3.6. ANSYS

This command defines the name of the Mechanical APDL job from which the analysis results will be obtained. The command is mandatory if BEAMST is to be performed following a Mechanical APDL analysis and must be omitted otherwise.

The ANSYS command is a preliminary command, and should only appear at the head of the BEAMST data set.

Parameters

ANSYS

Keyword

FNAME

Keyword to denote that the job names are specified in a job name list file (Optional).

Jobname
  1. Without FNAME – job name of the Mechanical APDL model to be processed. This is the name associated with the .RST file generated by Mechanical APDL (Alphanumeric, up to 32 characters).

  2. With FNAME – name of file containing paths and names of Mechanical APDL jobs to be included in the analysis together.

youngs

Young's Modulus (Optional, Real).

density

Material density (Optional, Real).

Notes

  1. BEAMST will only process certain Mechanical APDL beam element types in an ANSYS model. Valid element names are:

    BEAM44, BEAM188*, BEAM189*, PIPE16, PIPE59*, PIPE288*, PIPE289*

    Elements marked with * must be meshed within Mechanical APDL (that is, many elements to one member). The UNBR command should be used to define the unbraced length, otherwise incorrect results will be obtained.

  2. If youngs is omitted, the Young’s modulus of steel will be assumed, i.e. youngs = 2.1E11 N/m2. If youngs is specified, it is assumed that the value is consistent with the units adopted in the ANSYS analysis.

  3. If density is omitted, the density of steel will be assumed, i.e. density = 7850 kg/m3. If density is specified, it is assumed that the value is consistent with the units adopted in the ANSYS analysis.

  4. The job name list file specified after keyword FNAME consists of a number of data lines that define the Mechanical APDL results sets (i.e. load cases) to be analyzed by BEAMST. The format of each data line is described as follows:

    FullPathName (LCAnsys) (LCAsas)

    where

    FullPathName is the name of the .RST file including path if necessary. If no path is specified, it is assumed that the .RST file is located in the same directory as the BEAMST data file. If the specified string contains any embedded space, then the whole string must be bounded by double quotes (“).

    LCAnsys is the system result set number in the .RST file where results will be considered in BEAMST. If it is zero or not specified, all result sets in the .RST file will be transferred to BEAMST.

    LCAsas is the ASAS user load case number for this Mechanical APDL result set in BEAMST. If it is zero or not specified, it will be set as the last assigned BEAMST user load case number + 1. If multiple Mechanical APDL result sets are implied in the command (i.e. LCAnsys = 0), LCAsas defines the user load case number of the first

  5. If the Mechanical APDL job name is specified directly (i.e. without FNAME), all the Mechanical APDL results sets in the .RST file will be transferred to BEAMST with user load case numbers ranging from 1 to the number of result sets.

  6. If the BEAMST load cases care are obtained from multiple Mechanical APDL analyses, user must ensure that all the models are consistent as no cross checks will be carried out by BEAMST.

Examples

  1. The Mechanical APDL analysis is a single job called ANSYSJOB. All the load cases in this job will be analyzed in BEAMST.

    ANSYS ANSYSJOB

  2. The Mechanical APDL analysis information is contained in a job name file called Ansysfile.txt, which references three Mechanical APDL jobs called Ansysjob1, Ansysjob2 and Ansysjob3 located in different directories. The first load case (results set) in each of these 3 jobs will become load cases 10, 20 and 30 in BEAMST.

    ANSYS FNAME Ansysfile.txt

    The contents of file Ansysfile.txt are:

    C:\AnsysAnalysis\Job1\Ansysjob1 1 10

    “C:\AnsysAnalysis\Job2\Ansysjob2” 1 20

    C:\AnsysAnalysis\Job3\Ansysjob3 1 30


Release 18.2 - © ANSYS, Inc. All rights reserved.