Upcoming SlideShare
×

Thanks for flagging this SlideShare!

Oops! An error has occurred.

×
Saving this for later? Get the SlideShare app to save on your phone or tablet. Read anywhere, anytime – even offline.
Standard text messaging rates apply

# Workshop14 pipe-whip

1,388

Published on

abaqus,Workshop

abaqus,Workshop

2 Likes
Statistics
Notes
• Full Name
Comment goes here.

Are you sure you want to Yes No
• Be the first to comment

Views
Total Views
1,388
On Slideshare
0
From Embeds
0
Number of Embeds
0
Actions
Shares
0
117
0
Likes
2
Embeds 0
No embeds

No notes for slide

### Transcript

• 1. Workshop 14 Pipe Whip Analysis Introduction This workshop involves the simulation of a pipe-on-pipe impact resulting from the rupture of a high-pressure line in a power plant. It is assumed that a sudden release of fluid could cause one segment of the pipe to rotate about its support and strike a neighboring pipe. The goal of the analysis is to determine strain and stress conditions in both pipes and their deformed shapes. The simulation will be performed using ABAQUS/Explicit. This workshop is based on ABAQUS Benchmark Problem 1.3.9. Geometry and model Both pipes have a mean diameter of 6.5 in with a .432 in wall thickness and a span of 50 in between supports. The fixed pipe is assumed to be fully restrained at both ends, while the impacting pipe is allowed to rotate about a fixed pivot located at one of its ends, with the other end free. We exploit the symmetry of the structure and the loading and thus model only the geometry on one side of the central symmetry plane, as shown in Figure W14–1. The pipe geometry is modeled as a shell feature. Figure W14–1. Pipe model assembly 1. Start a new session of ABAQUS/CAE from the workshops/pipeWhip directory. 2. Switch to the Part module. 3. From the main menu bar, select PartCreate. impacting pipe fixed pipe axis of rotation
• 2. 4. In the Create Part dialog box: A. Name the part pipe-fixed. B. The pipe will be modeled using shell elements; thus, choose Shell as the base feature shape, Extrusion as the base feature type, and set the Approximate size to 20. C. Review the other defaults and click Continue. Since the pipe is modeled using a shell feature, the pipe radius must be equal to the mean pipe radius. 5. Use the Create Isolated Point tool to create points at the coordinates (0.0, 3.25) and (0.0, -3.25). 6. Sketch a circle of radius 3.25 in. as shown in Figure W14–2. Figure W14–2. Geometry sketch for the fixed pipe 7. Dimension the circle using the radial dimension tool from the toolbox shown as Figure W14–3. Figure W14–3. Dimensioning tools 8. Click mouse button 2 to continue; in the Edit Base Extrusion dialog box, enter 25.0 in. as the value of the extrusion depth. (Mouse button 2 is the middle mouse button on a 3-button mouse; on a 2-button mouse, press both mouse buttons simultaneously.) 9. From the main menu bar, select PartCopy and copy the part named pipe- fixed to a new part named pipe-impacting. W14.2 radial dimension tool Click on the black triangle to extend the toolbox option
• 3. 10. Switch to the part pipe-impacting by selecting it from the Part pull-down list in the context bar. 11. From the main menu bar, select FeatureEdit. 12. In the prompt area, click Feature List. 13. In the Feature List dialog box, select Shell-extrude-1 and click OK. 14. In the Edit Feature dialog box select Edit Section Sketch. 15. Delete the circle and sketch a semi-circle with the same radius as shown in Figure W14–4. Figure W14–4. Geometry sketch for the impacting pipe 16. Modify the depth of extrusion to be 50.0. 17. In the Edit Feature dialog box, click OK to generate the modified part. Materials and section Both pipes are made of steel. A von Mises elastic, perfectly plastic material model is used, with a yield stress of 45E3 psi. 1. Switch to the Property module. 18. From the main menu bar, select MaterialCreate. Create a material named Steel with the following properties: Modulus of elasticity: 30E6 psi Poisson's ratio: 0.3 Yield Stress: 45.0E3 psi Density: 7.324E-4 lb-sec2 /in4 19. From the main menu bar, select SectionCreate and create a homogeneous Shell section named PipeSection with a shell thickness of 0.432 in. 20. Use the analysis default section Poisson ratio of 0.5. W14.3
