Tutorials

Getting Started LS-DYNA/LS-PREPOST tutorial.

The way I did this was I went to the getting started tutorial for LS-Dyna on the support website:

Getting started with LS-Dyna

First I typed out the keyword file using this tutorial and the keyword manual. My notes about what I found out are described in the regular text below.

Once I ran this keyword file and new what the keyword file should look like I created the same keyword file using LS-Prepost. My notes on how to do this are described in the bold text below.

Follow the tutorial on the website with the regular text first, then go through in LS-prepost with the bold instructions.

Getting started: (make sure units are consistent!)
(Basic Keyword File) /ls-prepost instructions

File open>IGES file

*KEYWORD
Tells Dyna that keyword format is being used rather than structured format

(automatic)

*CONTROL_TERMINATION
This has to be used as a minimum to tell Dyna when to stop. (in this case 1 second) Can also apply other options if something happens first (certain cycle or deformation)

Page 3: select *control, select termination then click edit. Type in 1.0 for ENDTIM click accept and done

*DATABASE_BINARY_D3PLOT¬¬¬¬
For binary output files, If not specified in the keyword deck, then a complete output state will be written every time step. Contains plotting information to plot data over the three dimensional geometry of the model. (this can be plotted with LS-PREPOST)
Prints results every .1 second

Page 3: *Dbase, Binary_D3plot, type in .1 for DT, click accept and done.

*PART
We only have one part so part identification (pid=1) Only one section so (SECID=1) secid 1 is defined in the *SECTION, keyword block, Only one material so MID=1 defined in the *Material section

(4) go to page 5, PartD, select assi, select model, click secID in bottom panel, select the name of the solid section created in step 4, select MID in bottom panel select the material created in step 3. Assign part: click apply

To verify section properties (same panel) click prop click the model, select section at bottom then select material and view the cards

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

(3) go to page 3 click *section select solid from the list, click edit
Click new ID enter a title
Accept > done

*MAT_ELASTIC
Only one material defined by *PART, the density of this material is defined by RO, The Modulus of Elasticity is defined by E and Poison’s Ratio is defined by PR.

(2)Page 3, *MAT, group by: all sort: name or type (material 001-Elastic), Edit
Click new ID top left corner type in material density RO, Modulus of elasticity E and Poison’s ratio PR

Accept>done

*ELEMENT_SOLID
Defines a three dimensional solid element. EID is the Element ID, in this case an 8 node solid brick element. PID: as defined in part. N1 through N8, nodal points (start at back left and rotate counterclockwise along bottom face.

(1)Page 7 Block M >create, Type: multiple blocks,

I index list: type number of lines in mesh along I axis
J index: same for J
K index: same for K
X position list: enter x value at each line listed
Position list: same
Z position list: same
Click PList, select part

Or
Select single block and type in coordinates for each node (p1 ect.)

*This comes up with different nodes than that numbered in the keyword file example. Make sure you know which node is which.

*NODE
NID: node number, X,Y, Z coordinates,

TC: Translational Constraint
EQ.0 no constraints
EQ.1 constrained x displacement
EQ.2 constrained y displacement
EQ.3 constrained y displacement
EQ.4 constrained x and y displacements
EQ.5 constrained y and z displacements
EQ.6 constrained z and x displacements
EQ.7 constrained x, y, and z displacements

RC Rotational Constraint:
EQ.0 no constraints
EQ.1 constrained x displacement
EQ.2 constrained y displacement
EQ.3 constrained y displacement
EQ.4 constrained x and y displacements

(5) specify boundary conditions: go to page 5, click SPC, select create, select node, select which DOF to fix, click edge button under graphics window, select the node to fix in the graphics window.

To delete a constraint: select show, click constraint to delete in bottom window, click delete, press apply

OR:
go to page 3, click *Node, change TC and RC on card as listed above.

*LOAD_SEGMENT
Used to apply a distributed pressure load over one triangular or quadrilateral segment defined by four, six, or eight nodes LCID: load curve ID (pulled from *DEFINE_CURVE), SF: load curve scale factor, AT: arrival time of pressure, N1-N8 (id of nodes applied to)

(7) page 3, click *load, click segment, edit click dot next to LCID to select Define Curve. Keept SF, AT default, click dot next to nodes to pick where to apply the load

*DEFINE_CURVE
Used to define a load curve (load vs. time) LCID: only one load curve, A1, A2: points in time, o1: corresponding load value. (Two separate cards here)

(6)Page 3, click *DEFINE, curve, edit, click new ID, keep all variables default: type in A1 and O1 the first point, click insert, then type in second point and click insert, click accept and done

*END
End of keyword file

Formatting is strict, line everything up along left edge with even spacing.

LS-POST: (for both)

File>open> LS-DYNA Binary Plot open plot created by LS-DYNA

Select History under option 1 on right hand side menu.

Select Nodal, Z displacement, select node desired (7 in this case)

Click scale at bottom of graph ymin: -.12 and ymax

Unless otherwise stated, the content of this page is licensed under Creative Commons Attribution-ShareAlike 3.0 License