12.1. Output Controls

12.1.1. Results (Jobname.RST) vs. History (Jobname.HIS) Files

Results available for postprocessing depend on the information written to the Jobname.RST and Jobname.HIS files via the EDRST and EDHTIME commands (Main Menu> Solution> Output Controls> File Output Freq).

Note the distinction between the Jobname.RST and the Jobname.HIS files: The Jobname.RST file, used primarily in POST1 processing, contains solutions for the entire model, but captured at a relatively small number of time points. Generally, the Jobname.RST file contains just enough solutions to animate the results. The Jobname.HIS file, used in POST26, contains solutions captured at a relatively large number of time points, but for only a portion of the model. (Capturing a large number of solutions for the entire model would quickly fill up disk space.) As a comparison, the number of time steps in the Jobname.RST file is usually less than 100; in the Jobname.HIS file, it is usually 1000 or more.

12.1.2. Creating Components for POST26

Before reviewing results in POST26, you may create element and/or nodal components within your model. For example, during either the PREP7 or the SOLUTION phases of your analysis, choose a set of elements for which you want to review results. Create a component consisting only of those elements. You can also create a component consisting of a specified set of nodes. These components can be created via the GUI or by issuing the following commands:

ESEL,S,MAT,,1 !Select elements of material 1.
CM,elm1,elem !Create element component elm1.
NSLE !Select nodes from elements.
CM,nod1,node !Create nodal component nod1.

Element and nodal components should be limited to conserve disk space. For details on creating components, see the Basic Analysis Guide.

12.1.3. Writing the Output Files for POST26

Before using POST26 to review results, you must direct ANSYS LS-DYNA to write the appropriate information to the Jobname.HIS and other output files. While in either the PREP7 or SOLUTION phases of your analysis, specify the number of time steps, the element and nodal components to be analyzed, and the ASCII files to be written. You can specify this information via the GUI (Main Menu> Solution> Output Controls) or by issuing the following commands:

EDHTIME,NSTEPS  !Specify the number of time steps
                ! for time-history results.
EDHIST,elm1     !Specify the name of the element component.
EDHIST,nod1     !Specify the name of the nodal component.
EDOUT,GLSTAT    !Write ASCII file GLSTAT (Global time step
                ! and energy statistics).
EDOUT,MATSUM    !Write ASCII file MATSUM (Energy information
                ! for each PART).
EDOUT,SPCFORC   !Write ASCII file SPCFORC (Single point
                ! constraint (Reaction) forces).
EDOUT,RCFORC    !Write ASCII file RCFORC (Resultant interface
                ! force data).
EDOUT,SLEOUT    !Write ASCII file SLEOUT (Sliding interface 
                ! energy).
EDOUT,NODOUT    !Write ASCII file NODOUT (Nodal data).
EDOUT,RBDOUT    !Write ASCII file RBDOUT (Rigid body data).

Note to LS-DYNA Users--If you are familiar with other ASCII files created by the LS-DYNA program, you may want to issue EDOUT,ALL to write all possible ASCII files.


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