HM-4340: Pre-Processing for Bracket and Cradle Analysis

In this tutorial, you will learn how to set up an Abaqus input file in HyperMesh for obtaining the linear static response of a cradle and bracket assembly subjected to a 100 kN load on the bracket, with the cradle’s ends fully constrained.

You will learn how to:
  • View images of keywords and data lines in HyperMesh as they appear in the Abaqus input file
  • Create and edit Abaqus materials and section properties
  • Select Abaqus entity types for HyperMesh element and load configurations
  • Create loads and boundary conditions for model data (*KINEMATIC COUPLING and *BOUNDARY)
  • Create an Abaqus step containing title, analysis procedure, parameters, *CLOAD on bracket, and output requests
  • Export a model to an Abaqus formatted input file
Note: The units millimeters and kilonewtons (mm, kN) are used in this tutorial.

This exercise uses the bracket_cradle.hm file, which can be found in <hm.zip>/interfaces/abaqus/. Copy the file(s) from this directory to your working directory.

Load the User Profile and Model

In this step you will load the Abaqus user profile and model.

  1. Start HyperMesh Desktop.
  2. In the User Profile dialog, set the user profile to Abaqus, Standard3D.
  3. Open a model file by clicking File > Open > Model from the menu bar, or by clicking on the Standard toolbar.
  4. In the Open Model dialog, open the bracket_cradle.hm file.
    The bracket_cradle.hm file contains the following Abaqus model data:
    • ELSET bracket modeled with penta (C3D6) and hexa (C3D8) elements
    • ELSET cradle modeled with tria (S3) and quad (S4) elements
    • Two *KINEMATIC COUPLING entities at the bracket’s bottom bolt holes
    • Material named aluminum
    • *SOLID SECTION property for ELSET bracket with the aluminum material associated to it

Understand the Relationship between Abaqus and HyperMesh Entities

You can use HyperMesh card images to view images of keywords and data lines for defined Abaqus entities as interpreted by the loaded template. The keywords and data lines appear in the Abaqus 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 Abaqus keyword.

Review and edit card images by clicking on the Collectors toolbar. You can also review and edit the card image for many entities from the panel in which they are created. Most of the card images are also accessible from the Model Browser by right-clicking on the entity and selecting Card Edit from the context menu, or simply left-clicking on the entity displays it in the Entity Editor.

*ELEMENT with Sectional Property

The Abaqus keyword *ELEMENT, TYPE = <type>, ELSET = <name>, is defined by Abaqus elements collected in a HyperMesh component collector. One *ELEMENT keyword is written to the Abaqus input file for each element type in the component. The name of the ELSET is the name of the component.

If a property is assigned to a component, the ELSET name of that sectional property will be the name of the component collector. If properties are directly assigned to elements, HyperMesh will write an additional ELSET with the name of the property collector it is assigned to. The sectional property card will then point to this ELSET. Assignment of individual elements to a property takes precedence over assigning a component to a property. Individual element assignment is only recommended when the ratio of elements per component is very small. This is the situation explained in this tutorial.

The material referenced in the sectional property is defined by a HyperMesh material collector associated with the property collector. The diagram below shows how elements and its associated properties are organized in HyperMesh.


Figure 1.

Abaqus Materials in HyperMesh

An Abaqus *MATERIAL is a HyperMesh material collector with a card image.

There are four card images for the HyperMesh Abaqus templates: ABAQUS_MATERIAL, GASKET_MATERIAL (for the Standard templates), CONNECTOR_BEHAVIOR and GENERIC_MATERIAL. There are two ways to create a material collector and associate it to a component.

Method One: Drop-Down Menu
  • From the menu bar, create a material collector with a card image and edit it to define material data. By selecting the material while creating a property, it will automatically be assigned to the sectional property. As pointed out in the paragraph above, you can assign the property containing the sectional properties to a component or to individual elements. Assign properties to existing components or to individual elements, from the menu bar, by clicking Collectors > Assign > Component Properties or clicking Properties > Assign.
Method Two: Model Browser
  • In the Model Browser, while in either the model or material view, right-click and select Create to create a new material collector with the appropriate card image. If you select Create/Edit, the card image displays so you can set up all necessary parameters and keywords. Properties can also be created in this manner. You can directly assign the material to the new property by selecting the material in the Material name field.

Within the card image of each material card, it is possible to add as many data lines as you want for a material (such as *PLASTIC with yield stress, plastic strain, and temperature data). Manually enter the data in HyperMesh or import an Abaqus formatted input file on top of the model in HyperMesh to create the data lines.

Review the Card Image

In this step you will review the card image of one of the elements.

You will use the card editor panel to review elements, sectional properties, and materials as they appear in the Abaqus input file. Review and edit card images by clicking on an entity in the Model Browser and displaying it in the Entity Editor.

  1. Open the Card Edit panel by clicking Mesh > Card Edit > Elements from the menu bar.
  2. Verify that the entity selector is set to elems.
  3. Select an element from the bracket (blue elements).
  4. In the panel area, click edit.
    The card image for the element opens, and displays the element type (either C3D6 or C3D8) and the ELSET name as bracket.


    Figure 2.
  5. Click return to close the card image.

View the Property Card

In this step you will use the Entity Editor to view the sectional properties associated with the elements in the model's components.

In the Model Browser, Property folder, click bracket.
The Entity Editor opens, and displays the bracket’s *SOLID SECTION property and material assignment, which is aluminum.


Figure 3.

View the Material Collector Card

In this step you will use the Entity Editor to review the defined material, aluminum.

In the Model Browser, Material folder, click aluminum.
Then Entity Editor opens and displays the material's card data.


Figure 4.

Create the Material STEEL

In this step you will create a *MATERIAL with *ELASTIC to define as steel for the ELSET cradle. When you define the sectional property for the cradle component in the next section, the material will already be referenced in the property.

  1. In the Model Browser, right-click and select Create > Material from the context menu.
    HyperMesh creates and opens a material in the Entity Editor.


    Figure 5.
  2. For Name, type steel.
  3. Select the Elastic checkbox.
    This creates *ELASTIC.
  4. In the E field, type 200.
  5. For Poisson's ratio NU, type 0.3.

Assign the Material to the Component

In this step you will assign the material, Steel, to the component and define *SHELLSECTION for the cradle property.

  1. In the Model Browser, right-click and select Create > Property from the context menu.
    HyperMesh creates and opens a property in the Entity Editor.


    Figure 6.
  2. For Name, type cradle.
  3. For Material Name, click Unspecified >> Material.


    Figure 7.
  4. In the Select Material dialog, select steel and click OK.


    Figure 8.
  5. For Thickness, type 2.5.
  6. In the Model Browser, Component folder, right-click on cradle and select Assign from the context menu.
  7. In the Assign to Component(s) dialog, select cradle from the Property list.


    Figure 9.
  8. Click OK.

Understand HyperMesh Entity Configurations and Types

HyperMesh elements and load entities have two identifiers: configuration and type.

The entity configuration is a HyperMesh core feature while the entity type is defined by the template. For example, HyperMesh element configurations include rigid, spring, quad4, and hex8. Possible quad4 configuration types in the Standard3D template include S4, S4R, S4R5, among others. Similarly, HyperMesh load configurations include constraints, force, pressure, and temperature. In the HyperMesh Abaqus templates, pressure configuration types include DLOAD, DFLUX, FILM, DECHARGE and Radiate.

Most of the HyperMesh element and load configurations have their own panels. From the 1D, 2D, and 3D pages, use the Elem Types panel. Load types can be chosen directly in the related panels. You can also use the load or element types panels to change the type of load.

Kinematic Constraints in HyperMesh

With the exception of *EQUATION, Abaqus kinematic constraints, such as *KINEMATIC COUPLING and *MPC (BEAM, TIE, LINK, PIN), are rigid (1D) elements in HyperMesh. From the 1D page, use the Rigids panel to create them. Organize them into HyperMesh component collectors. No sectional property or material is needed for these entities. Hence, either organize them into their own component or into a component containing different Abaqus entities.

In the next few steps, you will create the Abaqus constraint *KINEMATIC COUPLING to simulate a bolt connecting the bracket’s top bolt hole to the cradle. The model already contains two *KINEMATIC COUPLING entities, one at each of the bracket’s bottom bolt holes. They are organized into the bracket component.

You will start by creating a new component in which you will organize all the *KINEMATIC COUPLING entities. This is not necessary, but is done to organize the data and demonstrate the selection of entities by configuration. This component will contain the *KINEMATIC COUPLING to be created. You will need to select any existing material to avoid creating one that is not needed.

Be sure to use the Elem Types panel to set the type for rigids to KINCOUP. This allows all elements created from the Rigids panel to be of the type *KINEMATIC COUPLING.

Finally, you will create the *KINEMATIC COUPLING using the Rigids panel.

Create a New Component Collector

In this step you will create a new component collector and set the element type rigid to KINCOUP.

  1. In the Model Browser, right-click and select Create > Component from the context menu.
    HyperMesh creates and opens a component in the Entity Editor.
    Note: This new component is now the current component. HyperMesh will automatically organize any new elements/geometry into this component.


    Figure 10.
  2. For Name, type connection.
  3. Click the Color icon and select a color for the component.
  4. Open the Element Type panel by clicking Mesh > Assign > Element Type from the menu bar.
  5. Go to the 1D subpanel.
  6. Click rigid= and select KINCOUP.
  7. Click update.
  8. Click return.

Create a Reference Node

In this step you will use the Distance panel to create a node at the center of the bolt hole to be the *KINEMATIC COUPLING reference node.

  1. Zoom into the top bolt hole as indicated in the following image.
  2. Open the Distance panel by pressing F4.
  3. Go to the three nodes subpanel.
  4. Select the three nodes on the top side of the bolt hole for N1, N2, and N3 as indicated in the image below.


    Figure 11.
  5. Click circle center.
    HyperMesh creates a node at the center of the selected nodes.
  6. Click return.

Move the *KINEMATIC COUPLING Entities

In this step you will move all of the *KINEMATIC COUPLING entities into the connection component using the Organize panel.

  1. Open the Organize panel by clicking Mesh > Organize > Elements > To Component from the menu bar.
  2. Click elems >> by config.
  3. Click config= and select rigidlink.
  4. Click type= and select KINCOUP.
  5. Switch the displayed/all toggle to all.
  6. Click select entities.
    HyperMesh selects all rigid links in the model.


    Figure 15.
  7. Click dest component= and select connection.
  8. Click move.
    HyperMesh moves all rigid links to the connection component.


    Figure 16.
  9. Click return.
    All *KINEMATIC COUPLING entities are now organized into the connection component. Model data definition is complete.

Use Step Manager for Initial Conditions

In HyperMesh, you can use the Step Manager tool to create, edit, review, re-order, and delete Abaqus initial conditions and steps.

You can open the Step Manager by clicking Tools > Loadsteps Browser > from the menu bar.


Figure 17.

The Step Manager has a default step named Initial Condition. This step is used to create boundary conditions and loads (initial conditions) in the model data portion of the Abaqus input file.

When you edit the Initial Condition step, the Load Step: Initial Condition dialog opens. You can only select valid boundary conditions and load types for model data in this dialog.


Figure 18.
Use this dialog from left to right by:
  • Selecting a load step type from the list (left column)
  • Creating a load collector (center area)
  • Creating the loads using the menu area (right side)

Define *BOUNDARY

In this step you will create constraints at the cradle’s ends using the Step Manager.

You will define the constraints as model data, not history data, by editing the Step Manager’s default step named Initial Condition. For this step, you will create a load collector and then create the constraints.

  1. Open the Load Step Manager by clicking Tools > Loadsteps Browser from the menu bar.
  2. In the Step tab, click Initial Condition.
  3. Click Edit to modify the step.
  4. In the Load Step: Initial Condition dialog, select Boundary from the first pane.
    Note: This specifies the type of initial condition you want to create.


    Figure 19.
  5. Click New to create a new load collector.
  6. In the Create Load Collector dialog, Name field, type constraints.


    Figure 20.
  7. Click Create.
  8. In the Load Collector table, select the Display checkbox for the constraints load collector.
  9. Optional: Next to the Display checkbox, click the Color box and select a color for the load collector.
  10. In the Load Collector table, click constraints.
    The collector becomes active, and new tabs appear on the right side of the dialog.


    Figure 21.
  11. In the Define tab, set Type to default (disp).
  12. Click Define from 'Constraints' panel.
    The panel opens.
  13. From the Standard Views toolbar, click .
  14. In the Constraints panel, click nodes >> by window.
  15. With the exception of the nodes at the ends of the cradle, draw a rectangle around all of the displayed nodes to select them as shown below.


