Mechanical APDL Structural Analysis Guide

13.2.2. Using FiberSIM Data in ANSYS

The general process for using FiberSIM .xml file data in your ANSYS simulation follows:

1. Create nodes.


2. Define material properties.


3. Specify element types.


4. Issue section commands (SECTYPE,SECDATA,SECCONTROL,SECOFFSET,SECREAD, and SLIST) as
   needed to apply material properties and thickness to flat layers.


5. Define elements.


6. Specify nodal DOF constraints as needed.


7. Solve.

The FiberSIM-ANSYS translation combines the layup order and layer orientations from FiberSIM with
the material and thickness information that you provide via ANSYS section (SECxxx) commands.

The following simple input file illustrat es each part of the process:

/bat,list

/show,sample,grph

/prep7

/title, Sample FiberSIM input data handling using SHELL281!

! Create nodes

!

n,21

n,22,10

n,23,10,7

n,24, ,7

ngen,2,10,11,14,1,,,4

!

! Define material properties

!

mp, ex,1,30e6! steel

mp, ex,2,10e6! alum

mp, ex,3,11e6! alum5

mp,prxy,1,.3

mp,prxy,2,.3

mp,prxy,3,.3

mp,dens,1,.00003

mp,dens,2,.00001

mp,dens,3,.00001

!

! Setup for element 2 using section commands and

! FiberSIM to define layer info

et,2,281

keyopt,2,8,1

sectype,4,shell,fibersim, lamin1

secdata,0.2,1,,,STEEL

secdata,1.0,2,,,ALUM

secdata,0.2,3,,,ALUM5

seccontrol, , , , .05 , , , ,100,0.155, 0 , 15 , 0 , 0

!

secoffset,bot

secread,sample,xml

/com ==================== issue slist,all

slist,all

!

! Define elements

!

type,2 $real,6 $secn,4 $e,21,22,23,24,25,26,27,28!

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

The FiberSIM-ANSYS Interface