The bracket in this example consists of 926 nodes and 1719 S3R elements. The model contains seven different element sets. Each element set has a different thickness and is modeled as a laminated composite with 20 layers.

Ten unrestrained vibration modes are computed. The first six frequencies are approximately zero. The frequencies for the first four flexible modes are listed in Table 4–1.

The Abaqus finite element model is shown in Figure 4–1.

The complete input file, moldflow_ex1.inp, is shown below.

***************************************************************
**
** translated data from the Moldflow interface files named
** "moldflow_ex1.pat"
**  and
** "moldflow_ex1.osp"
**
** to the following Abaqus input files:
**
**            input file = moldflow_ex1.inp:  YES
**
** neutral material file = moldflow_ex1.shf:  YES
**                         (for *ELASTIC/*EXPANSION data)
**
**   initial stress file = moldflow_ex1.str:  YES
**                         (for *INITIAL CONDITIONS data)
**-------------------------------------------------------------
** echo of header information from the Moldflow interface 
** files:
**
** TITL information from .osp file:
** TITL
**
** FILE information from .osp file:
** FILE  JUN14-2002  11:13:29 mpi310 Residual Stress & 
** Properties
**
**      number of nodal properties = 0
**    number of element properties = 13
**                 number of nodes = 926
**          number of TRI elements = 1719
**           number of 1D elements = 0
**
** Moldflow results were written with ISP coding, i.e.,
** this is a filled anisotropic material with residual stresses
**           ------ -----------          ----
**-------------------------------------------------------------
** this input file was created with the following keyword data:     
**
**      *NODE     (926 nodes)
**
**      *ELEMENT  (1719 S3R elements)
**
**      *SHELL SECTION, COMPOSITE  (7 ELSETs)
**
**      *MATERIAL
**      *ELASTIC, TYPE=SHORT FIBER
**      *EXPANSION, TYPE=SHORT FIBER
**       (elastic and expansion data will be read from file
**        moldflow_ex1.shf)
**
**      *INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS,
**       INPUT=moldflow_ex1.str
**
**      *STEP
**       (Dummy step data.  Loads and boundary conditions
**        may need to be added to complete the model.)
***************************************************************
*HEADING
TITL
***************************************************************
*NODE, NSET=NALL, INPUT=moldflow_ex1_nodes.inp
***************************************************************
*ELEMENT, TYPE=S3R, ELSET=EALL, INPUT=moldflow_ex1_elements.inp
***************************************************************
*INCLUDE, INPUT=moldflow_ex1_elsets.inp
***************************************************************
*INCLUDE, INPUT=moldflow_ex1_sections.inp
***************************************************************
*MATERIAL,NAME=moldflow_mat_01
*ELASTIC,TYPE=SHORT FIBER
*EXPANSION,TYPE=SHORT FIBER
*DENSITY
1500.,
***************************************************************
*INITIAL CONDITIONS,TYPE=STRESS,SECTION POINTS,
 INPUT=moldflow_ex1.str
***************************************************************
*STEP
*FREQUENCY, EIGENSOLVER=LANCZOS
10, 
*END STEP
**
** SIGN: ljoXzAUD!NPKmw==
**