OS-T: 1394 Axi-Symmetric Ball Joint

This tutorial demonstrates how to carry nonlinear analysis for Axi-symmetric ball joint for pull load of 10,000N using OptiStruct.

Figure 1 illustrates the structural model used for this tutorial: Simplified model of Ball joint consisting of ball stud, ball joint housing and a bolt. It is represented as 2D axisymmetric model.


Figure 1. Model and Loading Description
Analysis with a portion of the full model with axi-symmetry boundary conditions. The following exercises are included:
  • Set up the Ball Joint 2D axi symmetric analysis in HyperMesh
  • Submit the job in OptiStruct
  • View results in HyperView

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Open the Model

  1. Click File > Open > Model.
  2. Select the Ball_Joint_2D_Axisymmetry.hm file you saved to your working directory from the optistruct.zip file. Refer to Access the Model Files.
  3. Click Open.
    The Ball_Joint_2D_Axisymmetry.hm database is loaded into the current HyperMesh session, replacing any existing data.

Set Up the Model

Mesh the Model with CQAXI Elements

The meshed 2D part has CQUAD4 elements and for axisymmetric model CQAXI elements are used.

  1. Select 2D panel > Element Types.
  2. Activate the 2D&3D panel.
  3. Click CQUAD4, select CQAXI.


    Figure 2. Change Element Type
  4. Click elements > displayed.
    All the elements displayed are selected.
  5. Click update and return.
  6. From the 2D&3D panel, select elements > displayed.
  7. Click review and return.
    Element type is verified.


    Figure 3. CQAXI Element Type

Create Contact Surfaces

This step creates the main surface for the ball stud.

  1. In the Model Browser, right-click and select Create > Contact surface from the context menu.
  2. For Name, enter main.
  3. In the Entity Editor, click on the elements, and select add shell edges > free edges and select the edge of the ball stud where it is in contact with the housing.


    Figure 4. Selection of 2D Elements for Contacts
  4. Deselect the elements which are not in contact with the housing, select reverse normal and click add.
    The main surface is now created.
  5. In the Model Browser, right-click and select Create > Contact surface from the context menu.
  6. For Name, enter secondary.


    Figure 5. Secondary Contact Elements for Housing
  7. In the Model Browser, right-click and select Create > Contact surface from the context menu.
  8. For Name, enter Main_ball_Stud.
  9. Select the elements of the ball stud which are in contact with the bolt using shell edges.
  10. Similarly create a contact surface for bolt and rename it to Secondary_bolt.


    Figure 6. Main and Secondary Contact Elements for Ball Stud and Bolt
    Tip: To deselect elements, toggle from free edges to elements and deselect elements which are not in contact using the Shift and left mouse button.
    The contact surfaces for contact between ball stud and bolt is accomplished.

Create the Contacts

First, you will create the contact between ball stud and housing, then the contact between bolt and ball stud.

  1. In the Model Browser, right-click and select Create > Contact from the context menu.
  2. For Name, enter CONTACT1.
  3. For Property Option, select static coeffic friction in the Entity Editor.
  4. For MU1, enter 0.2.
  5. For SSID (Secondary), select Contactsurf from the drop-down menu and select Secondary surface.
  6. For MSID (Main), select Contactsurf from the drop-down menu and select main (contact surface).
  7. In the Model Browser, right-click and select Create > Contact from the context menu.
  8. For Name, enter TIE.
  9. For Card Image, select TIE.
  10. For SSID (Secondary), select Secondary_bolt from the drop-down menu.
  11. For MSID (Main), select Main_ball_stud from the drop-down menu.

Create the Material

  1. In the Model Browser, right-click and select Create > Material from the context menu.
  2. For Name, enter MAT1.
    A new material, MAT1 has beeen created.
  3. For Card Image, select MAT1.
  4. For NU (Poisson's Ratio), enter 0.3.
  5. Enter the material values next to the corresponding fields.


