Interfacing ANSYS and LS-DYNA

Sample Problem #1: Cylindrical Bar Impacting a Rigid Wall

 

Pre-Processing

 

Open ANSYS

·         ANSYS Interface has pull-down menu on the top. These menus cover functions such as plotting, display, and selection of entities. Help menu is also at this location.

·         ASNSY has also menus on the left side of the screen. These menus cover pre-processing, processing, and post-processing.

·         ANSYS needs to know that you are planning to create LS-DYNA model. That is why you need to select LS-DYNA Explicit Explicit in the Preferences

 

 

Define element type

 

 

Define material type.

Material model used is inelastic, plastic kinematic with the following characteristics:

Density (g/cm3) = 8.93

Elastic Modulus (g/msec2 cm) = 1.17

Tangent Modulus (g/msec2 cm) = 1.0x10-3

Yield Strength (g/msec2 cm) = 4.0x10-3

Poisson’s Ratio = 0.33

Hardening Parameter = 1.0

 

 

 

Import a Parasolid file (Note: You can create the quarter cylinder volume in ANSYS using Modeling menu)

File

            Import

                        Para…

 

Mesh Volume

Note: Once the volume becomes more complicated, hex elements will not work and tetrahedral elements become the only choice 

 

 

 

Add Boundary Conditions

These are the boundary conditions:

  1. The surface at the origin cannot move in the z-direction
  2. The two surface of symmetry cannot move in the normal direction

 

PlotCtrls

            Pan Zoom Rotate

                  Front

Select nodes on the vertical edge

Restrict these nodes in UX, AY, and AZ

Select nodes on the horizontal edge

Restrict these nodes in UY, AX, and AZ

 

PlotCtrls

            Pan Zoom Rotate

                        Left

 

Select nodes on the left edge

Restrict them in UZ

 

 

Set Time Controls

Set Output Controls
Specify the Output

(You can specify the output to either ANSYS, LS-DYNA, or both)

 

Save File (It is very important to save in ANSYS format (*.db) since it cannot read DYNA format (*.k))

File

            Save As

                        Sample1hx.db

 

Note: You will get warning that there is no explicit load defined. Ignore it since we will add the load outside ANSYS.

Initial Velocity:         

Initial velocity and contact can be input in ANSYS by creating component and assigning the initial velocity or contact specification to this component. It is much easier to create boxes that enclose the nodes within specific segments of your model.  You can do this by adding the following to your *.k program. In this section two boxes are created:

·         Box #1 encloses the surface at the origin

·         Box #2 encloses all other nodes

Place the text near the end of the *.k file.

 

*DATABASE_EXTENT_BINARY

         0         0         3         1         0         0         0         0

         0         0         4         0         0         0

*DEFINE_BOX

$        i         f         f         f         f         f         f

$    boxid       xmm       xmx       ymn       ymx       zmn       zmx

         1     -1.e6      1.e6     -1.e6      1.e6     -1.e6  0.50e-02

*DEFINE_BOX

$        i         f         f         f         f         f         f

$    boxid       xmm       xmx       ymn       ymx       zmn       zmx

         2     -1.e6      1.e6     -1.e6      1.e6  0.50e-02      1.e6

*INITIAL_VELOCITY

$        i         i         i

$     nsid    nsidex     boxid

         0         0         1

$        f         f         f         f         f         f

$       vx        vy        vz      

       0.0       0.0       0.0       0.0       0.0       0.0

*INITIAL_VELOCITY

$        i         i         i

$     nsid    nsidex     boxid

         0         0         2

$        f         f         f         f         f         f

$       vx        vy        vz       vxe       vye       vze

       0.0       0.0   -0.0227       0.0       0.0       0.0