Interfacing ANSYS and LS-DYNA

Sample Problem #8: Impact on a Cylindrical Shell

 

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 in the Preferences

In Windows, select Start

Programs

ANSYS Release 7.0

ANSYS Interactive

            In Product Selection, choose: ANSYS DYNAPrepPost

                        Run

 

 

Define element type

Element Group #1: shell element (thickness=0.125),

 

 

 

 
 

Assign Thickness to the Plates

 

 

Define material type.

 

Inelastic, perfectly plastic kinematic material is used for group #2 with the following characteristics:

Density (lb-sec2/in4) = 2.5E-4

Elastic Modulus (lb/in2) = 1.05E7

Yield Strength (g/msec2 cm) = 4.4E4

Poisson’s Ratio = 0.33

Hardening Parameter = 1.0

Hardening Modulus (lb/in2) = 0.0

 

 

 

 

 

 

Create the shell

Create keypoints to describe the arc

Click Apply

Repeat with:

Point #2 at 0,2.93,0

 

 

Create the arc (by center and radius)

 

 

Select origin

Select other point

Enter angle as 60 degrees

 

If we need the arc in the first quadrant, we should reflect it.

 

 

Select the arc

 

 

Plot

            Replot

 

PlotCtrls

            Pan, Zoom, Rotate

                        Iso

 

 

Note: It may be a good idea if duplicate keypoints are deleted to make selection of points easier.

 

 

Create two more lines to make the patch

 

 

Create Area

Select the 4 lines

 

Meshing

Plot

            Lines

 

 

 

 

Click on Areas

Select area

 

Add Boundary Conditions

Plot

            Elements

PlotCtrls

            Pan, Zoom, Rotate

            Click on Top

 

Choose the nodes in the y-z plane

           

 

Choose the nodes on the lower edge

Constrain all degrees of freedom

           

 

Choose nodes on the two remaining edges

Constrain them in the x and y directions

 

Set Simulation Time

Set Output Controls

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

Specify the Output Frequency

 

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

File

            Save As

                        ex8b.db

 

 

Initial Velocity:         

Initial velocity can be input by creating 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 one box is created:

·         Box #1 encloses the interior nodes and the symmetry edge

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

 

$

$     define section

$

*DEFINE_BOX

$        i         f         f         f         f         f         f

$    boxid       xmm       xmx       ymn       ymx       zmn       zmx

         2,-0.01,2.5,1.49,2.95,-12.5,-.01  

$     initial condition section

$

*INITIAL_VELOCITY

$        i         i         i

$     nsid    nsidex     boxid

         0         0         2

$        f         f         f         f         f         f

$       vx        vy        vz        wx        wy        wz

       0.0,-5650.0,0.0,0.0,0.0,0.0