Z-mat/ANSYS interface

Description

The Zansys functionality mirrors very much the same principals as in the Z-mat for ABAQUS port, and so we refer the user to that documentation as well. This section provides a getting started guide to Zansys.

Syntax

% Zansys [ opts]  problem  \(\hookleftarrow\)

Getting started

Perform a standard installation of Z-set, including the binaries and shared files. The install location will henceforth be referred to as the Z7PATH. The launch procedures for Zansys will also need to be able to locate the ansys

Note

In versions prior to 8.3.6 it was necessary to perform a user build and link process in order to generate a user executable of ansys. The newer versions interface with via shared libraries, and henceforth the user needs to do nothing special for the interface to work. There are some test cases in the %Z7PATH%\test\Zansys\INP directory. The Z-mat material files are named 10#.txt where # is the material number selected in the test using ansys commands such as:

TB,USER,4,0,0
TB,STATE,4,,40
MPCHG,4,1

which would set the Z-mat material for element group 1 to be read in the file 104.txt. Currently all the commands listed in the Z-mat handbook for the ABAQUS interface are supported with ANSYS as well, except the use of multiple field variables. Temperature is available as a parameter, and can be set using commands like:

BFUNIF,TEMP,523.0

The name TEMP will be re-mapped to temperature in the Z-mat files. To try the test cases, do for example:

z:
cd %Z7PATH%\test\Zansys\INP
Zansys plast3

which launches the ansys GUI from which the input file can be loaded:

/INPUT,plast3,inp

Elements and output Z-mat for ansys must be run using the 18x class elements. In order to get output for the state variables in the Z-mat material model, an additional command must be issued to get the variables stored to the output database, such as:

OUTRES,SVAR,ALL,

To plot the variable one can use the command:

PLESOL,SVAR5,1

Note

With user materials in the solver is by default set to not extrapolate integration point stresses to the nodal points. In fact only does this extrapolation by default for linear materials, while most other codes assume that a least-squares fit extrapolation method should be done in all cases. In order to activate extrapolation the following lines can be used before the SOLVE command is issued:

ERESX,YES

With the Z-set RST file reader direct integration point visualization is supported, so unfortunately there is no refined solution for this issue.