Most of the major LS-DYNA capabilities are supported in the ANSYS LS-DYNA program and can be conveniently accessed through the graphical user interface of this program. It should be noted, however, that there are a number of other capabilities in the LS-DYNA program that cannot be directly accessed through the GUI of the ANSYS LS-DYNA program. Some examples are:
several material properties, such as fabric, soil, etc.
certain element types, such as seat belt
application of constraints on rigid bodies in the local coordinate system
Although these capabilities cannot be directly accessed, users who are familiar with the LS-DYNA program can still use these features indirectly in the ANSYS LS-DYNA program. The procedure for including additional features is outlined below.
Note: Only the LS-DYNA features that are described in the ANSYS LS-DYNA documentation and available through the ANSYS LS-DYNA interface are supported features. Although you can access other features as described below, features that you implement by editing the LS-DYNA input file are not supported.
After modeling has been completed, you can issue the EDWRITE
command instead of issuing the SOLVE command. (In the GUI, pick
.)
EDWRITE will create the LS-DYNA input file
Jobname.K. (Note that if the analysis is a small restart, the
input file will be named Jobname.R, and if it is a full restart,
the input file will be named
Jobname_nn.K.)
The difference between the EDWRITE command and the SOLVE command is that step number 3 discussed in Solution Process will not be executed. That is, Jobname.K will be written (along with headers to the ANSYS results files), but the solution process of the LS-DYNA program will not be started. After issuing EDWRITE, use one of the following two methods to include additional functionality in the explicit dynamic analysis.
Exit the ANSYS LS-DYNA program.
Edit the LS-DYNA input file Jobname.K to incorporate the items that are not supported directly through the ANSYS LS-DYNA program.
Execute the LS-DYNA executable separately in the same directory where the two results files, Jobname.RST and Jobname.HIS, reside. The solution produced by the LS-DYNA executable will be appended to these results files.
After completion of the LS-DYNA execution, enter the ANSYS LS-DYNA program and view the results using the postprocessors (POST1 and POST26).
Using another window, go to the directory where the ANSYS LS-DYNA program was started. Do not exit the ANSYS LS-DYNA program in the original window.
Edit the LS-DYNA input file Jobname.K to incorporate the items that are not supported directly through the ANSYS LS-DYNA program.
Execute the LS-DYNA executable separately in the same directory (where the two results files, Jobname.RST and Jobname.HIS, reside). The solution produced by the LS-DYNA executable will be appended to these results files. (Remember, you have not exited the ANSYS LS-DYNA program in the original window.)
After completion of the LS-DYNA execution, go back to the original window and view the results using the ANSYS LS-DYNA postprocessors.
For both Method A and Method B, you execute the LS-DYNA program by running the lsdynaxxx script (where xxx is the ANSYS release number) with the correct arguments:
lsdynaxxx i = jobname.k pr = product name
For example, if you have ANSYS LS-DYNA at ANSYS Release 18.2 and your input file is “crashtest.k”, you would type:
lsdyna182 i=crashtest.k pr=dynapc
You may need additional command line arguments, depending on what type of analysis you are running. For example:
For an implicit-to-explicit sequential solution (REXPORT and EDDRELAX commands; see Implicit-to-Explicit Sequential Solution), the argument "m=drelax" is required.
For a restart analysis, (EDSTART command; see Restarting), the argument "r=d3dumpnn" is required, where nn is the number of the dump file (01, 02, ... 99) to be used as a starting point.
To run the double precision version of LS-DYNA, the "-dp" argument is required.
For any type of analysis, you can specify the memory to be used by including the command line argument "memory=n", where n is the desired amount of memory in words.
When using these methods to modify the file Jobname.K, nodes and elements must not be changed. Also, note that the ANSYS LS-DYNA database is not updated with the changes you make in file Jobname.K. Thus, if an attempt is made to view the modified items in the PREP7, POST1 or POST26 processors after the solution is complete, the original version, and not the modified version, will be shown. (For these reasons, editing the LS-DYNA keyword input file, Jobname.K, is NOT a supported feature of ANSYS LS-DYNA.) In all cases, the complete set of results can be postprocessed in the LS-PREPOST postprocessor (assuming you requested LS-DYNA results files via the EDWRITE command).
In a typical ANSYS LS-DYNA analysis, the results file headers are written when you issue the SOLVE command (or when you issue EDWRITE). However, the LS-DYNA solver also has the ability to create the .RST and .HIS results file headers when only a file.K input file exists. This allows you to take a preexisting file.K, solve it using LS-DYNA, and then postprocess the results with the ANSYS LS-DYNA program.
To use this method, first make sure that the model defined in the .K file does not contain any features that ANSYS LS-DYNA does not support. Then edit the .K file so that the *DATABASE_FORMAT command is set to either 1 for ANSYS only results files, or 2 for ANSYS and LS-DYNA results files. Next, run the lsdynaxx script as described above.
You can then postprocess the results using POST1 and POST26. If the corresponding ANSYS database does not exist, element attributes (material properties, real constants, etc.) will not be available in the results files. However, you should still be able to postprocess the results using the ANSYS postprocessors. If you requested LS-DYNA results files, you will also be able to postprocess the results using LS-PREPOST.