<?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 = "Features that are supported by Tosca are considered within this section."/><meta name = "description" content = "Features that are supported by Tosca are considered within this section."/><meta name = "DC.format" content = "HTML5"/><meta name = "DC.identifier" content = "tso-c-usr-solver-abaqus-nonlinguide"/><meta name = "DC.language" content = "en"/><link rel = "stylesheet" type = "text/css" href = "../DSDocUI_XML34.css"/><title>Guide for Nonlinear Models</title>
<script type = "text/javascript" src = "../DSDocUI_Highlight34.js">
  	/* */
  	</script></head><body onLoad = "highlightSearchTerms();" id = "tso-c-usr-solver-abaqus-nonlinguide">
<a name = "hj-top"> </a><table class = "table1" id = "table11"><tr><td><table class = "DocHeader"><tr><td class = "DocHeader1" colspan = "2"><h1>Guide for Nonlinear Models</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">Features that are supported by <span class = "ph">Tosca</span> are considered within this section. </span>

</p>
<p>This page discusses: </p><ul><li><a href = "#tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings" id = "toc_rg" title = "">Solver Settings</a></li><li><a href = "#tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-ErrorMessages" id = "toc_rg" title = "">Error Messages in .msg-files</a></li></ul>
</p></td></tr></table></td></tr></table>




<div class = "body conbody">

<div class = "section" id = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings"><h2 class = "title sectiontitle">Solver Settings</h2>

<p>To obtain better convergence behavior, use the following settings when running an optimization
   with a nonlinear model:</p>
<p><pre class = "codeblock">
*STEP, NLGEOM=YES, INC=10000, extrapolation=NO
** (INC=number of increments)
*STATIC
**(initial, step time, min, max) 
0.1, 1.0, 1e-14, 1.0 
</pre></p>
<p> In the following, <span class = "ph">Abaqus</span> 
    related remarks that should be taken into account when optimizing structures with nonlinear behavior are summarized. </p>
<table class = "table"><caption/><colgroup><col style = "width:50%"/><col style = "width:50%"/></colgroup><thead class = "thead">
<tr class = "row">
<th class = "entry" id = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Topic: </th>
<th class = "entry" id = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> Remark: </th>
</tr>
</thead><tbody class = "tbody">
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Time increment </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> By default, <span class = "ph">Abaqus</span> 
                       uses the automatic time incrementation based on the initial, step time, minimum, and maximum time
                       increments. In the case of a nonlinear analysis,
                       it is recommended to use a small minimum time increment as well as a higher number of increments
                       to run a stable analysis. The following default is the syntax for the 
                       <span class = "ph">Abaqus</span>
                       input file for the respective step. <p>
                       <pre class = "codeblock">
                       *STEP, INC=100
                       ** (INC=increments)
                       *STATIC
                       ** (initial, step time, min, max) 
                       1.0, 1.0, 1e-05, 1.0 
                       </pre>
                       </p> Having a minimum time increment smaller than <code class = "ph codeph">1e-07</code> might further improve the
                       convergence but also strongly increases the computation time. More details can be found in the
                       <span class = "ph">Abaqus</span> documentation. </td>
</tr>
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Element type </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> Based on the utilized integration schemes the element types are split
                       into fully integrated elements like C3D8 or C3D4 and reduced integrated elements like C3D8R. In the
                       case of reduced integration elements in the model, activate the enhanced hourglass technique. The
                       following is the syntax for the <span class = "ph">Abaqus</span> 
                       input file:
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *SECTION CONTROLS, NAME=&lt;SEC NAME&gt;, HOURGLASS = ENHANCED 
                       </code>
                       </pre>
                       </td>
</tr>
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Solver instabilities </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> If the optimization fails because of <span class = "ph">Abaqus</span> 
                       convergence issues, further details can be investigated in the *.msg or *.dat files generated
                       by <span class = "ph">Abaqus</span> in the critical step. The following are the
                       most expected warnings or errors: <ul class = "ul">
                       <li class = "li"><span class = "ph uicontrol">The strain has exceeded fifty times the strain to cause first yield at ‘n’ points.</span></li>
                       <li class = "li"><span class = "ph uicontrol">Too many attempts made for this increment.</span></li>
                       <li class = "li"><span class = "ph uicontrol">Time increment required is less than the minimum specified.</span></li>
                       <li class = "li"><span class = "ph uicontrol">The solution fails to converge in the maximum number of iterations.</span></li>
                       </ul> </td>
</tr>
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Stabilization and contacts </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> In nonlinear static problems, instabilities like buckling or material
                       softening might occur. If these instabilities are localized, there a local transfer of strain energy
                       occurs from one part to another and global solution methods might not work. Here, automatic
                       (artificial) damping stabilization might help. The damping might help to get the model to converge but
                       at a loss of convergence speed and accuracy. Therefore, the damping factor is best to be chosen
                       as small as possible. The ratio of stabilization dissipation energy (ALLSD) to internal energy
                       (ALLIE) of the whole model should not be bigger than 5%. By default, the value is
                       <code class = "ph codeph">FACTOR=2e-4</code>. The following is the syntax for the 
                      <span class = "ph">Abaqus</span> 
                       input file for the respective step:
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *STATIC, STABILIZE, FACTOR=&lt;damping factor=""&gt;, ALLSDTOL
                       </code>
                       </pre>
                       It might also help to use
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *SURFACE BEHAVIOR, PENALTY=LINEAR
                       , 0., .001
                       </code>
                       </pre>
                       for contacts to relax the liner penalty stiffness. The default is  1.0.
                       <div class = "note"><span class = "run-in.note">Note:
			</span><span class = "notecontent"> A “good” value for the damping factor can be different from one model to another. In cases with
                       contact modeling, rigid body motion might occur while the contact is not fully established. </span></div>
 