    Figure 22.
  16. Select the exterior checkbox then click select entities.
    HyperMesh selects all nodes outside the window you drew.


    Figure 23.
  17. Constrain the selected nodes in all six directions by selecting all dof (degree of freedom) checkboxes.
  18. Click create.
    HyperMesh creates the constraints.


    Figure 24.
  19. Click return to go back to the Step Manager.
  20. Exit the Initial Condition step and return to the Step Manager by clicking close.

Define History Data

The history data portion of the Abaqus input file defines the sequence of events for the simulation.

The loading history is divided into a series of steps. Each step contains the type of simulation, loads, constraints, output requests, and contacts (for Abaqus Explicit). The Abaqus *STEP option marks the start of a step, while the *END STEP option marks the end.

In the Step Manager you can create, review, edit, delete, and re-order the Abaqus steps. In the Step Manager, loads are organized into load collectors and output requests are organized into HyperMesh output blocks.

Define the Abaqus Step

For this analysis, you will be looking at the linear static response of the cradle and bracket assembly to a 100 kN load applied on the bracket, with the cradle’s ends fully constrained.

This is a single event, therefore only one Abaqus step is needed. In this step you will use the Step Manager to define the step's title, heading, parameters, and the analysis procedure, and then apply a concentrated force (*CLOAD) on the bracket’s arm.

  1. In the Step Manager, Step tab, click New.
  2. In the Create New Step dialog, Name field, type step1.
  3. Click create.
    HyperMesh creates a new step.
  4. In the first pane, click Title.
    Additional options display, from which you can define the step's title.
  5. Select the Step heading checkbox and type 100kN load.
  6. Click Update.
  7. In the first pane, click Parameter.
  8. Write the step's name to the Abaqus input file by selecting the Name checkbox.
  9. Set the analysis for small-scale, linear deformations by selecting the Perturbation checkbox.
  10. Click Update.
  11. In the first pane, click Analysis procedure.
  12. Set Analysis type to static.
  13. Click Update.
  14. Click Text to review what has been defined so far for the step.


    Figure 25.
  15. When you are finished reviewing the contents of the window, click Close.
  16. In the first pane, expand Concentrated loads and click CLOAD-Force.
  17. Click New to create a new load collector.
  18. In the Create Load Collector dialog, Name field, type force.
  19. Click Create.
  20. Optional: Next to the Display checkbox, click the Color box and select a color for the load collector.
  21. In the Load Collector table, click force.
    The collector becomes active, and new tabs appear on the right side of the dialog for the selected load type (CLOAD-Force).


    Figure 26.
  22. In the Define tab, click Define from ‘Forces’ Panel.
    HyperMesh opens the Forces panel, from which you can create a CLOAD.
  23. Select the central node on the top side of the bracket's arm as indicated in the following image.


    Figure 27.
  24. In the magnitude= field, type -100.
  25. Leave the system selector set to global system.
  26. Set the orientation selector to z-axis for the force's direction vector.
  27. Click create.
    HyperMesh creates the force.


    Figure 28.
  28. Click return to go back to the Step Manager.

Specify Output Requests

In this step you will use the Step Manager to specify displacement and stress results to output to the .odb and .fil results files for step1. You will then export the model to an .inp file.

  1. In the first pane of the Load Step dialog, expand Output request and click ODB file.
  2. Click New to create a new output block.
  3. In the Create Output block dialog, Name field, type step1_output.
  4. Click Create.
  5. In the Output block table, click step1_output.
  6. From the Output tab, select the Output checkbox.
  7. Leave Output set to field.
  8. Select the Node output and Element output checkboxes.


    Figure 29.
  9. Click the Node Output tab. From this tab you can specify the nodal displacement output for the .odb file.
  10. From the list of output options, expand Displacement and select the U checkbox.


    Figure 30.
  11. Click Update.
  12. Click the Element Output tab. From this tab you can specify elemental stress output for the .odb file.
  13. From the list of output options, expand Stress and select the S checkbox.


    Figure 31.
  14. Click Update.
  15. In the first pane of the Load Step dialog, expand Output request and select Result file (.fil).
    Note: The output block, step1_output, is still highlighted (active) in the Output block table.


    Figure 32.