• 4. 21. Select Gauss quadrature for shell section integration with three integration points through the thickness. 22. From the main menu bar, select AssignSection and assign the shell section to both parts. Model assembly You will now create an instance of each pipe and position them relative to one another. 1. Switch to the Assembly module. 23. From the main menu bar, select InstanceCreate. In the Create Instance dialog box, select both parts and toggle on Auto-offset from other instances. 24. Modify the position of the impacting part as follows: A. From the main menu bar, select InstanceTranslate. Select the impacting pipe as the instance to be translated, and define the translation vector using the start and end points indicated in Figure W14–5. Figure W14–5. Translation used to position the impacting pipe D. From the main menu bar, select InstanceRotate and rotate the impacting pipe 90 degrees about the axis defined by the two points shown in Figure W14–6. W14.4 Start point of translation vector (center point on bottom edge of impacting pipe) End point of translation vector
• 5. Figure W14–6. Rotation used to position the impacting pipe Since ABAQUS/Explicit considers the shell thickness in its contact calculations and does not permit any initial overclosures, the initial position of the pipes must account for the shell thickness. 25. Modify the vertical position of the impacting pipe as follows: · From the main menu bar, select InstanceTranslate. Translate the impacting pipe a distance of 0.432 in. in the vertical direction. This will eliminate any initial overclosure between the pipes. The fixed pivot at the end of the impacting pipe will be modeled using a rigid body constraint. This constraint will tie the nodes at one end of the impacting pipe with a reference node that will act as the pivot point. 26. From the main menu bar, select ToolsReference Point and create a reference point at the location shown in Figure W14–7: Figure W14–7. Final assembly and reference point W14.5 end point of rotation axis start point of rotation axis
• 6. Analysis step and output requests Because of the high-speed nature of the event, the simulation is performed using a single explicit dynamics step. 1. Switch to the Step module. 27. From the main menu bar, select StepCreate to create a Dynamic, Explicit step with a time period of 0.015 seconds. Accept all defaults for the time incrementation and other parameters. 28. From the main menu bar, select OutputField Output RequestsEdit F-Output-1 and review the preselected field output requests. Change the frequency at which the output is written to 12 equally spaced intervals. 29. Create a geometry set consisting of the reference point. This set will be used to restrict output of the reaction force history to this region. From the main menu bar, select ToolsSetCreate. In the Create Set dialog box, name the set RefPt and click Continue. Select the Ref Pt in the viewport, and click Done. 30. From the main menu bar, select OutputHistory Output Requests Create and request stored history output to the ODB at 100 equally spaced time intervals during the analysis containing the following information: · Reaction forces at the constrained end of the fixed pipe. Use the set RefPt to restrict the output. Interactions You will now define a contact interaction between the two pipes and constrain the pivot end of the impacting pipe to behave like a rigid body. To facilitate the definition of the contact interaction and rigid body constraint, the pipes will first be partitioned into different regions. The partitions will also serve another purpose: they will permit selective mesh refinement in the regions where contact is expected to take place. Partitions The impacting pipe will be divided into three regions of lengths 15, 20, and 15 in., respectively. The fixed pipe will be divided into two regions of lengths 18 and 7 in. each. Partitioning the impacting pipe 1. Switch to the Interaction module. 31. From the main menu bar, select ToolsDatumPlane3 points. Create a datum plane by selecting the 3 points shown in Figure W14–8. W14.6
