Defining LS-DYNA Model and Load Data, Controls, and

Output - HM-4605

In this tutorial, you will learn to:

• View DYNA keywords in HyperMesh as they will appear in the exported DYNA input file
• Understand part, material, and section creation and element organization
• Create sets
• Create velocities
• Understand the relation of DYNA entity type to HyperMesh element and load configurations
• Create nodal single point constraints
• Create contacts with set segment ID
• Define output and termination
Export models to LS-DYNA formatted input
• files
Tools/Utilities

The following tools/utilities set the foundation for settings up an Ls-Dyna input deck with
HyperMesh:

• LS-Dyna FE input translator

• FE output template
• Ls-Dyna Utility menu
• User Profile
Exercises

This tutorial contains the following exercises:

Exercise 1: Define Model Data for the Head and A-Pillar Impact Analysis

Exercise 2: Define Boundary Conditions and Loads for the Head and A-Pillar Impact Analysis
Exercise 3: Define Termination and Output for the Head and A-Pillar Impact Analysis

Section 1: Define Model Data

Relation of *PART, *ELEMENT, *MAT, and *SECTION to Each Other

*ELEMENT EID PID

*PART PID SID MID

*SECTION SID
*MAT MID

A *PART shares attributes such as section properties (*SECTION) and a material model
(*MAT). A group of elements (*ELEMENT) sharing common attributes generally share a
common part id (PID). The figure below shows how the keywords *PART, *ELEMENT,
*MAT and *SECTION relate to each other. A unique PID assigns a material id (MID) and a
section id (SID) to an element.

The figure below shows how the keywords *ELEMENT, *PART, *SECTION, and *MAT are
organized in HyperMesh.

*ELEMENT EID PID Elements are organized into a component

collector

*PART PID SID Component collector’s card image

MID

*SECTION SID Property collector with a property card

image. Assign a property to a *PART by
pointing to the property collector in the
component collector’s card image.

*MAT MID Material collector with a material card

image. Assign the material to the *PART
by associating the material collector to the
component collector.
Component, property and material collectors are created and edited from the collectors panel.

View DYNA Keywords in HyperMesh

A HyperMesh card image allows you to view the image of keywords and data lines for defined
DYNA entities as interpreted by the loaded template. The keywords and data lines appear in the
exported DYNA input file as you see them in the card images. Additionally, for some card
images, you can define and edit various parameters and data items for the corresponding
DYNA keyword.

Card images can be viewed using the Card Editor panel which can be accessed from either the
Tool menu, the Card Editor icon in the toolbar, or from the right-click context menus in the
Model Browser and Solver Browser.

Create *MAT

In HyperMesh, a *MAT is a material collector with a card image. To relate it to a *PART, the
material collector is associated to a component collector. A material collector can be created
from the Model Browser, Solver Browser or by selecting the Material drop down menu and
choosing Create.

Update a Component’s Material

Update any component with any material from the component collectors panel, update sub-
panel.

Material Table Utility

This utility allows you to do the following:

• View a list of all existing materials in the model and attributes for them.
• Create, edit, merge and check for duplicate materials.
This utility is located in the LS-DYNA Utility tab under DYNA Tools page.

Create *SECTION

In HyperMesh, *SECTION is a property collector with a card image. This is created in the
property collectors panel, create sub-panel.

Exercise 1: Define Model Data for the Head and A-Pillar Impact Analysis

The purpose for this exercise is to help you become familiar with defining LS-DYNA
materials, sections and parts using HyperMesh.

This exercise comprises of setting up the model data for an LS-DYNA analysis of a hybrid III
dummy head impacting an A-pillar. The head and A-pillar model is depicted below.

Head and A-pillar model (Ch2_Image1.tif)

This exercise contains the following tasks.

• Define the material *MAT_ELASTIC for the A-pillar part and head part.
• Define *SECTION_SHELL for the A-pillar.
• Define *SECTION_SOLID for the head.
Define *PART for the A-pillar and the
• head.
Step 1: Load the LS-DYNA user profile

1. From the Preferences drop down menu, click User Profiles…

2. Select the LsDyna profile and click OK.
Step 2: Retrieve the HyperMesh file head_start.hm

1. You can retrieve the .hm file in one of the following two ways:
From the File drop down menu, point to Import..., click on HyperMesh Model and browse to
• select the .hm file. Click Apply.

