The ANSYS-specific Command Environment

The interface program works in conjunction with an ANSYS-specific command environment. This environment is activated via the command 'PROPERTY FE-PROG ANSYS' and is used to prompt the user for loading conditions and material and physical property definitions. Environment variable FG_PRE_INT (see section 1.4 ) can be used to make ANSYS the default environment for all models.

It is important to note that the analysis environment cannot be changed when material properties, physical properties or loads have been defined in the FEMGEN model.

In addition a Resource file can be used to customise the program to ANSYS. The Resource file may be edited whilst the program is running. An example of a FEMGV Resource file 'femsys.ini' is shown below:

     
#
# This is a FEMGV Resource file. 
#
# Related Files: 
#
# fgvstr.str :- FEMGV startup file used to set environment variables
# FGVSYN.SYN :- Synonym file for command macros and hot keys.
#                                  
# Customised Analysis Environments.
# =================================
# 
# Use these settings in conjunction with environment variable
# FG_PRE_INT in the startup file. Note that more
# than one analysis package may be defined here if desired.
#
# ANSYS Resources:
#
# Set default element variants.
#
Femsys.ansys-variant.all.BE2  : BEAM4
Femsys.ansys-variant.all.TR3  : PLANE42
Femsys.ansys-variant.all.TR6  : PLANE2
Femsys.ansys-variant.all.QU4  : PLANE42
Femsys.ansys-variant.all.QU8  : PLANE82
Femsys.ansys-variant.all.PE6  : SOLID45
Femsys.ansys-variant.all.P15  : SOLID95
Femsys.ansys-variant.all.HE8  : SOLID45
Femsys.ansys-variant.all.HE20 : SOLID95
#
# Set ANSYS degree of freedom names.
#           
Femsys.ansys-dofname.internal.1 : UX
Femsys.ansys-dofname.external.1 : UX
Femsys.ansys-dofname.internal.2 : UY
Femsys.ansys-dofname.external.2 : UY
Femsys.ansys-dofname.internal.3 : UZ
Femsys.ansys-dofname.external.3 : UZ
Femsys.ansys-dofname.internal.4 : ROTX
Femsys.ansys-dofname.external.4 : ROTX
Femsys.ansys-dofname.internal.5 : ROTY
Femsys.ansys-dofname.external.5 : ROTY
Femsys.ansys-dofname.internal.6 : ROTZ
Femsys.ansys-dofname.external.6 : ROTZ
Femsys.ansys-dofname.internal.8 : PRES
Femsys.ansys-dofname.external.8 : PRES
Femsys.ansys-dofname.internal.10 : VOLT
Femsys.ansys-dofname.external.10 : VOLT
Femsys.ansys-dofname.internal.11 : TEMP
Femsys.ansys-dofname.external.11 : TEMP
#
# End of Resource File
#

The FEMGV2.3 commands used with previous versions of the Interface Program are still available. Attention is drawn to the new FEMGV commands that may be useful to the ANSYS users. The following gives some examples of these new commands, (see the FEMGV User Manual for further information).

     
MESHING TYPES S1 PLANE82   
MESHING TYPES 6SURFS SOLID95
MESHING TYPES 5SURFS SOLID95

CONSTRUCT COORDSYS CYLINDRIC CS1 P1 P2 P3
PROPERTY LOAD FORCE LO1 S1 100 1
PROPERTY ATTACH LO1 CS1

CONSTRUCT SCURVE SC1 SURFACE LINE L1 ELIPSE 10
PROPERTY ATTACH LO1 SC1

CONSTRUCT LMASK LM1 SURFACE .2 .8 .2 .8
PROPERTY ATTACH LO1 LM1

PROPERTY BOUNDARY CONSTRAINT L1 XSYMM

PROPERTY BOUNDARY PRESCRIBE S1 T 273
                
UTILITY TABULATE FE [ANSYS] BE2 

UTILITY GRAPH SCURVE SC1

LABEL MESH TYPES 

LABEL OPTIONS CONSTRNTS TEXT ON