                       By using <code class = "ph codeph">*CONTACT CONTROL, STABILIZE</code>, artificial damping is
                       introduced to increase stabilization. The damping coefficient is calculated automatically by default
                       if no value is assigned. 
                       <div class = "note"><span class = "run-in.note">Note:
			</span><span class = "notecontent"> When using step and contact stabilization simultaneously, a type of
                       "over-damping" occurs and the result becomes physically unrealistic. Therefore, a combination
                       of both commands is not recommended.
                       </span></div>
</td>
</tr>
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Solving convergence problems </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> For some convergence issues, it is not required to change the physics
                       of the models at all. The following warnings/errors can be found in the *.msg file. <ul class = "ul">
                       <li class = "li"> <span class = "ph uicontrol">Too many attempts made for this increment:</span> <p>This error occurs when
                       the solution seems to diverge and the solver reaches the default limits of iteration attempts
                       (5 for <span class = "ph">Abaqus</span>) 
                       for the corresponding time increment. It can  be solved by adding
                       <pre class = "codeblock">
                       <code class = "ph codeph"> 
                       *Controls, parameters=time incrementation
                       , , , , , , , 50, , ,
                       </code>
                       </pre>
                       which increases the iteration limit to 50. A value in this order is recommended.</p></li>
                       <li class = "li"> <span class = "ph uicontrol">The strain has exceeded fifty times the strain to cause first yield at ‘n’
                       points:</span>
                       <p>This error occurs most often when the strain rate at plastic regions
                       within the model gets too large. This can also be monitored by plotting the plastic dissipation
                       energy (ALLPD) in CAE or with <code class = "ph codeph">*ENERGY OUTPUT</code> or <code class = "ph codeph">*ENERGY PRINT</code>
                       <code class = "ph codeph">ALLPD</code>. Using parabolic step extrapolation or add damping factor might help to
                       solve this problem.
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *STEP, NAME=&lt;step name=""&gt;, NLGEOM=YES,   EXTRAPOLATION=PARABOLIC, INC=1000
                       </code>
                       </pre>
                       Or
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *Static, stabilize, factor=0.0002, allsdtol=0.05, continue=NO
                       </code>
                       </pre></p></li>
                       <li class = "li"> <span class = "ph uicontrol">Time increment required is less than the minimum specified:</span>
                       <p>This error can be misleading since multiple errors lead to this message. One option is to use the
                       following settings
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *STATIC
                       0.1, 1.0, 1e-14, 1.0
                       </code>
                       </pre>
                       Sometimes this error message is also associated with other problems where it helps to use the
                       contact stabilization or artificial damping instead (see above). <div class = "note"><span class = "run-in.note">Note:
			</span><span class = "notecontent">0.11 as a value for the
                       initial time increment is a recommended setting balancing convergence stability and speed.
                       </span></div>
</p></li>
                       <li class = "li"><span class = "ph uicontrol">The solution fails to converge in the maximum number of iterations:</span>
                       <p>This error means that the limit of consecutive equilibrium iterations is reached (default = 16).
                       It can be increased by adding to (for example 50) the following lines to the corresponding step.
                       <pre class = "codeblock">
                       <code class = "ph codeph">
                       *Controls, parameters=time incrementation
                       , , ,50 , , , , , , ,
                       </code>
                       </pre>
                       </p></li>
                       </ul> </td>
</tr>
<tr class = "row">
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__1"> Other step settings </td>
<td class = "entry" headers = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-settings__entry__2"> Quite often the error message is not specific or might have different
                       causes. Therefore, a few additional commands are mentioned in the following 
                       that might help to get the model to converge. <ul class = "ul">
                       <li class = "li"> When the simulation contains discontinuous behavior such as slip-stick 
                       or cracking, the following command might help. <code class = "ph codeph"> *CONTROLS,
                       ANALYSIS=DISCONTINUOUS</code> </li>
                       <li class = "li">When the contact formulation contains finite sliding, unsymmetric 
                       matrix storage and solving algorithm might help. <code class = "ph codeph"> *STEP,
                       UNSYMM=YES</code> </li>
                       </ul> </td>
</tr>
</tbody></table>
</div>


<div class = "section" id = "tso-c-usr-solver-abaqus-nonlinguide__tso-c-usr-solver-abaqus-nonlinguide-ErrorMessages"><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">Error Messages in .msg-files</h2>

<table class = "table"><caption/><colgroup><col/></colgroup><tbody class = "tbody">
<tr class = "row">
<td class = "entry"><br/><img class = "image" src = "../TsoUserImages/NonLinSizing_ErrorMessages.jpg" width = "756"/><br/></td>
</tr>
</tbody></table>
<p>The above error messages appear most often in the .msg file during a
failed optimization. The corresponding command might solve the problem. The error
“time increment required is less the minimum specified” occurs with different
problems and cannot be solved with a single command. It helps to analyze the
model with respect to tie contact, plasticity, element size, and other
instabilities.</p>
</div>

  
</div>

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