<!DOCTYPE html
  PUBLIC "-//W3C//DTD HTML 4.01 Transitional//EN">

<!--
Copyright (c) 2006 UGS Corp.

All Rights Reserved.

This software and related documentation are proprietary to UGS Corp.
-->
<html>
   <head>
      <meta http-equiv="Content-Type" content="text/html; charset=UTF-8">
      <title>Reviewing the Results</title>
      <script language="javaScript">
        abridged="false";
        displayConditions=new Array();
      </script>
      <link type="text/css" href="../css/main_styles.css" rel="stylesheet">
   </head>
   <body class="bodydocs" onload="top.pageLoader()" bgcolor="#FFFFFF">
      <div class="title_topic2" id="xps10_pagetitle">Reviewing the Results</div>
      <hr noshade="true"><a name="gsprelim_11044"></a><p class="para_topic">You cannot simply move directly to the displacement and stress results and accept the answers.  You are responsible for verifying the correctness of the model.  Some common checks are described in this section.</p>
      <div class="title_division">Check for Error Messages, Epsilon, and Reasonable Displacements</div><a name="gsprelim_11048"></a><p class="para_division">No error or warning messages are present in the .f06 (results) file&mdash;this is certainly no guarantee of a correct run, but it&rsquo;s a good first step.  Also, examine the value of epsilon on page 6 of the output.  It is very small (~10<sup class="superscript">&ndash;16</sup>), showing stable numerical behavior.  Next, it is a good policy to check the displacement values, just to verify that they are not absurdly out of line with the physical problem or that a geometric nonlinear analysis is not required.  For example, this beam displacing several inches might indicate that a load is orders of magnitude too high, or that a cross sectional property or an elastic modulus has been incorrectly specified.  In our case, the lateral displacements (page 8 of the output) are on the order of 10-3 inches, which seems reasonable for this problem.
      </p>
      <table border="0">
         <tr>
            <td valign="top" align="left"><img align="left" src="../graphics/note.gif" alt="Note" title="Note"></td>
            <td valign="bottom" align="left" width="100%">
               <div class="para_note"><a name="gsprelim_11055"></a><p class="para_note_body">Suppose you did obtain displacements of several inches&mdash;or perhaps into the next city.  Shouldn&rsquo;t NX Nastran give some sort of engineering sanity warning?  The answer is no, because the program is doing precisely what it was told to do and has no ability to judge what a reasonable displacement is.  Recall that our analysis is linear and that the MAT1 material property entry thinks that the elastic modulus E is the material curve.  This distinction is shown in Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11121');return(false);">1-</a>.
                  </p>
               </div>
            </td>
         </tr>
      </table><a name="gsprelim_11121"></a><div class="figure">
         <p align="left"><img align="bottom" src="graphics/gsprelim7.gif"></p>
      </div>
      <div class="title_figure">Figure. Reality versus Modeling</div><a name="gsprelim_11122"></a><p class="para_division">The MAT1 entry states that our material is always elastic and infinitely strong.  In reality, we will violate restrictions on small displacements and material linearity given sufficient loading.</p>
      <div class="title_division">Check Reactions</div><a name="gsprelim_11127"></a><p class="para_division">To check static equilibrium, we calculate the reaction forces at the constraints and obtain 33.3 lbs. in the +y direction at grid point 1 and 66.6 lbs. in the +y direction at grid point 4 (Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11306');return(false);">1-</a>(a)).  These values match the forces of single point constraint reported on page&nbsp;9 of the output (T2 in this table means forces in the Y direction).  Thus, the load and resulting reactions make sense.
      </p>
      <div class="title_division">Check Shear Along the Beam</div><a name="gsprelim_11136"></a><p class="para_division">The shear diagram for the beam is shown in Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11306');return(false);">1-</a>(b).  The output lists the shear forces across each element as -33.3 lbs. for elements 1 and 2 and +66.6 lbs. for element&nbsp;3.
      </p><a name="gsprelim_11137"></a><p class="para_division">Note that shear occurs only in plane 1 (the plane of the applied force).  The sign convention for CBAR element internal shear forces in Plane 1 (<sub class="subscript">elem</sub>&mdash;y<sub class="subscript">elem</sub> plane) is shown in Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11174');return(false);">1-</a>:
      </p><a name="gsprelim_11174"></a><div class="figure">
         <p align="center"><img align="bottom" src="graphics/gsprelim22.gif"></p>
      </div>
      <div class="title_figure">Figure. CBAR Element Shear Convention (Plane 1)</div><a name="gsprelim_11175"></a><p class="para_division">Thus, the signs make sense with respect to the applied load.</p><a name="gsprelim_11306"></a><div class="figure">
         <p align="center"><img align="bottom" src="graphics/gsprelim26.gif"></p>
      </div>
      <div class="title_figure">Figure. Beam Reaction Forces, Shear Diagram, and Moment Diagram</div>
      <div class="title_division">Displacement and Stress Results</div><a name="gsprelim_11309"></a><p class="para_division">The displacement at the point of application of the load (GRID 3) is shown in the results:</p>
      <p class="para_division"><img align="bottom" src="graphics/u_eq.gif" border="0">.
