12.2. Using POST1 with ANSYS LS-DYNA

The first step in POST1 is to read data from the results file into the database. If the database does not already contain model data, issue the RESUME command to read the database file (or in the GUI pick Utility Menu> File> Resume Jobname.db). Then issue the SET command to read in the desired set of results (or in the GUI pick Main Menu> Postproc> Read Results> By Load Step or By Time/Freq).

The typical POST1 operations available in ANSYS are also available in ANSYS LS-DYNA. You can display the deformed shape, show contour and vector displays, and obtain tabular listings just as you would in ANSYS. For details on these and other POST1 postprocessing functions, see the Basic Analysis Guide.

When using POST1, you can rotate stress results into a defined coordinate system using the RSYS command. Stress data will be rotated during printout, display, or element table operations. RSYS supports stress output for all explicit element types except BEAM161, COMBI165, and composite SHELL163 (KEYOPT(3) = 1). To use RSYS in models that contain these element types, you must unselect the unsupported elements before issuing the RSYS command.


Note:  Strain data results cannot be rotated for any explicit elements. If you request strain results when RSYS is not set to the global Cartesian coordinate system, the printing or plotting command will be ignored.


When you display results in POST1, failed elements will automatically be removed from the display. Failed elements are elements that exceed the specified failure criteria (for example, failure strain). In some cases, the mesh connectivity may appear to be lost due to the number of failed elements in the model at a given time step. However, the elements are still in the selected set, and the model will behave as expected physically. (During the LS-DYNA solution, failed elements are removed from the solution after they fail.)

12.2.1. Animating Results

You can also display animated shapes using POST1 capabilities; for example, you could animate the element centroidal stresses superimposed on the deformed shape. After you have read in a set of results from the Jobname.RST file, pick Utility Menu> PlotCtrls> Animate> Over Results. Then use the “push-button” animation controls in the dialog box to start, stop, resume, and otherwise control the animation.

If you are using command input, use the appropriate plotting command (for example, PLESOL) followed by the ANDATA command (as shown below).

PLESOL,Item,Comp
ANDATA

This command method reads in all results data and animates the plot. For faster plotting, use the INRES command to select specific types of solution data before issuing the above commands:

INRES,Item

12.2.2. Element Output Data

Remember that the results available for POST1 processing differ from element to element. For a complete description of output data for each explicit dynamics element (LINK160, BEAM161, PLANE162, SHELL163, SOLID164, COMBI165, MASS166, LINK167, SOLID168), see the Element Reference.

The stress output for explicit dynamic elements is true stress. The strain is the time integration of the incremental strain. The incremental strain is calculated from the incremental displacement, assuming a linearized relationship. So the strain measure is similar to the logarithmic strain definition. However, the reported shear strain is the engineering shear strain.

For the PLANE162, SHELL163, SOLID164, and SOLID168 elements, the available strain output depends on the type of material models used. For all material models, total strains (total strain components, total principal strains, total strain intensity, and total equivalent strain) are always available. For the following material models, elastic strains are also available.

Isotropic Elastic
Bilinear Isotropic
Bilinear Kinematic
Viscoelastic
Johnson-Cook Plasticity
Powerlaw Plasticity
Strain Rate Dependent Plasticity
Piecewise Linear Plasticity
3 Parameter Barlat Plasticity

For the following plastic material models, equivalent plastic strain is available. However, plastic strain components and principal plastic strains are not available.

Bilinear Isotropic
Bilinear Kinematic
Temperature Dependent Bilinear Isotropic
Elastic-Plastic Hydrodynamic
Steinberg
Johnson-Cook Plasticity
Powerlaw Plasticity
Strain Rate Dependent Plasticity
Piecewise Linear Plasticity
Geological Cap
Barlat Anisotropic Plasticity
3 Parameter Barlat Plasticity
Transversely Anisotropic Elastic Plastic
Transversely Anisotropic FLD
Bamman
Rate Sensitive Powerlaw Plasticity
Zerilli-Armstrong
Elastic Viscoplastic Thermal
Modified Piecewise Linear Plasticity

Below are some additional notes about the explicit dynamics elements:

  • With SOLID164, stress and strain solutions are saved only at the element centroid, regardless of whether you use 1-point or 8-point integration (KEYOPT(1)).

  • With BEAM161 and SHELL163 elements, stress and strain solutions are saved only at the element center (for each layer for shell elements), regardless of whether you use full or reduced integration.

