> 
</ul> 
</div>
 
</div>
 
</td></tr></table><script type = "text/javascript" src = "../DSDocUI_Bottom34.js">/* */</script></body>
</html>
