8.6.3.2.3. Solution Monitoring
This option provides a facility to monitor a solution value at a specified node in a specified DOF. The
command also provides a means to quickly review the solution convergence efficiency, rather than at-
tempting to gather this information from a lengthy output file. For instance, if an excessive number of
attempts were made for a substep, the information contained in the file provides hints to either reduce
the initial time step size or increase the minimum number of substeps allowed through the NSUBST
command to avoid an excessive number of bisections.
Command(s):MONITOR
GUI: Main Menu> Solution> Unabridged Menu> Load Step Opts> Nonlinear> Monitor
Additionally, the NLHIST command allows you to monitor results of interest in real time during solution.
Before starting the solution, you can request nodal data such as displacements or reaction forces at
specific nodes. You can also request element nodal data such as stresses and strains at specific elements
to be graphed. Pair-based contact data are also available. The result data are written to a file named
Jobname.nlh.
For example, a reaction force-deflection curve could indicat e when possible buckling behavior occurs.
Nodal results and contact results are monitored at every converged substep while element nodal data
are written as specified via the OUTRES setting.
You can also track results during batch runs. To execute, either access the ANSYS Launcher and select
File Tracking from the Tools menu, or type nlhist150 in the command line. Use the supplied file
browser to navigate to your Jobname.nlh file, and select it to invoke the tracking utility. You can use
this utility to read the file at any time, even after the solution is complete.
Command(s):NLHIST
GUI: Main Menu> Solution> Results Tracking
8.6.3.2.4. Birth and Death
Specify birth and death options as necessary. You can deactivate (EKILL) and reactivate (EALIVE) selected
elements to model the removal or addition of material in your structure. As an alternative to the
standard birth and death method, you can change the material properties for selected elements (MPCHG)
between load steps.
Command(s):EKILL,EALIVE
GUI: Main Menu> Solution> Load Step Opts> Other> Birth & Death> Kill Elements
Main Menu> Solution> Load Step Opts> Other> Birth & Death> Activate Elem
The program "deactivates" an element by multiplying its stiffness by a very small number (which is set
by the ESTIF command), and by removing its mass from the overall mass matrix. Element loads (pressure,
heat flux, thermal strains, and so on) for inactive elements are also set to zero. You need to define all
possible elements during preprocessing; you cannot create new elements in SOLUTION.
Those elements to be "born" in later stages of your analysis should be deactivated before the first load
step, and then reactivated at the beginning of the appropriate load step. When elements are reactivated,
they have a zero strain state, and (if NLGEOM,ON) their geometric configuration (length, area, and so
on) is updated to match the current displaced positions of their nodes. See the Advanced Analysis Guide
for more information about birth and death.
Another way to affect element behavior during solution is to change the material property reference
number for selected elements:
Command(s):MPCHG
GUI: Main Menu> Solution> Load Step Opts> Other> Change Mat Props> Change Mat Num
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationNonlinear Structural Analysis