• From toolbar, click the Files icon and browse to select the .hm file. Click Open.
The model loads into the graphics area.

Step 3: Define the material *MAT_ELASTIC for the A-pillar and head

1. Access the Materials panel in one of the following ways:

• From the Materials drop down menu, click Create.

• From the toolbar, click the Materials icon.

2. Go to create sub-panel.
3. For name =, type elastic
4. For card image =, select MATL1.
5. Click create/edit to create the material and edit its card image.
6. Click the [Rho] field and enter 1.2 E-6 for the density.
7. For Young’s modulus [E], specify 210.
8. For Poisson’s ratio [Nu], specify 0.26.
9. Click return to go to the Material panel.
10. Click return.
Step 4: Define *SECTION_SHELL with a thickness of 3.5 mm for the A-pillar

1. Access the Properties panel in one of the following ways:

• From the Properties drop down menu, click Create.

• From the toolbar, click Properties icon .

2. For name =, type section3.5.
3. In the type= field, select surface.
4. For card image =, select SectShll.
5. For thickness =, enter 3.5
6. Click create/edit to open the card image for the property.
Notice that a thickness (T1) of 3.5 is assigned to *SECTION_SHELL card image.

7. Click return to the go back to the Properties panel.

Step 5: Define *SECTION_SOLID for the head

1. In the Properties panel, in the name = field, type solid.

2. In the type= field, select surface.
3. For card image =, select SectSld.
4. Click create to create the property.
5. Click return to go back to the main menu.
Step 6: Define *PART for the A-pillar

It’s *MAT_ELASTIC is the material collector named "elastic". Its *SECTION_SHELL is the
property collector named "section3.5".

1. From the Collectors drop down menu, select Edit and select Component.
2. Go to update sub-panel.
3. Set the collector to comps.
4. With the comps selector active, select the component pillar.
5. For card image =, select Part.
6. For material =, select elastic.
7. For property =, select section3.5.
8. Click update/edit.
Notice that a *PART has been created and a section (SID) and a material (MID) has been
9. assigned to it.
10. Click return to the collectors panel.
11. Remain in this panel for the next step.
Step 7: Define *PART for the head

It’s *MAT_ELASTIC is the material collector named "elastic". Its *SECTION_SOLID is the
property collector named "solid".

1. With the comps selector active, select the component head.

2. For card image =, select Part.
3. For material =, select elastic.
4. For property =, select solid.
5. Click update/edit.
Notice that a *PART has been created and a section (SID) and a material (MID) has been
assigned to it.

6. Click return to go back to the collectors panel.

7. Click return to go back to the main menu.
The exercise is complete. Save your work to a HyperMesh file.

Section 2: Define Boundary Conditions and Loads

*INITIAL_VELOCITY_(Option)

The table below describes DYNA keywords for defining initial velocity.
DYNA keyword Velocity applied to … Setup in HyperMesh

*INITIAL_VELOCITY set of nodes, Entity set of nodes,

*SET_NODE_LIST load collector with
InitialVel card image

*INITIAL_VELOCITY_GENERATIO one *PART or set of Entity set of comps,

N parts, load collector with
*SET_PART_LIST InitialVel card image

*INITIAL_VELOCITY_NODE individual nodes Created from velocity

panel,
organized in load collector
with no card image
*SET

With the exception of *SET_SEGMENT, all *SET types are created from the entity sets panel
in the Analysis page, or from clicking Tools, Create and Sets. Graphically view a set’s contents
with the review function in the entity sets panel. *SET_SEGMENT is created from the
contactsurfs panel and is discussed in this chapter.

HyperMesh Entity Configurations and Types

HyperMesh elements and loads have two identifiers: configuration and type. Configuration is a
HyperMesh core feature. Type is defined by the loaded FE output template. A configuration
can support multiple types. Before creating elements or loads, select the desired type from
either the elem types panel (in the 1D, 2D and 3D pages) or by clicking Mesh, Assign and
clicking Element.

