Getting Started

Problem Definition

Consider the deformation of an aluminum block sitting on the floor with a pressure applied to the top surface.

Input File Preparation

The first step is to create a mesh and define node points. Since we are just getting started, we will define the mesh as consisting of only 1 element and 8 node points as shown in the following figure. Also, we will use default values for many of the parameters in the input file, and therefore not have to enter them.

The following steps are required to create the finite element model input file.

The first line of the input file must begin with *KEYWORD. This identifies the file as containing the keyword format instead of the structured format which can also be used (see LS-DYNA Structured User s Manual):

    *KEYWORD

The first input block is used to define solution control and output parameters. As a minimum, the *CONTROL_TERMINATION keyword must be used to specify the problem termination time. We will apply the pressure load as a ramp from 0 Pa to 70.e+05 Pa during a time interval of 1 second. Therefore, the termination time is 1 second. Additionally, one of the many output options should be used to control the printing interval of results (e.g., *DATABASE_BINARY_D3PLOT). We will print the results every 0.1 seconds:

    *CONTROL_TERMINATION 
            1.
    *DATABASE_BINARY_D3PLOT 
            .1

The second input block is used to define the model geometry, mesh, and material parameters. The following description and map may help to understand the data structure in this block. We have 1 part, the aluminum block, and use the *PART keyword to begin the definition of the finite element model. The keyword *PART contains data that points to other attributes of this part, e.g., material properties. Keywords for these other attributes, in turn, point elsewhere to additional attribute definitions. The organization of the keyword input looks like this:

The LS-DYNA Keyword User Manual should be consulted at this time for a description of the keywords used above. A brief description follows:

*PART

We have 1 part identified by part identification (pid=1). This part has attributes identified by section identification (sid=1) and material identification (mid=1).

*SECTION_SOLID

Parts identified by (sid=1) are defined as constant stress 8 node brick elements by this keyword.

*MAT_ELASTIC Parts

identified by (mid=1) are defined as an elastic material with a density Á, a modulus of elasticity E, and a Poisson ratio of µ.

*ELEMENT_SOLID

Eight node solid brick elements identified by element identification (eid=1) have the attributes of (pid=1) and are defined by the node list (nid)

*NODE

The node identified by (nid) has coordinates x,y,z.

Our finite element model consists of 1 element, 8 nodes, and 1 material. Keeping the above in mind, the data entry for this block looks like this:

    *PART 
    aluminum block 
    $--------+---------+---------+---------+---------+---------+---------+---------+ 
    $      PID     SECID       MID     EOSID      HGID      GRAV    ADPOPT      TMID
             1         1         1 
    *SECTION_SOLID 
    $--------+---------+---------+---------+---------+---------+---------+---------+
    $    SECID    ELFORM       AET
             1 
    *MAT_ELASTIC 
    $--------+---------+---------+---------+---------+---------+---------+---------+
    $      MID        RO         E        PR        DA        DB         K
             1     2700.   70.e+09        .3 
    *ELEMENT_SOLID 
    $------+-------+-------+-------+-------+-------+-------+-------+-------+-------+
    $    EID     PID      N1      N2      N3      N4      N5      N6      N7      N8
           1       1       1       2       3       4       5       6       7       8 
    *NODE 
    $------+---------------+---------------+---------------+-------+-------+-------+
    $    NID               X               Y               Z      TC      RC
           1              0.              0.              0.       7       7       
           2              1.              0.              0.       5       0 
           3              1.              1.              0.       3       0 
           4              0.              1.              0.       6       0 
           5              0.              0.              1.       4       0 
           6              1.              0.              1.       2       0 
           7              1.              1.              1.       0       0 
           8              0.              1.              1.       1       0

The third input block is used to define boundary conditions and time dependent load curves. We are applying a load of 70.e+05 Pa to the top surface of the block defined by nodes 5-6-7-8. We will ramp the load up from 0 Pa to 70.e+05 Pa during a time interval of 1 second:

    *LOAD_SEGMENT 
    $--------+---------+---------+---------+---------+---------+---------+---------+ 
    $     LCID        SF        AT        N1        N2        N3        N4  
             1        1.        0.         5         6         7         8 
    *DEFINE_CURVE 
    $--------+---------+---------+---------+---------+---------+---------+---------+ 
    $     LCID      SIDR       SFA       SFO      OFFA      OFFO    DATTYP
             1        
    $------------------+-------------------+
    $                 A1                  O1
                      0.                  0.
                      1.             70.e+05
    *END

The last line in the input file must have the keyword *END

LS-DYNA solution

The vertical and horizontal displacement of node 7, calculated by LS-DYNA, are shown in the following 2 graphs. The solution to this simple problem can be calculated analytically. The LSDYNA solution compares exactly with the analytical solution.

The vertical displacement due to a 70.0e+05 Pa pressure load can be calculated by:

The horizontal displacement is: