HyperWorks Solvers

RD-3510: Cantilever Beam with Bolt Pretension

»Click here to display Table of Contents« RADIOSS > Tutorials and Examples > Tutorials > Large Displacement Finite Element Analysis > HyperMesh:

RD-3510: Cantilever Beam with Bolt Pretension
RD-3510: Cantilever Beam with Bolt Pretension

This tutorial demonstrates how to simulate a simple cantilever problem with a concentrated load at the free end, using Dynamic Relaxation (/DYREL) method to obtain a static solution.

rd3510_cantilever_13

Model Description

•	UNITS: Length (mm), Time (ms), Mass (kg), Force (kN) and Stress (GPa)

•	Simulation time:

o	CANTILEVER_0000.rad [0 – 25.1 ms]

•	Steps to setup this model:

o	Fix the Cantilever Beam to the support with a 10 kN pre-tension. The bolt attains 10 kN in 10 ms and remains constant thereafter.

o	After pre-tension, a concentrated load of 0.2 kN is gradually applied at the free end of the beam from 10 ms to 25 ms and it remains constant thereafter.

•	Material used:

Elasto-plastic material /MAT/LAW2.

[Rho_I] Initial density = 7.83e-6 Kg/mm3

[E] Young’s modulus = 205 GPa

[nu] Poisson’s ratio = 0.29

[a] Yield Stress = 0.792 GPa

[b] Hardening Parameter = 0.510 GPa

[n] Hardening Exponent = 0.26

[SIG_max] Maximum Stress = 0.95 GPa

[c] Strain rate coefficient = 0.014 GPa

[EPS_0] Reference strain rate = 1

Input file for this tutorial: CANTILEVER_0000.rad

Exercise

Step 1: Load the RADIOSS (Block) User Profile

1.	Launch HyperMesh Desktop.

2.	From the Preferences menu, select the User Profiles or from the toolbar, click the icon.

3.	Select RADIOSS (Block140) and click OK.

Step 2: Load the solver deck

1.	Click File > Import > Solver Deck or click .

2.	Click the Select File icon to open the CANTILEVER_0000.rad file you saved to your working directory from the radioss.zip file. Refer to Accessing the Model Files.

3.	Click Open.

4.	Click Import.

5.	Click Close to close the window.

Step 3: Create a rigid body connecting spring ends to Bolt Support component

1.	In the Model browser, right-click and select Create > Component.

A component is created and is shown in the Entity Editor (EE), below the Model browser.

2.	Using the Entity Editor (EE), change the Name to Rigids.

3.	Set the Card Image as None.

4.	In the Model browser, hide the component 1.

5.	Click the Mask icon in the toolbar.

6.	In the graphics area, select one element from the bolt.

rd3510_bolt_support

7.	Click on elems >> by attached to select the whole bolt.

8.	Click mask to hide them and click return.

9.	From the 1D page, select the rigids panel.

10.	Click the selector arrow nodes 2-n: and change it to multiple nodes.

11.	In the rigids panel, for primary node, select the node at the end of spring, as shown in Fig 1 below, and for nodes 2-n, select the nodes, as shown in Fig 2.

Note: Be sure to set the selector to multiple nodes.

rd3510_fig1

Fig 1

rd3510_fig2

Fig 2

12.	With all the DOF’s checked, click create to create the rigid body.

13.	Click the Mask icon in the toolbar and click reverse to show remaining elements of the bolt.

14.	Click return to exit the panel.

15.	In the Model browser, rght-click the 3 components and click Show to display onscreen, as shown below.

16.	Use Steps 3.10 through 3.12 to create a rigid body with the nodes shown in the following image with the other ends of the springs as the primary node and the nodes on the bolts as slave nodes.

rd3510_rigid

Step 4: Create and assign material, property to Plate and Support bolts

1.	In the Model browser, click the component 1. The component appears in the Entity Editor.

2.	Change the name of the component to Plate.

3.	Set Card Image to Part.

4.	In the Model browser, right-click and select Create > Material.

5.	For Name, enter Steel and set the Card Image to M2_PLAS_JOHNS_ZERIL and click Yes to confirm.

6.	Enter the values, as shown below.

rd3500_03

7.	In the Model browser, right-click and select Create > Property.

8.	For Name, enter Plate, and set the Card Image to P14_SOLID and click Yes to confirm.

9.	In the Model browser, click the component 2, the EE for the component opens.

10.	For Name, enter Bolt_Support.

11.	Set the Card Image to Part.

12.	For Prop_Id, click Unspecified > Property and select the property, Plate and click OK.

13.	For Mat_Id , click Unspecified > Material and select the material, Steel and click OK.

Step 5: Create and update properties for Pre-tensioner Spring

1.	In the Model browser, select the component 3, which opens the Entity Editor.

2.	For Name, enter Spring.

3.	Set the Card Image to Part.

4.	In the Model browser, right-click and select Create > Property. A new property is created and a dialog opens with the new property.

5.	Change the Name to Spring.

6.	Set the Card Image to P32_SPR_PRE and click Yes to confirm.

7.	Fill in the other values, as shown below:

rd3510_spring_13

8.	In the Model browser, click on the property Spring to open the Entity Editor.

9.	Right-click on IFUN2 and select Create to create and attach a curve. A Create Curve dialog opens.

10.	Change the Name of the curve to Stiffness.

11.	Click Close to exit the dialog.

12.	In the Model browser, select the curve Stiffness, right-click and select Edit from context menu.

13.	The XY curve editor appears. Fill in the values, as shown below.

rd3510_curve_editor_13

14.	Click Update > Close. The created curve is assigned to the property.

Step 6: Defining Boundary Conditions to fix bottom of the BOLT_SUPPORT

1.	From the Tools menu, start the BCs Manager.

2.	For Name, enter FIXED, set Select type to Boundary Condition and set GRNOD to Nodes.

rd3510_bc

3.	Click on the nodes, the nodes selection appears; by window option, select the bottom layer of the bolt support, as shown below and the selection should appear as shown below in the XY Plane view:

rd3510_entity_13

4.	Fix all translational degrees of freedom.

rd3510_bc_all

5.	Click Create to create the constraint. The created constraint appears in the table and a handle appears in graphics area.

Step 7: Defining the load (CLOAD) of the edge of the beam

1.	For Name, enter LOAD, set Select type to Concentrated Load and set GRNOD to Nodes.

2.	Select the nodes on the edge of the beam, as shown in the image below by window option.

rd3510_cload_13

3.	For Direction, select Y.

4.	Set Scale Y, to -1.0 to apply load in negative Y direction.

5.	Click the Create/Select curve tab. A GUI to enter curve appears.

6.	Create a curve with Name LOAD and enter the values, as shown below using the same procedure explained in Step 5.

x = {0, 10, 25, 250}

y = {0, 0, 0.02, 0.02}

7.	Click Update and Close in the XY curve editor GUI, the created curve is assigned to the BC.

8.	Click Create to finish the creation of the load at the selected nodes.

Step 8: Define a contact interface between Plate and Support_Bolt

1.	In the Model browser, right-click and select Create > Contact. A contact is created and the Entity Edit opens.

2.	Set Name as SELF.

3.	Set Card Image to TYPE7 and click Yes to confirm.

4.	Click on Grnod_id (S) in the EE and set the selector to Components.

5.	Pick the components Plate and Support_Bolt using the list selection dialog.

6.	Click on Surf_id (M) in the EE and set the selector to Components.

7.	Pick the components Plate and Support_Bolt using the list selection dialog.

8.	Set Igap to 0.

9.	For FRIC, enter 0.1 and for GAPmin, enter 0.04.

Step 9: Create time history to obtain displacement at free end

1.	In Model browser, right-click and select Create > Output Block From the Analysis page, select the output block panel.

2.	In the Entity Editor, set the name to Deflection and select the nodes on the free end of the cantilever, as shown in the following image:

rd3510_deflection_13

3.	Set NUM_VARIABLES to 1 and click on the Data:Var icon . A table will open, enter the variable name DEF.

4.	Click edit and enter the variable name DEF.

rd3510_deflection_14

Step 10: Create output request and control cards

For this exercise the output request will be generated from the Engine file assistant which is located in the Utility browser.

1.	To start the Engine file assistant, select Tools > Engine File Assistant.

2.	Input the values, as shown below:

rd3510_engine_file_assistant

Step 11: Run the model checker

1.	Click Tools > Model Checker > RadiossBlock to open the Model Checker tab.

2.	The Model Checker will display a list of perceived errors within the model.

For most of these issues, the Model Checker is equipped to auto-correct many issues, decreasing the possibility of a solver error.

3.	Click the Apply Auto Correction icon and click the Run icon to auto-correct issues within the model.

Step 12: Export the model

1.	Click File > Export or click the Export icon .

2.	For File:, click the folder icon and navigate to the destination directory where you want to export to.

3.	For Name, enter CANTILEVER 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.

Step 13: Run the model in the solver

1.	Go to Start > Programs > Altair HyperWorks 2017 > RADIOSS.

2.	For Input file, browse to the exercise folder and select the file CANTILEVER_0000.rad.

rd3510_radioss_mgr_13

3.	Post-process the results with HyperView.

4.	Using HyperGraph, open the T01 file and plot the deflection at the free end of the cantilever.

rd3510_results

See Also:

RADIOSS Tutorials