RD-T: 3595 Three Point Bending with HyperMesh

This tutorial demonstrates how to set up 3-point bending model with symmetric boundary conditions in Y direction.


rd3595_3point_bending
Figure 1.

Model Description

  • UNITS: Length (mm), Time (s), Mass (ton), Force (N) and Stress (MPa)
  • Simulation time: in Engine file [0 - 6.601e-002 s]
  • Only one half of the model is modeled because it is symmetric.
  • The supports are totally fixed. An imposed velocity of 1000 mm/s is applied on the Impactor in the (-Z) direction
  • Model size = 370mm x 46.5mm x 159mm
  • Honeycomb Material /MAT/LAW28: HONEYCOMB

    [Rho_I] Initial density = 3.0e-10ton/mm3

    [E11], [E22] and [E33] Young's modulus (Eij) = 200 MPa

    [G11], [G22] and [G33] Shear modulus (Gij) = 150 MPa

  • Elasto-Plastic Material /MAT/LAW36: Inner, Outer and Flat

    [Rho_I] Initial density = 7.85-9ton/mm3

    [E] Young's modulus = 210000 MPa

    [nu] Poisson's ratio = 0.29

  • Strain Curve:
      0 1 2 3 4 5 6 7 8 9
    STRAIN 0 0.012002 0.014003 0.018003 0.022002 0.026003 0.030006 0.032 0.033005 0.033523
    STRESS 325 335.968 343783 349.245 358.649 372.309 383.925 388.109 389.292 389.506
  • Elastic Material /MAT/PLAS_JOHNS: Impactor

    [Rho_I] Initial density = 8e-9ton/mm3

    [E] Young's modulus = 208000 MPa

    [nu] Poisson's ratio = 0.29

Load the Radioss User Profile

  1. Launch HyperWorks Desktop.
  2. From the Preferences menu, select User Profiles or click the userProfile-24 icon in toolbar.
  3. Select Radioss (Block140) and click OK.

Open the Model File

  1. Click the Open Model icon fileOpenModel-24 to open the BENDING_0000.rad file you saved to your working directory from the radioss.zip file.
  2. Click Open.
    The model loads into the modeling window.

Create and Assign the Material and Property for HCFOAM

  1. In the Model Browser, right-click and select Create > Material.
    The new material appears in the Entity Editor.
  2. For Name, enter Foam.
  3. For Card Image, select M28_HONEYCOMB and click Yes to confirm.
  4. Input values, as shown below:

    rd3595_foam_13
    Figure 2.
  5. In the Model Browser, right-click and select Create > Property to create a new property.
  6. For Name, enter Foam and set the new property Card Image as P14_SOLID. Leave all the settings as default, except for ISOLID which should be set to 24.
  7. In the Model Browser, right-click on the component HCFoam and select Assign. Assign Foam as the Prop_Id and Foam as the Mat_Id.
  8. Click Apply.

Create and Assign the Material and Property for Inner

  1. In the Model Browser, right-click and select Create > Material.
    The new material appears in the Entity Editor.
  2. For Name, enter Inner.
  3. For Card Image, select M36_PLAS_TAB and click Yes to confirm.
  4. Input the values, as shown below:

    rd3595_inner_14
    Figure 3.
  5. In the Model Browser, right-click and select Create > Property to create a new property.
  6. For Name, enter Inner and set Card Image as P1_SHELL. Leave all the settings as default, except for Ishell which should be set to 4 and Thick which should be set to 9.119e-01.
  7. In the Model Browser, right-click on the component Inner and select Assign. Assign Inner as the Prop_Id and Inner as the Mat_Id.

Create and Assign the Material and Property for Outer

  1. In the Model Browser, right-click on the material Inner and select Duplicate. Name the new material Outer.
    This creates a new material that is identical to the source material.
  2. In the Model Browser, right-click on the property Inner and select Duplicate. Name the new property Outer.
    This creates a new property that is identical to the source property.
  3. In the Model Browser, right-click on the component Outer and select Assign. Assign Outer as the Prop_Id and Outer as the Mat_Id.