      </p><a name="gsprelim_11314"></a><p class="para_division">The deflection is in the -y direction as expected.</p><a name="gsprelim_11315"></a><p class="para_division">The CBAR element stresses at the point of application of the load (GRID 3) are reported by end b of CBAR 2 and end a of CBAR 3.  Positive stress values indicate tension and negative values indicate compression.  The top of the beam is in compression and the bottom of the beam is in tension.  Stress recovery point 1 is located on the top of the beam and point 2 is located at the bottom of the beam, as shown in Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11395');return(false);">1-</a>:
      </p><a name="gsprelim_11395"></a><div class="figure">
         <p align="center"><img align="bottom" src="graphics/gsprelim58.gif"></p>
      </div>
      <div class="title_figure">Figure. Bar Element Output Nomenclature</div><a name="gsprelim_11396"></a><p class="para_division">The NX Nastran CBAR element stress output (Figures 6-7) is interpreted as shown in Figure <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11430');return(false);">1-</a>:
      </p><a name="gsprelim_11430"></a><div class="figure">
         <p align="center"><img align="bottom" src="graphics/gsprelim18.gif"></p>
      </div>
      <div class="title_figure">Figure. Bar Element Stress Output</div><a name="gsprelim_11434"></a><p class="para_division">Therefore, the top surface of the beam (point 1) sees &ndash;999.5 lb/in (compression) and the bottom surface sees 999.5 lb/in (tension).</p>
      <div class="title_division">Comparing the Results with Theory</div><a name="gsprelim_11440"></a><p class="para_division">First, the deflection at the point of application of the load will be determined by hand.  This calculation does not include shear effects, so it can be directly compared with the NX Nastran results shown in the NX Nastran Output.  The deflection due to bending only is calculated as follows:</p><a name="gsprelim_11485"></a><p class="para_division"><img align="bottom" src="graphics/gsprelim27.gif" border="0"></p><a name="gsprelim_11490"></a><p class="para_division"><img align="bottom" src="graphics/gsprelim34.gif" border="0"></p><a name="gsprelim_11491"></a><p class="para_division">This value is in exact agreement with the T2 value for GRID 3 on page 8 of the NX Nastran output.</p><a name="gsprelim_11492"></a><p class="para_division">The effect of shear deflection is determined by adding the second continuation of the PBAR entry and rerunning the job.  The new Bulk Data Section is shown in Listing<a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11508');return(false);">1-2</a>.      
      </p><a name="gsprelim_11508"></a><div class="figure">
         <p align="left"><img align="bottom" src="graphics/LIST_1-3_1.gif"></p><a name="gsprelim_11506"></a><p class="para_figure"> Shear Factor K: K1 = K2 = 5/6 = .8333 for rectangular sections</p>
      </div>
      <div class="title_figure">Listing 1-2. Shear Factor K on PBAR Entry</div><a name="gsprelim_11515"></a><p class="para_division">The deflection results are given in the output:      </p>
      <p align="left"><img align="bottom" src="graphics/LIST_1-3_2.gif"></p><a name="gsprelim_11516"></a><p class="para_division">Comparing deflection at GRID 3 with and without shear, we have:</p><a name="gsprelim_11520"></a><p class="para_division"><img align="bottom" src="graphics/gsprelim39.gif" border="0">   (without shear) = -2.221112E-3 inch  
      </p>
      <p class="para_division"><img align="bottom" src="graphics/gsprelim40.gif" border="0">   (with shear) = -2.255780E-3 inch
      </p><a name="gsprelim_11524"></a><p class="para_division">Thus, adding shear to the model results in about 1.6% greater deflection of GRID 3.</p><a name="gsprelim_11525"></a><p class="para_division">The stresses on the top and bottom surfaces of the beam at the point of application of the load are given by</p>
      <p class="para_division">&sigma; = bending stress = &plusmn;Mc/I</p>
      <p class="para_division">    where:       </p>
      <table width="100%" align="center">
         <colgroup span="1">
            <col span="1" width="22*">
            <col span="1" width="20*">
            <col span="1" width="252*">
         </colgroup>
         <tr valign="top">
            <td colspan="1" rowspan="1"><a name="gsprelim_11532"></a><p class="para_td">M</p>
            </td>
            <td colspan="1" rowspan="1">
               <p class="para_td">=</p>
            </td>
            <td colspan="1" rowspan="1"><a name="gsprelim_11536"></a><p class="para_td">moment at GRID point 3</p>
            </td>
         </tr>
         <tr valign="top">
            <td colspan="1" rowspan="1"><a name="gsprelim_11538"></a><p class="para_td">c</p>
            </td>
            <td colspan="1" rowspan="1">
               <p class="para_td">=</p>
            </td>
            <td colspan="1" rowspan="1"><a name="gsprelim_11542"></a><p class="para_td">distance from neutral axis to outer fiber</p>
            </td>
         </tr>
         <tr valign="top">
            <td colspan="1" rowspan="1"><a name="gsprelim_11544"></a><p class="para_td">I</p>
            </td>
            <td colspan="1" rowspan="1">
               <p class="para_td">=</p>
            </td>
            <td colspan="1" rowspan="1"><a name="gsprelim_11548"></a><p class="para_td">bending moment of inertia in plane 1</p>
            </td>
         </tr>
      </table><br><a name="gsprelim_11553"></a><p class="para_division">From <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/02topic_13.html#gsprelim_11306');return(false);">1-</a>(c), the moment at GRID 3 is 666.6 in-lb.  Thus,
      </p>
      <p align="center"><img align="bottom" src="graphics/gsprelim42.gif"></p><a name="gsprelim_11558"></a><p class="para_division">which is in agreement with the NX Nastran results.</p>
   </body>
</html>