• 7. Figure W14–8. Points used to define datum plane 32. From the main menu bar, select ToolsPartitionFaceSketch. 33. Select the curved face on the impacting pipe as the face to be partitioned and the datum plane as the plane on which the partitions will be sketched. 34. Specify the projection distance as Through All and accept the default projection direction as shown in Figure W14–9. 35. Select the circular edge highlighted in Figure W14–9 when prompted for an edge that will appear vertical and to the right of the sketch. Figure W14–9. Sketch projection direction W14.7 projection direction
• 8. 36. Sketch two vertical lines for the partitions as shown in Figure W14–10. 37. Create the partition. Figure W14–10. Face partition sketch Partitioning the fixed pipe 1. From the main menu bar, select ToolsPartitionFaceShortest path between 2 points to partition the fixed pipe using the 2 points highlighted in Figure W14–11. This partition will later be used for assigning edge seeds. W14.8
• 9. Figure W14–11. Face partition using shortest path between 2 points 38. From the main menu bar, select ToolsDatumPlaneOffset from plane. 39. Select the datum plane created earlier as the plane from which to offset. 40. In the prompt area, click Enter Value to choose the method by which to specify the offset distance. If necessary, flip the direction of the arrow indicating the offset direction so that it points in the direction shown in Figure W14–12. 41. Specify an offset distance of 7.0 in. Figure W14–12. Projection direction for fixed pipe partition W14.9 Select these two points offset direction base datum plane new datum plane
• 10. 42. From the main menu bar, select ToolsPartitionFaceUse datum plane. 43. Select the surface of the fixed pipe as the face to be partitioned and the datum plane created above as the plane with which to create the partition, as shown in Figure W14–13. 44. Create the partition. Figure W14–13. Partition of the fixed pipe Contact interaction 1. From the main menu bar, select InteractionPropertyCreate. 45. In the Create Interaction Property dialog box, select Contact as the interaction type and click Continue. 46. In the Edit Contact Property dialog box, select MechanicalTangential Behavior and choose the Penalty friction formulation. Enter a friction coefficient of 0.2, and click OK to close the dialog box. 47. From the main menu bar, select InteractionCreate. 48. In the Create Interaction dialog box, choose step-1 as the step in which the interaction will be created and select the Surface-to-surface contact (Explicit) type. For the impacting pipe, the outer surface of its center region will be used for contact; for the fixed pipe, the outer surface of its shorter region will be used for contact. 49. Define contact between these surfaces as shown in Figure W14–14. W14.10 Partition the fixed pipe with this datum plane
• 11. Figure W14–14. Surfaces involved in contact Rigid body constraint 1. From the main menu bar, select ConstraintCreate. 50. In the Create Constraint dialog box, select Rigid body as the constraint type and click Continue. 51. In the Edit Constraint dialog box, select the region type Tie (nodes) and click Edit in the right side of the dialog box. 52. Select the edge shown in Figure W14–15 as the tie region for the rigid body. 53. Similarly, select the point in the viewport identified by the label Ref Pt as the rigid body reference point. Figure W14–15. Rigid body constraint master surface slave surface W14.11 tie region
• 12. Boundary conditions The edges located on the symmetry plane must be given appropriate symmetry boundary conditions. One end of the impacting pipe and both ends of the fixed pipe are fully restrained. 1. Switch to the Load module. 54. From the main menu bar, select BCCreate. 55. In the Create Boundary Condition dialog box, select Symmetry/ Antisymmetry/Encastre as the boundary condition type and click Continue to create the boundary conditions shown in Figure W14–16. · Symmetry boundary conditions: Select the edges shown in Figure W14–16; and in the Edit Boundary Condition dialog box, choose the ZSYMM (U3=UR1=UR2=0) boundary condition. · Fully constrained boundary conditions: Select the edge shown in Figure W14–16; and in the Edit Boundary Condition dialog box, choose the ENCASTRE (U1=U2=U3=UR1=UR2=UR3=0) boundary condition. · Pinned Boundary condition: Select the Ref Pt; and in the Edit Boundary Condition dialog box, choose the PINNED (U1=U2=U3=0) boundary condition. Figure W14–16. Boundary conditions Initial conditions The impacting pipe is given an initial angular velocity of 75 radians/sec about its supported (pinned) end. symmetry: ZSYMM BC (all edges on this plane) fully constrained end: ENCASTRE BC W14.12 PINNED BC
