1. Axisymmetric Analysis of a Pipe Assembly
Workbench 8
2-D Modeling in Workbench
Axisymmetric Analysis of a Pipe Assembly

2. 2D Modeling
Upper String
Stress Joint
Lower String
Threads
Goal
Set up axisymmetric analysis in Workbench, solve and postprocess.
Model Description
2D model of pipe assembly consisting of an upper and lower drill string connected by a stress joint.
Elements: Axisymmetric (2-D) elements
Contact: Use bonded contact to simulate the threads, rather than modeling them explicitly. Use frictionless contact for all other surface interactions.
Loads: Internal Pressure, top tension load
Results: Von Mises, radial, axial and hoop stresses. Total deformation.

3. …2D Modeling in Workbench
Start ANSYS Workbench. On the Start screen, next to “Open”, scroll down to “DesignModeler Geometry”.
Click “Browse” in the lower right corner, and browse to the file “pipeconnection.agdb” and click “Open”.

4. …2D Modeling in Workbench
Click on the “Project” tab to return to the Project Page.
Under “Default Geometry Options” click on “Advanced Geometry Defaults” to expand the advanced options. Change the “Analysis Type” to 2-D.
Under “DesignModeler Tasks”, click “New Simulation”.

5. ..2D Modeling in Workbench
Close the Simulation Wizard.
Click on “Geometry” in the Tree. Click on the first part (“Lower String”), then hold down the Shift key, and click the last part (“Upper String”), so that all parts are highlighted.
In the Details View, click the drop down box next to “Behavior” and change it to “Axisymmetric”.

6. …2D Modeling in Workbench
Click on “Contact” in the Tree. In the Details view, click on the drop-down menu next to “Same Body Grouping” and change it to “No”.
Select both contact pairs, then right-click and select “Delete”. Right-click on “Contact” in the Tree, and select “Create Automatic Contact”. This creates separate contact pairs for each pair of lines in the model, and allows us to set different contact conditions for each.
Click on Contact Region 2 in the Tree (this is the contact between the top of the Lower String and the Stress Joint). In the Details View, change the Type to “Frictionless”.
Do the same for Contact Regions 3 and 5.

7. …2D Modeling in Workbench
Click on “Mesh” in the Tree. In the Details View, change the “Global Control” to “Advanced”. Set the “Element Size” to in.
Right-click “Mesh” in the Tree, and select “Preview Mesh”.

8. …2D Modeling in Workbench
Click on “Environment” in the Tree. In the Context Toolbar, select “Structural” then “Frictionless Support”. Set the selection filter to “Edge”, then select the bottom edge of the Lower String. Click “Apply” in the Details View.
Select “Structural” in the Context Toolbar again, then select “Pressure”. Hold down the Ctrl key and select the three lines on the inside (left-hand side) of the assembly, then click “Apply” in the Details View. Enter a Magnitude of 10,000 psi.
Select “Structural” in the Context Toolbar again, then select “Force”. Select the top edge of the Upper String, then click “Apply” in the Details View. Change “Define By” to “Components” in the Details View. Enter a Magnitude of 80,000 psi in the Y-direction.

9. …2D Analysis in Workbench
Choose “Solution” in the Tree. Select “Stress” from the Context Toolbar, then select “Equivalent (von-Mises)”. Also choose “Deformation” -- ”Total” from the toolbar, .
Click “Solve” from the toolbar.
Once the model is done solving, click on “Equivalent Stress” and “Total Deformation” in the Tree to view the results.

10. …2D Modeling in Workbench
When modeling axisymmetric parts, we generally like to look at radial, axial and hoop stresses. Click on “Solution” in the Tree, then choose “Stress” on the Context Toolbar. Select “Normal”. By default, the orientation of this stress result is the X-axis, which in an axisymmetric analysis, is equal to the Radial Stress. Right-click on “Normal Stress” in the Tree, and click “Rename”. Change the name to “Radial Stress”.
Insert “Normal Stress” two more times. In the second, change the Orientation in the Details View to “Y-axis” and change the name to “Axial Stress”. For the third Normal stress, change the orientation to “Z- axis” and rename it “Hoop Stress”. Click “Solve” and view these new results items.
Radial Stress
Axial Stress
Hoop Stress