    Figure 7. Material Properties

Create the Properties

  1. In the Model Browser, right-click and select Create > Property from the context menu.
  2. For Name, enter PAXI.
  3. For Card Image, select PAXI.
  4. For Material, select MAT1.


    Figure 8. Element Property
  5. In the Property tab, click on the component ball_stud, click property and select PAXI.
  6. In the Property tab, click on the component ball, click property and select PAXI.
  7. In the Property tab, click on the component housing, click property and select PAXI.


    Figure 9. Assign Property to Components

Apply Loads and Boundary Conditions

Create SPCs Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
    A default load collector displays in the Entity Editor.
  2. For Name, enter SPC1.
  3. Click BCs > Create > Constraints to open the Constraints panel.
  4. Select the edge of ball stud edges of 2D Axisymmetric and for only dof-1 (Translational X is fixed), enter 0.
  5. Click Create.


    Figure 10. Constraints for Ball Stud
  6. In the Model Browser, right-click and select Create > Load Collector from the context menu.
  7. For Name, enter SPC2.
  8. Click BCs > Create > Constraints to open the Constraints panel.
  9. Select free edges of housing, as shown in Figure 11 and select all dof 1, 2, 3, 4, 5, 6 and enter a value of 0.
    All degrees of freedom are fixed.
  10. Click return.


    Figure 11. Constraints for Housing
  11. In the Model Browser, right-click and select Create > Load Collector from the context menu.
  12. For Name, enter SPCADD.
  13. For Card Image, select SPCADD.
  14. For SPCADD_NUM_SET, enter 2.
  15. In data set, select SPC1 and SPC2.


    Figure 12. SPCADD
  16. Similarly, create load new load collectors and enter the names as NLPARM, NLADAPT and NLOUT.
  17. For Card Images, select the values shown below.


    Figure 13. NLPARM, NLADAPT and NLOUT

Create Force Load Collector

This step will outline how to apply the force.

  1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
  2. For Name, enter Force.
  3. Click BCs > Create > Force to open the Force panel.
  4. Toggle to faces and select face of ball stud.
  5. Toggle back to nodes and deselect nodes.
    Note: Use the Shift + right-mouse button.
  6. Select only the nodes shown in Figure 14.
  7. For Magnitude, enter 1000, select y-axis, and click create.


    Figure 14. Apply Force (Pull Load)
    Tip: To deselect nodes, toggle to nodes and deselect nodes for which forces are not applied.

Create Load Steps

  1. In the Model Browser, right-click and select Create > Load Step.
    A default load collector displays in the Entity Editor.
  2. For Name, enter Ball_Joint.
  3. Expand Subcase Definition, and for Analysis type, select Non-linear static.
  4. For SPC, select SPCADD.
  5. For LOAD, select Force.


    Figure 15. Create Load Step

Define Output Control Parameters

  1. From the Analysis page, select control cards.
  2. Click on GLOBAL_OUTPUT_REQUEST.
  3. Below CONTF, DISPLACEMENT, STRAIN and STRESS, set Option to Yes.
  4. Click return twice to go to the main menu.

Submit the Job

  1. From the Analysis page, click the OptiStruct panel.

    OS_1000_13_17
    Figure 16. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter Ball_Joint for filename.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to submit the job.

View the Results

  1. Once you receive the message Process completed successfully in the command window, click HyperView.
  2. Open the results and plot the displacement and the von Mises stress contour at 100% load.
  3. On the toolbar, click resultsContour-16 (Contour).
  4. Under Result type, from the first drop-down menu, select Displacement.
  5. Click Apply.


    Figure 17. Contour Panel
    Contour of displacement plot is observed at end of load factor.


    Figure 18. Displacement Contour
  6. Toggle to element 2D & 3D stresses and click Apply.
  7. To view results of solid model from axisymmetric model, click from the panels window.
  8. For Specify axisymmetry axis, select Y.
  9. For Count, enter 20.
  10. For Total angle, enter 180 and click Apply.


    Figure 19. Rotate Axisymmetric Elements


    Figure 20. Element Stress Results by using Symmetry of Rotations