Use the load types sub-panel from the Analysis panel only when creating loads directly on
nodes or elements. For all other cases, the load is defined by creating a load collector with a
card image. For example, *INITIAL_VELOCITY_NODE (applied directly to nodes) is created
from the velocities panel while *INITIAL_VELOCITY (applied to nodes in a set) is a load
collector with the InitialVel card image.

You can see a list of element and load configurations in the elem types panel and the load types
panel, respectively. These panels are pictured below.
 elem types panel

load types panel

Some element configurations are rigid and quad4. When a dyna.key template is loaded, types
of the rigid configuration are RgdBody, ConNode and GenWeld
(*CONSTRAINED_NODAL_RIGID_BODY, *CONSTRAINED_NODE_SET and
*CONSTRAINED_GENERALIZED_WELD_SPOT).

Similarly, some load configurations are force and pressure. Types of the pressure configuration
are ShellPres and SegmentPre (*LOAD_SHELL_ELEMENT and *LOAD_SEGMENT).

Most element and load configurations have their own panels. For example, rigids are created
from the rigids panel and constraints are created from the constraints panel.

*BOUNDARY_SPC_(Option)

The table below describes DYNA keywords for defining nodal single point constraints.

DYNA keyword Constraint applied to … Setup in HyperMesh

*BOUNDARY_SPC_NOD individual nodes These are constraints created

E from the constraints panel and
organized into a load collector
with no card image.

*BOUNDARY_SPC_SET a set of nodes This is an entity set of nodes

*SET_NODE_LIST referenced in a load collector’s
 BoundSpcSet card image.
*CONTACT and *SET_SEGMENT

With the exception of *CONTACT_ENTITY, DYNA contacts are created from the interfaces
panel from the BCs drop down menu. (*CONTACT_ENTITY is created from the rigid walls
panel from the BCs drop down menu.)

A DYNA contact is a HyperMesh group. When you want to manipulate a *CONTACT, such as
delete, renumber, or display it off, you select groups.

DYNA Contact Master and Slave Types

DYNA has multiple contact master and slave types from which to choose. The table below lists
these types. While HyperMesh supports all of them, this chapter focuses on contacts with slave
and master type 0, set segment id. Chapter three focuses on the other slave and master types.

*SET_SEGMENT and Contactsurfs Panel

*SET_SEGMENT is created from the contactsurfs panel. Additionally, from this panel, you
can add and remove elements from an existing *SET_SEGMENT and adjust the normal of
segments without adjusting the normal of elements.

The graphical representation of a contactsurf is pyramids, one pyramid for each segment. The
orientation of a pyramid represents the normal orientation of the segment. By default, the
orientation of a pyramid is the same as the normal of the element underneath.

A *SET_SEGMENT is specified in a *CONTACT from the interfaces panel, add sub-panel

with master: or slave: type set to csurfs.

Exercise 2: Define Boundary Conditions and Loads for the Head and A-Pillar Impact Analysis

The purpose for this exercise is to help you start becoming familiar with defining LS-DYNA
boundary conditions, loads and contacts using HyperMesh.

This exercise comprises of setting up the boundary conditions and loads data for an LS-DYNA
analysis of a hybrid III dummy head impacting an A-pillar. The head and A-pillar model is
depicted below.
 Head and A-pillar model

This exercise contains the following three tasks.

