WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14

Transcription

1 WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD For ANSYS release 14

2 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated. Goal: The goal is determine the fatigue life due to a varying bending moment using the hot spot stress method. Page 2

3 1. Launch ANSYS WorkBench: a. From the Project Page, in the File menu select Restore Archive and click on [Browse] b. Select the Workbench archive Workshop_6_4_geometry.wbpz and click on [Open] c. Save the model in the training directory specified by the teacher. Page 3

4 2. Add a Static Structural analysis connection to existing geometry: 3. Open the Simulation file: The Workbench Project page will appear. Either double-click on the Setup (highlighted) to open the existing Simulation database Static Structural or right click and select Edit. Page 4

5 4. Review the geometry: Note that the beam and plate is two separate volumes joined together as a multi body part i.e. the two volumes share a common surface. See that the bottom surface of the plate has a gap modeled. On the top surface of the VKR-beam there is a line imprinted starting from the weld toe. Activating visibility of vertices, there is two points imprinted on the line. The first point lay 4 mm away from the weld toe and the second point lay 10 mm from the weld toe according to the hot spot method. Page 5

6 5. Review and suppress contact pair The default contact setup create bonded contact between top surface of beam and the large surface on top plate. Suppress the contact pair between the large surface of the plate and top surface of the VKR-beam. Another option is to change the contact type to frictionless or frictional contact but this will result in long analysis time so don t do it unless there is plenty of time available for the workshop. Page 6

7 6. Create the mesh: The default settings will generate a relative course mesh. A rule of thumb is trying to keep the ratio between shortest and longest element edge less than 1/3. In some situations the ratio 1/5 may be acceptable. Recall that the hot spot method require that the effect of the geometric singularity shall not influence the stress in the hot spots, a fine mesh is required with at least 2-3 element between weld toe and first hot spot point. Introduce global mesh controls as shown in figure top right. Create a Sphere of influence at the vertex for the first hot spot point. Page 7

8 7. Apply displacement boundary conditions In Outline select Static Structural Select the two surfaces in the symmetry cut. Under Supports select Remote Displacement and enter 0 (zero) for all displacement and rotational components. Page 8

9 8. Apply bending moment: Select the surface at free end of the VKR-beam. Under Loads Select Moment Under Details of Moment change Define By to Components and specify a bending moment about the X-axis of Nmm. Page 9

10 9. Define named selection for use in results evaluation: To facilitate the results evaluation using the hot spot method a command object will be used that extract the stresses at the hot spot point and calculates the stress at the hot spot Required input to the command object is two named selections, one for each hot spot point. Select the vertex (point) for the first hot spot point laying 4 mm from weld toe. Create a named selection with name: W1_L1_SP1 W1= weld number 1 L1= line number 1 SP1= hot spot point 1 on line Repeat procedure for second hot spot point: W1_L1_SP2 Page 10

11 10. Create global results plots for: Total deformation Von Mises Stress Maximum Principal 11. Insert a command object 12. Import the file consisting of command objects Open the file HotSpotStress.txt and the contents of the file will be displayed in the command object window. Page 11

12 13. Insert a command object, continued: Verify that the labels of the named selections do match the numbers specified in command object. Change the output key to Hot to get the result in Details of Commands (APDL) window. 14. Save the project 15. Run the analysis Page 12

13 16. Review the results for: Total deformation (pay attention to local deformation in VKR-beam near weld) Von Mises Stress Maximum Principal (global and path) What is the hot spot stress in VKR-beam? Answer: MPa 17. Calculate fatigue life: This joint type have the fatigue weld class FAT=100 according to IIW-1823, Detail category T according to DNV RP-C203 (equal to FAT90) and detail category 100 according to Eurocode 3. Use FAT100 and m=3. m 6 FAT N = 2 10 σ Calculated fatigue life is cycles. Page 13

14 18. Save the project. 19. If time permits: Check the parameter box for hot spot stress. Close the Simulation window On project page open the Parameter Set The parameter DS_Hot_Spot_Path define the location of the of the hot spots along the weld on the flat surface. The parameter may vary between 0.01 to mm. Enter values between 5 and 35 mm using a step of 5 mm. Update all design points and create a graph on hot spot stress versus lateral position Page 14