- Overlap the areas (Main Menu> Preprocessor> Modeling> Operate> Booleans> Overlap> Areas)
or glue them (Main Menu> Preprocessor> Modeling> Operate> Booleans> Glue> Areas) where
appropriate. - Save the model.
- Set the number of line divisions for all lines (Main Menu> Preprocessor> Meshing> Size Cntrls>
ManualSize> Lines> Picked Lines or use the MeshTool). - Select Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Write From Areas. A
picker appears. Pick the area(s) of the cells. - The program creates cells on the areas. Bad shape messages may appear during the mesh, but you
can ignore them.You may, however, see an "Unable to mesh area ...." message; if you do, clear the
elements from all areas (Main Menu> Preprocessor> Meshing> Clear> Areas) and repeat steps 4
and 5. - Write the .SECT file out to a unique name in the Write Section Library File dialog and click OK.
- Read in the user mesh file (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Read
Sect Mesh) to calculate the section properties. Material properties must be defined to calculate the
cross section shear correction factors, material-weighted centroids and the shear centers.
15.3.2.1. Line Element Size
Even if you have already set the line element size (LESIZE), you will see the following message:
Line element sizes may need to be specified for desired cross-section mesh. Please refer to the
LESIZE command.
If you have already set the line element size, click the Close button to continue. If you have not already
set it, issue LESIZE with the appropriate information.
When creating cells on the area using the GUI, it is not necessary to define a plane element type. On
the other hand, you must define a plane element type and mesh the area if you issue the SECWRITE
command explicitly.MESH200 with KEYOPT(1) = 7 and PLANE183 are the only valid plane element types.
15.3.3. Creating Custom Cross Sections with Mesh Refinement and Multiple Materials
When performing a plasticity analysis, you may need to refine the cross section mesh. A cross section
consisting of more than one material may be defined to represent layers, reinforcements or sensors.
When defining a multiple-material cross section, you will need to specify the material that each cross
section cell is made of. You can take a previously-created cross section and modify it.
To create a custom cross section with a refined mesh and/or multiple materials, perform the following
tasks:
- Either read a common section (Main Menu> Preprocessor> Sections> Beam> Custom Sectns> Edit/Built-
up> Edit Common) from the database or read a custom section from a .SECT file. (Main Menu> Pre-
processor> Sections> Beam> Custom Sectns> Edit/Built-up> Edit Custom) - The Graphics window displays a MESH200 plot.
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationBeam Analysis and Cross Sections