• Define velocity on all nodes of the head with *INITIAL_VELOCITY

Constrain the pillar’s end nodes in all six degrees of freedom with
• *BOUNDARY_SPC_NODE
Define a contact between the head and A-pillar with
• *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE
Step 1: Make sure the LS-DYNA user profile is still loaded

1. From the Preferences drop down menu, click User Profiles, or click the User Profiles icon.
2. Select LsDyna.
Step 2: Retrieve the HyperMesh file head_2.hm

1. Retrieve the model file, head_2.hm.

Take a few moments to observe the model using various visual options available in
2. HyperMesh (rotation, zooming, etc.).
Step 3: Create a node set, *SET_NODE_LIST, containing all the nodes in the head component

1. Access the entity sets panel in one of the following ways:

• From the Tools drop down menu, click Create and click Sets
• From the Analysis page, click entity sets
2. For name =, type Vel_Nodes.
3. For card image, select Node.
With the nodes selector active, select nodes and select by collector and select the component
4. head(2).
5. Click create to create the set.
6. Click return to go back to the main menu.
Step 4: Define the velocity

1. Click on the load collectors icon on the toolbar.

2. For name =, type init_vel.
3. For the card image = select InitialVel.
4. Click create/edit to create the load collector and edit its card image.
5. In the node set id [NSID] field, select the entity set Vel_Nodes.
6. In the initial velocity in the global x-direction, VX field, specify 5.
7. Click return to go back to the load collectors panel.
8. Stay in the load collectors panel for the next step.
Step 5: Create a load collector for the constraints to be created

1. For name = type SPC.

2. For creation method select no card image.
3. Optionally select a color for the load collector.
4. Click create to create the load collector.
5. Click return to go back to the main menu.
Step 6: Create constraints on the pillar’s end nodes

1. Access the constraints panel in one of the following ways:

• From the BCs drop down menu, click Create and select Constraints.
• From the Analysis page, click constraints.
2. Leave the entity selector set to nodes.
3. Select nodes and select by sets and select the pre-defined entity set nodes for SPC.
4. Notice the nodes at the pillar’s ends are highlighted.
5. Leave all six degrees of freedom, dof1 thru dof6, active.
6. Set the load type as BoundSPC.
7. Click create to create the constraints.
8. Click return to go back to the main menu.
Step 7: Define a *SET_SEGMENT for the slave entities, the A-pillar elements

1. From the BCs drop down menu, select Create and select Contact Surfaces.
2. For name = type pillar_slave.
3. For the card image select setSegment.
4. Optionally select a color for the contactsurf.
With the elems selector active, select elems and select by collector and then select the pillar
5. component.
6. Click create to create the contactsurf.
7. Review the contactsurf to make sure its pyramids are pointing out of the pillar.
8. Stay in this panel for the next step.
Step 8: Define a *SET_SEGMENT for the master entities, the head elements

1. Select the solid faces sub-panel.

2. For name = type head_master.
3. For the card image = select setSegment.
4. Optionally select a color for the contactsurf.
With the elems selector active, select elems and select by collector and then select the head
5. component.
6. Leave the toggle set to nodes on face.
7. Click the yellow nodes selector to make it active.
8. Select three nodes belonging to the same face of a solid element.
9. For the break angle, leave it set to 30.
10. Click create to create the contactsurf.
11. Review the contactsurf to make sure its pyramids are pointing out of the head.
12. Click return to go back to the main menu.
Step 9: Create a HyperMesh group with the SurfaceToSurface card image

1. Access the interfaces panel in one of the following ways:

• From the BCs drop down menu, select Create and click Interfaces
• From the Analysis page, click interfaces
2. Go to create sub-panel.
3. For name = type contact.
4. For type = select SurfaceToSurface.
5. Click create to create the group.
6. Stay in the interfaces panel for the next step.
Step 10: Add the slave and master contactsurfs to the HyperMesh group

1. Select the add sub-panel.

2. For the master type select csurfs.
3. Click the contactsurfs selector and select the head_master contactsurf.
4. Click update in the master: line, to the right of the yellow contactsurfs selector.
5. For the slave type select csurfs.
6. Click the contactsurfs selector in the slave: line and select pillar_slave.
7. Click update in the slave: line.
8. Stay in the interfaces panel for the next step.
Step 11: Edit the group’s card image to define the AUTOMATIC option

1. Select the card image sub-panel.

2. Click edit to edit the group’s card image.
3. Under Options, click the toggle to select Automatic.
4. Click return to go back to the main menu.
5. Stay in the interfaces panel for the next step.
Step 12: Review the group’s master and slave surfaces

1. Select the add sub-panel.

2. For name =, select contact.
3. Click review.
4. Notice the master and slave entities are temporarily displayed blue and red, respectively.
5. Click return to go back to the main menu.
The exercise is complete. Save your work to a HyperMesh file.