• 13. 1. Use ToolsQueryPoint to determine the coordinates of two end points on the axis of rotation at the pivot end of impacting pipe as shown in Figure W14–17. Figure W14–17. Points on axis of rotation The coordinates will be printed out to the CLI as shown in Figure W14–18. Figure W14–18. Point coordinates 56. From the main menu bar, select FieldCreate. 57. In the Create Field dialog box, set the step to Initial and accept the default category and type selections. Click Continue to proceed. 58. Select the impacting pipe as the region to which the initial velocity will be assigned, and click Done. 59. In the Edit Field dialog box, change the field definition to Rotational only. Enter a value of 75 for the Angular velocity. Use the coordinates of the first point indicated in Figure W14–17 to define the first axis point and the coordinates of the second point indicated in Figure W14–17 to define the second axis point. Mesh W14.13 second point first point
• 14. The pipes will be meshed with S4R shell elements. A finer mesh density will be used in the regions of the pipes where impact will is expected to occur. 1. Switch to the Mesh module. 60. From the main menu bar, select MeshElement Type and select the whole model by clicking the left mouse button and dragging across the viewport. Examine the various options available in the Element type dialog box, and accept the default element type S4R. 61. From the main menu bar, select SeedEdge By Number and assign the number of edge seeds to each edge shown in Figure W14–19. Figure W14–19. Edge seeds 62. From the main menu bar, select MeshInstance and select both pipes as the part instances to be meshed. The mesh is shown in Figure W14–20. W14.14 9 28 9 16 12 9 7 12
• 15. Figure W14–20. Instance meshes Analysis 1. Switch to the Job module. 63. From the main menu bar, select JobCreate and create a job named pipe- whip. 64. Open the Job Manager, and click Submit to submit the job for analysis 65. Monitor the progress of the job by clicking Monitor in the Job Manager. Visualization 1. Once the analysis completes successfully, click Results in the Job Manager to switch to the Visualization module. 66. Plot the undeformed and the deformed model shapes. From the main menu bar, select ToolsColor Code and specify different colors to the two pipe instances, as shown in Figure W14–21. W14.15
• 16. Figure W14–21. Deformed model shape 67. From the main menu bar, select AnimateTime History to animate the deformation history. 68. Plot the contours for Mises stress and PEEQ on the deformed shape. The contour plots are shown in Figure W14–22. Figure W14–22. Contour plots 69. From the main menu bar, select ResultHistory Output to create time history X–Y plots of the model’s kinetic energy (ALLKE), internal energy (ALLIE), and dissipated energy (ALLPD). 70. In the History Output dialog box, click Plot to display the curves and click Dismiss to close the dialog box. The energy plot is shown in Figure W14–23. W14.16 MISES PEEQ
• 17. Figure W14–23. Energy histories Near the end of the simulation, the impacting pipe is beginning to rebound, having dissipated the majority of its kinetic energy by inelastic deformation in the crushed zone. 71. From the main menu bar, select ToolXY DataManager. In the XY Data Manager, click Create. In the Create XY Data dialog box, choose ODB history output and click Continue. Select the three reaction forces components, and click Save As. Save the components using the default names. Click Dismiss to close the dialog box. 72. Simultaneously plot the total reaction components (RF1, RF2, RF3) versus time by selecting the three curves in the XY Data Manager and clicking Plot. The curves appear in Figure W14–24. W14.17
• 18. Figure W14–24. Reaction force histories W14.18