  • When using BEAM161 and SHELL163 elements, you must specify both the number of integration points for which you want ANSYS LS-DYNA to calculate the results (using real constants) and the number of these points for which you want results stored (using the EDINT command). By default, the number of integration points (NIP) is set to 2 for shell elements; you can specify up to 5 points (layers) for the Gauss integration rule. For more than 5 layers, you need to use either the trapezoidal integration rule or the user-defined integration rule. (Note--The trapezoidal rule is not recommended for less than twenty integration points, especially in bending.) Also by default, the number of layers you specify using EDINT,SHELLIP is set to 3 for shell elements. If NIP = 2, the results at the bottom correspond to integration point 1, the results at the top correspond to integration point 2, and the results at the middle are an average of the top and bottom results. For beam elements, results are saved for 4 integration points by default (BEAMIP = 4 on the EDINT command). For the resultant beam formulation (KEYOPT(1) = 2), there is no stress output, regardless of the BEAMIP setting. If you set BEAMIP = 0, no stress output is written for any of the beam elements. In this case, the beams will not appear in any POST1 plots because the program assumes they are failed elements.

  • With SHELL163 elements use the LAYER,NUM command to specify the layer for which you want results. Layers are numbered starting from the bottom layer and moving up for stress data. However, for strain data, layer 1 is the bottom layer and layer 2 is the top layer, no matter how many layers exist. Strain information is saved only at these two layers. Further, data is only available at the middle of the layer, not at the top or bottom surface of a layer (or the element, for that matter). To get results close to the element surface, specify a large number of integration points through the thickness of the shell. However, saving data for all of these layers can become expensive.

  • SHELL163 is not affected by the SHELL,LOC command. By default, output data for the top layer is displayed when plotting data (PLNSOL, PLESOL), but data for the top and bottom layers appears on printed results.

12.2.3. Postprocessing after Adaptive Meshing

If you use adaptive meshing in an explicit dynamic analysis, the analysis will typically produce multiple results files. The procedure for postprocessing these files is slightly different than postprocessing a single results file.

Adaptive meshing can be used in ANSYS LS-DYNA to refine the mesh of shell elements during a large deformation analysis (see Adaptive Meshing for details on how to use adaptive meshing). When adaptive meshing is included in an analysis, the number of elements in the model may increase during the solution as the mesh is improved to conform to a user specified element aspect ratio. As the number of elements in the model changes, the extension of the results file is updated to represent a new finite element mesh for the model.

The name of the results file extension is incremented as follows:

Jobname.RS01 - First mesh refinement
Jobname.RS02 - Second mesh refinement
Jobname.RS03 - Third mesh refinement
etc.

In order to postprocess multiple results files, you must specify the appropriate filename and extension (FILE command) to examine a particular time step. You should not resume the original model database (.DB file), as the mesh in that database will not match what is in the results files. The sample input below demonstrates a typical postprocessing session.

/POST1
FILE,Jobname,RS01 ! Specify the results file for the first
                  ! mesh refinement
SET,LIST          ! List out the time steps that were written
                  ! for the first mesh refinement
SET,1,2           ! Set the results to a particular time
                  ! step value
PRNSOL,. . .      ! Print or display the results

Caution:  The element attributes are not saved on the RSnn file. Therefore, care must be taken when using select logic during postprocessing with these files. Also, you should not attempt to perform a solution using only the information contained in these files, nor should you attempt to save a new database from these files.


You should not use the standard method for animating results (ANDATA command) after adaptive meshing because it is only valid for animating a single results file (Jobname.RST). Instead, you must use the ANMRES command to animate results when multiple results files are present (Jobname.RS01, Jobname.RS02, etc.).

Before starting the animation, you must use the /FILNAME command to specify the jobname that the results will be animated across. Because results are animated across multiple files with the same jobname, simply specifying the FILE command will not allow multiple results animations.

The following sample input demonstrates a typical animation session using ANMRES. In this example, the jobname is 'impact' and the animation runs from results file impact.rs01 to impact.rs10. The results file increment is two and the time delay is 0.5 seconds.

/FILNAME,impact
/POST1
FILE,impact,rs01
SET,last
PLNSOL,s,eqv
ANMRES,.5,1,10,2

In the GUI, the ANMRES command is accessed from the utility menu: Utility Menu> PlotCtrls> Animate> Over Results. Choose the options to animate over multiple results files and then use the push-button animation controls in the dialog box to start, stop, resume, and otherwise control the animation.


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