Section 3: Define Control Cards and Specify Output

*CONTROL and *DATABASE

The *CONTROL cards are optional and can be used to change defaults and activate solution
options, such as mass scaling, adaptive meshing and an implicit solution. It is advisable to
define *CONTROL_TERMINATION in a model to specify a job’s end time.
The *DATABASE cards are optional, but are necessary to obtain output files containing
results.
In HyperMesh, with the exception of the cards listed in the table below, all *CONTROL and
*DATABASE cards are created from the control cards panel from either the Setup menu or the
Analysis page.

*DATABASE cards NOT created from control cards panel

DYNA card Panel used to create card

*DATABASE_CROSS_SECTION_(Option) PLANE option, rigid walls panel

SET option, interfaces panel

*DATABASE_HISTORY_(Option) output blocks panel

*DATABASE_NODAL_FORCE_GROUP interfaces panel

Exercise 3: Define Termination and Output for the Head and A-Pillar Impact Analysis

The purpose for this exercise is to help you becoming familiar with defining LS-DYNA control
data and output requests using HyperMesh.
This exercise comprises of defining the termination and output for an LS-DYNA analysis of a
hybrid III dummy head impacting an A-pillar. The head and A-pillar model is shown in the
image below.

Head and A-pillar model

This exercise contains the following four tasks.

Specify the time at which LS-DYNA is to stop the analysis with

• *CONTROL_TERMINATION
• Specify ASCII output with *DATABASE_(Option) cards
• Specify the output of d3plot files with *DATABASE_BINARY_D3PLOT
• Export the model to an LS-DYNA 970 formatted input file
Step 1: Make sure the LS-DYNA user profile is still loaded

Step 2: Retrieve the HyperMesh file head_3.hm

Step 3: Specify the time at which you want LS-DYNA to stop the analysis with
*CONTROL_TERMINATION

1. The control cards panel can be accessed by one of the following ways,
- From the Setup drop down menu, click Create and Control Cards
- From the Analysis page, click control cards
2. Click next to scroll through the list and go to the next page.
3. Select CONTROL_TERMINATION.
A card image pops up.

4. For the termination time of the analysis, ENDTIM, specify 2.5.

5. Click return to go back to the control cards panel.
Step 4: Specify the output of d3plot files with *DATABASE_BINARY_D3PLOT

1. Click next to scroll through the list and go to the next page.
2. Select DATABASE_BINARY_D3PLOT.
3. For the interval between outputs in the D3PLOT file, [DT] field, specify 0.1.
4. Click return to go back to the control cards panel.
Step 5: Specify ASCII output with *DATABASE_(Option) cards

1. Click next to scroll through the list and go to the next page.
2. Select DATABASE_OPTION.
3. For the GLSTAT file, [GLSTAT] field, specify 0.1.
This specifies the output of global data at every 0.1 ms.

4. For the MATSUM file, [MATSUM] field, specify 0.1.

This specifies the output of material energies every 0.1 ms.

5. For the SPCFORC file, [SPCFORC] field, specify 0.1.

This specifies the output of SPC reaction forces every 0.1 ms.

6. Click return to go back to the control cards panel.

7. Click return to go back to the main menu.
Step 6: Export the model as an Ls-Dyna keyword file

1. From the File drop down menu, select Export...

2. Make sure LS-DYNA is selected as the File type: and the appropriate template is selected.
3. Enter the file name as head_complete.key.
4. Click Apply.
Step 7 (Optional): Submit the LS-DYNA input file to LS-DYNA 970

1. From the desktop’s Start menu, open the LS-DYNA Manager program.
2. From the solvers menu, select Start LS-DYNA analysis.
3. Load the file head_complete.key.
4. Click OK to start the analysis.
Step 8 (Optional): Post-process the LS-DYNA results using HyperView

The exercise is complete. Save your work to a HyperMesh file.