<!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>The Finite Element Model</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_topic3" id="xps10_pagetitle">The Finite Element Model</div>
      <hr noshade="true">
      <div class="title_division">Applying the Loads</div><a name="gsfem_10128"></a><p class="para_division">The uniform distributed load is applied to the three CBAR elements using a PLOAD1 entry.  One PLOAD1 entry is required for each element.  We have chosen fractional scaling, which means that the physical length of the element is normalized to a length of 1.0.  Since the distributed load runs the entire length of each element, each PLOAD1 entry will be applied from 0.0 to 1.0.  Since the load is uniform, P1&nbsp;=&nbsp;P2&nbsp;=&nbsp;22.0&nbsp;lb/in.</p><a name="gsfem_10130"></a><p class="para_division">The concentrated end moment is applied using a MOMENT entry.  The direction of the moment (by the right hand rule) is about the +z axis.  Thus,</p>
      <p class="para_division"><img align="bottom" src="graphics/gsfem11.gif" border="0"></p><a name="gsfem_10138"></a><p class="para_division">where M is the magnitude of 120.0 in-lb, and </p>
      <p class="para_division"><img align="bottom" src="graphics/gsfem12.gif" border="0"></p>
      <p class="para_division">is the vector (0.,&nbsp;0.,&nbsp;1.).</p><a name="gsfem_10139"></a><p class="para_division">The load set ID is 10, and the loads are selected in the Case Control Section with the Command LOAD = 10.</p>
      <div class="title_division">Applying the Constraints</div><a name="gsfem_10141"></a><p class="para_division">Grid 1 is fixed in a wall, so all six DOFs (123456) are constrained to zero.  This can be done directly on the GRID entry using Field 8 (PS&mdash;permanent single point constraints associated with the grid point).  No other constraints are required in this model.</p>
      <div class="title_division">Output Requests</div><a name="gsfem_10143"></a><p class="para_division">The Case Control Command DISP = ALL is required to report displacements.  In addition, it is a good idea to look at constraint forces at the wall as part of checking out the model.  Thus, we will add the Case Control Command SPCF = ALL.</p>
      <div class="title_division">The Input File</div><a name="gsfem_10148"></a><p class="para_division">The complete input file is shown in Listing <a class="links" href="javascript:void(0)" onclick="top.openFile('get_start/03topic_3.html#gsfem_10150');return(false);">2-1</a>.
      </p><a name="gsfem_10150"></a><div class="figure"><a name="gsfem_10151"></a><pre class="indent">
    ID MPM,EXAMPLE2 
SOL 101 
TIME 100 
CEND 
ECHO=BOTH 
DISP=ALL 
SPCF=ALL 
LOAD=10 
TITLE=EXAMPLE 2 
SUBTITLE=CANTILEVER BEAM 
LABEL=DISTRIBUTED LOAD AND END MOMENT 
$ 
BEGIN BULK 
$     DEFINE 
GRID POINTS  
GRID,1,,0.,0.,0.,,123456 
GRID,2,,10.,0.,0. 
GRID,3,,20.,0.,0. 
GRID,4,,30.,0.,0. 
$ 
$     DEFINE CBAR ELEMENTS  
CBAR,1,101,1,2,0.,1.,0. 
CBAR,2,101,2,3,0.,1.,0. 
CBAR,3,101,3,4,0.,1.,0. 
$ 
$     DEFINE CBAR ELEMENT CROSS SECTIONAL PROPERTIES 
PBAR,101,201,2.,.667,.1667,.458,,,
+PB1 +PB1,1.,.5 
$ 
$     DEFINE MATERIAL PROPERTIES 
MAT1,201,30.E6,,.3 
$ 
$     DEFINE UNIFORM DISTRIBUTED LOAD 
PLOAD1,10,1,FY,FR,0.,-22.,1.,-22. 
PLOAD1,10,2,FY,FR,0.,-22.,1.,-22. 
PLOAD1,10,3,FY,FR,0.,-22.,1.,-22. 
$ 
$     DEFINE CONCENTRATED MOMENT AT FREE END 
MOMENT,10,4,,120.,0.,0.,1. 
ENDDATA
  
</pre></div>
      <div class="title_figure">Listing 2-1. </div>
   </body>
</html>