Update 1D Element Properties Using Cross Sections

Use the Section Property tool to update properties assigned to bar2 or rod elements (target) using a cross section on various entities as the source.

1. From the Mesh ribbon, click the Section Property tool.

   
   
   Figure 1.

2. Select 1D elements to update.

   Selection is filtered to retain only valid elements (bar2 and rod configurations). Moreover, for OptiStruct and Nastran, a further filter is performed on element types to retain only CBAR/CBEAM/CROD elements.

3. Select source elements.
   Sources are the entities intersected with a plane used to calculate sectional properties. Valid sources types are:

   • Solids
   • Surfaces
   • Elements

   If surfaces or 2D elements are selected, then the intersection with a plane (lines) is inflated using local thickness. It is mandatory to have a valid property with a thickness value assigned to sources. In the case of surfaces, it must be done at the component level.

   Moreover, the source entities' materials are used to evaluate material weighted sectional properties. As specified in Materials, if a material is not available for a region, the default is used.

4. Use the microdialog options to define plane locations and where intersections are generated on source elements.

   
   
   Figure 2. Section Cut: a) Single cut b)Per element c)Per node

   Single cut

   Update a list of elements with a single property extracted from a single user-defined location. Click to define the cutting plane. You can adjust the base point and plane normal. Placing the cutting tool on a target element will adjust the plane’s normal along the selected element’s X axis.

   A single preview shows intersections before proceeding. Changing the source updates the preview.

   The reference point (see Orientation and Offset) is the intersection of the cutting plane with a target element. This defines the reference orientation and offset.

   If you perform a section cut using a plane which does not intersect any of the target elements (Figure 3), then the reference point is extracted from the plane's base point.

   You need to pay attention to the local normal and relative position of the manipulator in the section cut to obtain accurate result to assign to its target selection. Target elements must have consistent orientation.

   
   
   Figure 3. Single cut out of targets

   Cut per element

   Automatically perform a section cut on each target element. As explained in Orientation and Offset, the resultant section is valid per element no matter its orientation. The intersection is done by default on the midpoint of the target element. You can set a value (0 to 1) to specify the parametric position between the target element’s nodes (Figure 4). The orientation can’t be changed. The plane is normal to the target’s X axis.

   Since a cut is performed per element, all meshing processes and calculations are done as many times as target elements selected. This is obviously more time consuming than a single cut. Whenever a region of multiple targets share the same section, it is advisable to use the Single Cut method to reduce computation time.

   
   
   Figure 4. Intersection at 30% resp. 80% of each element

   Cut per node

   A cut is performed on each node of the target elements. If adjacent elements form a vertex angle between their X axis below the threshold angle tolerance, a single cut is done for common nodes; otherwise, one cut per element is performed at the same node using different normal. No additional test is done on (Y,Z) axis deviation from adjacent elements. Properties will be created with two beam sections: one at each end station. If a single cut is done on a node, the two adjacent properties share the same beam section for their relative station.

5. Click in the microdialog to toggle between a finite and infinite plane

   In some situations, it is best to consider a finite plane to intersect sources. In the Figure 5, using the (default) infinite planes would result in undesired regions considered during trimming. In such cases, you can switch to a finite plane and define the width and height of the section cut. However, it is not possible to define the size location per location. The width and height will be common for all intersections.

   Finite planes are available for all types of cuts (single | per element | per node) and all types of sources. However, when sources are Solid geometries, a cut is considered valid only if it fully crosses boundary surfaces (solid partial cut is not supported).

   
   
   Figure 5. Finite size planes

6. Click on the guide bar to define how to handle welds and contacts.
   See Disconnected Parts for more information.
7. Optional: Select a target material.

   If the Auto calculate checkbox is turned on below the guide bar, a homogenized material is automatically generated. Otherwise, if switched off, select a target material to be used.

   Refer to comments in Sectional Property Evaluation Theory regarding the normalization of sectional properties using material to obtain correct stiffnesses.

8. Click .

   The sectional properties calculation is launched. When the process is done, a review of the calculated sections is shown. Properties are created based on the element configuration and assigned to elements. Offset is applied to target elements. Material and beam sections are generated per property.

   The review considers real section shapes (after inflates) as well as offsets. If you proceed with different selections or exit the tool, the graphic review goes away.

   The actual shape of a section is currently not saved in the generic beam section generated. Using Beam details view will show an equivalent rectangle as usual.

   
   
   Figure 6.