Create and Assign the Material and Property for Impactor

  1. In the Model Browser, right-click and select Create > Material.
    The new material shows up in the Entity Editor.
  2. For Name, enter Impactor.
  3. For Card Image, select M1_ELAST.
  4. Input the values, as shown below:

    rd3595_impactor_13
    Figure 4.
  5. In the Model Browser, right-click on the property Inner and select Duplicate. Name the new property Impactor.
    This creates a new property that is identical to the source property.
  6. In the Model Browser, right-click on the component Impactor and select Assign. Assign Impactor as the Prop_Id and Impactor as the Mat_Id.

Create a Rigid Body for Impactor and Support

  1. In the Model Browser, right-click and select Create > Component.
  2. For Name, enter Impact rigid.
  3. Click Color and select a color from the color palette.
  4. Set Card Image to None.
  5. Go to the 1D page and select the rigids panel.
  6. Verify that you are in the create subpanel.
  7. For dependent, switch to comps.
  8. For primary node, switch to calculate node.
  9. Click comps.
  10. Select Impactor, then click select.
  11. Click create.
  12. Click return to exit the panel.
  13. Similarly, create rigid body for Support component in a collector with the name Support rigid using steps 1 to 12.

    rd3595_impact_rigid
    Figure 5.

Define the Imposed Velocity and Boundary Condition for the Impactor

  1. From the Utility menu, start the BCs Manager.
  2. For Name, enter IMPOSED_VELOCITY, set Select type to Imposed Velocity and set the GRNOD to Nodes.
  3. Click nodes and select the master node of the rigid body of the Impactor, as shown in the following image.

    rd3595_impvel
    Figure 6.
  4. Set the Direction as Z.
  5. Set Scale Y to -1000.0 as the direction of velocity is opposite to the global Z-axis.
  6. Set the Curve ID to Select curve.
  7. Select the predefined curve to Func1.
  8. Click create to create the imposed velocity.

    rd3595_imposedvel_10SA1
    Figure 7.
  9. For Name, enter Impactor_constraints, set Select type to Boundary Condition and set the GRNOD to Nodes.
  10. Click nodes and select the master node of the rigid body.
  11. Check all the degrees of freedom to constrain, except Tz.
  12. Click create to create the boundary condition.

Define the Fixed Boundary Condition for Support

  1. From the Utility menu, start the BCs Manager.
  2. For Name, enter Support_fixed, set Select type to Boundary Condition and set the GRNOD to Nodes.
  3. Select the master node of the rigid body created on Supporter, as shown in the following image.
  4. Check all the degrees of freedom.
  5. Click create to create the boundary condition.

    rd3595_impvel
    Figure 8.

    rd3595_supportfix_13
    Figure 9.

Define the Symmetry Boundary Condition for Foam, Inner, Outer and Flat

  1. From the Utility menu, start the BCs Manager.
  2. For Name, enter SYMMETRY_XZ, set Select type to Boundary Condition and set the GRNOD to Nodes.
  3. Select the nodes of the foam, inner, outer and flat, as shown in the following image.
  4. Check the translational degrees of freedom Y and rotational degrees of freedom X and Z to constraint.
  5. Click create to create the boundary condition.

    rd3595_symmetry_xz
    Figure 10.

    rd3595_symmetry_13
    Figure 11.
  6. Click close to exit the BC Manager.

Define the Contacts between Beam and Support

  1. Launch the Solver Browser by clicking View > Browsers > HyperMesh > Solver.
  2. In the Solver Browser, right-click and select Create > INTER > TYPE7.
  3. Enter the values, as shown below:

    rd3595_support_13
    Figure 12.
  4. Set the Surf_id (M) for the master selection to Components and select the Support component.
  5. Set the Grnod_id (S) for the slave selection to Components and select the Flat component.
  6. Similarly, create the contact for Impactor with Outer, as shown below.

    rd3595_impactor2_13
    Figure 13.

