Mechanical APDL Basic Analysis Guide - Ansys

prnsol
finish
5.9.2. VT Accelerator Re-run
Once you have performed an analysis using the VT Accelerator option [STAOPT,VT or TRNOPT,VT], you may
rerun the analysis; the number of iterations required to obtain the solution for all load steps and substeps
will be greatly reduced. You can make the following types of changes to the model before rerunning:
• Modified or added/removed loads (constraints may not be changed, although their value may be
modified)
• Materials and material properties
• Section and real constants
• Geometry, although the mesh connectivity must remain the same (i.e. the mesh may be morphed)
VT Accelerator allows you to effectively perform parametric studies of nonlinear and transient analyses in a
cost-effective manner (as well as to quickly re-run the model, which is typically necessary to get a nonlinear
model operational).
5.9.2.1. VT Accelerator Re-run Requirements
When rerunning a VT Accelerator analysis, the following files must be available from the initial run:
• Jobname.DB – the database file. It may be modified as listed in the previous section.
• Jobname.ESAV – Element saved data
• Jobname.RSX – Variational Technology results file
5.9.2.2. VT Accelerator Re-run Procedure
The procedure for rerunning a VT Accelerator analysis is as follows:
1. Enter the ANSYS program and specify the same jobname that was used in the initial run with /FILNAME
(Utility Menu> File> Change Jobname).
2. Resume the database file using RESUME (Utility Menu> File> Resume Jobname.db) and make any
modifications to the data.
3. Enter the SOLUTION processor using /SOLU (Main Menu> Solution), and indicate that this is a restart
analysis by issuing ANTYPE,,VTREST (Main Menu> Solution> Restart).
4. Because you are re–running the analysis, you must reset the load steps and loads. If resuming a database
saved after the first load step of the initial run, you will need to delete the loads and redefine the loads
from the first load step.
5. Initiate the restart solution by issuing the SOLVE command. See Obtaining the Solution (p. 112) for details.
6. Repeat steps 4, 5, and 6 for the additional load steps, if any.
5.10. Exercising Partial Solution Steps
When you initiate a solution, the ANSYS program goes through a predefined series of steps to calculate the
solution; it formulates element matrices, triangularizes matrices, and so on. Another SOLUTION command,
PSOLVE, (Main Menu> Solution> Partial Solu) allows you to exercise each such step individually, completing
just a portion of the solution sequence each time. For example, you can stop at the element matrix formu-
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
5.10. Exercising Partial Solution Steps
123