Define the Self Contact between the Beam Components

  1. Using the directions in Define the Contacts between Beam and Support, create a new Type 7 interface named Self with the components Outer, Inner, and Flat as Master and the same components Outer, Inner, and Flat as Slave.
    This will make the components self-contact instead of self-penetrate.
  2. Verify that the interface has a Fric of 0.1 and Gapmin of 0.2.

    rd3595_self_13
    Figure 14.

Create the Interface Time History

  1. Right-click in the Solver Browser and select Create > TH > INTER.
  2. For Name, enter IMPACTOR.
  3. Switch the entity selector to groups.
  4. Click groups and select the interfaces Impactor and Support from the list.
  5. Click OK.
  6. Set NUM_VARIABLES to 1 and Data: Var to DEF.

    rd3595_impactor_14
    Figure 15.

Create Output Request and Control Cards

  1. Launch the HyperMesh Solver Browser from View > Browsers > HyperMesh > Solver.
  2. Right-click in the Solver Browser general area to create the cards, shown below with the given values for each parameter:
    Keyword Type Keyword Parameter Parameter Value
    CONTROL CARDS TITLE Status [Checked]
    CONTROL CARDS TITLE TITLE 3PBENDING
    ENGINE KEYWORDS RUN Status [Checked]
    ENGINE KEYWORDS RUN RunName 3PBENDING
    ENGINE KEYWORDS RUN RunName 1
    ENGINE KEYWORDS RUN Tstop 7.01e-2
    ENGINE KEYWORDS TFILE Status [Checked]
    ENGINE KEYWORDS TFILE Time_frequency 0.0001
    ENGINE KEYWORDS PRINT Status [Checked]
    ENGINE KEYWORDS PRINT N_Print -100
    ENGINE KEYWORDS ANIM/ELEM Status [Checked]
    ENGINE KEYWORDS ANIM/ELEM VONM [Checked]
    ENGINE KEYWORDS ANIM/ELEM EPSP [Checked]
    ENGINE KEYWORDS ANIM/VECT Status [Checked]
    ENGINE KEYWORDS ANIM/VECT VEL [Checked]
    ENGINE KEYWORDS ANIM/VECT CONT [Checked]
    ENGINE KEYWORDS ANIM/DT Status [Checked]
    ENGINE KEYWORDS ANIM/DT Tstart 0
    ENGINE KEYWORDS ANIM/DT Tfreq 2.5e-3
    ENGINE KEYWORDS DT Status [Checked]
    ENGINE KEYWORDS DT Tscale 0.0
    ENGINE KEYWORDS DT Tmin 0.0
    ENGINE KEYWORDS DT/NODA Status [Checked]
    ENGINE KEYWORDS DT/NODA CST_0 [Checked]
    ENGINE KEYWORDS DT/NODA/CST_0 Tscale 0.9
    ENGINE KEYWORDS DT/NODA/CST_0 Tmin 7e-7
    ENGINE KEYWORDS DT/NODA DEL [Checked]
    ENGINE KEYWORDS DT/NODA/DEL Tscale 0.9
    ENGINE KEYWORDS DT/NODA/DEL Tmin 3.5e-8
    ENGINE KEYWORDS RBODY_ENGINE RBODY/ON Status [Checked]
    ENGINE KEYWORDS RBODY_ENGINE NUM_rbnodes 2
    ENGINE KEYWORDS RBODY_ENGINE Data: Nodes 29664

    29665

Export the Model

  1. Click File > Export or click the Export icon .
  2. Click the folder icon and navigate to the destination directory where you want to export to.
  3. For Name, enter 3BENDING and click Save.
  4. Click the downward-pointing arrows next to Export options to expand the panel.
  5. Select Merge starter and engine file to export both the Starter and Engine file in one file.
  6. Click Export to export the file.

Run the Model in the Solver

  1. Go to Start > Programs > HyperWorks 2019 > Radioss.
  2. For Input file, browse to the exercise folder and select the file 3PBENDING_0000.rad.
  3. Click Run.

Review the Results

  1. See if there are any warnings or errors in .out files.
  2. Using HyperView, plot the displacement, strain contour and vectors.