equivalent stress to the yield stess.

Transcription

1 Example [Ansys Workbench/Thermal Stress and User Defined Result] A 50m long deck sitting on superstructures that sit on top of substructures is modeled by a box shape of size 20 x 5 x 50 m 3. It is subjected to 80 o C at top surface and convection all lateral surfaces. The end surfaces are fixed. The convection coefficient of air is given by 50 W/m 2 - o C and the ambient temperature is 20 o C. The material is Structural Steel. (a) Compute the thermal stress distribution. (b) When the yield stess varies with temperature by, obtain the ratio of the equivalent stress to the yield stess. Figure The model deck and typical bridge structure (Michigan Dept of Transportation) Solution. 1. Add Static Thermal Analysis [Geometry] 2. Sketching tab> create the section 3. Modeling tab >Extrude > Generate [Model] 4. Click Steady-State Thermal analysis in Outline 5. Temperature > pick the top surface > Apply > enter the temperature 6. Convection > pick all lateral surfaces > Apply > enter the film coefficient and bulk temperature 7. Click Solution in Outline 8. Thermal > Temperature and Total Heat Flux 9. Solve 10. Drag and drop Static Structural analysis on top of Solution cell. The Schematic Map appears as 11. Double click Model cell [Model] 12. Click Static Structural in Outline 13. Imported Load from thermal analysis solution has been added 14. Supports > Fixed Support > pick both end surfaces > Apply

2 15. Add Total Deformation and Equivalent Stress in Solution 16. Solve 17. The Equivalent Stress appears as 18. Click Solution in Outline > click Worksheet on top menu bar 19. Scroll down to BFE and right click >Create User Defined Result 20. BFE is the name for temperature in Ansys and appears in Outline 21. Right click > Rename > change it to Y(T) > enter Expression of Y(T) using BFE for temperature > change Identifier to YT > see the result of Y(T) 22. Right click Solution in Outline > Insert > User Defined Result > right click it and change the name to SMargin > In Details, enter Expression as SEQV/YT and Identifier = SMargin 23. See user defined SMargin as

3 Example [CFX] A water tank has dimensions as shown below. The units are in MKS. The thickness is 0.1 m outward from the given dimensions. (a) Create the tank by Revolve on XYPlane and the outlet pipe by Extrude on a new plane located at 10 m from XYPlane. Also, Blend with Radius = 0.5 m on the edge between two surfaces. (b) Then, use Tools > Thin to create a thin structure. Use the outward thickness = 0.05 m. (c) Use Fill option to fill the tank for fluid. (d) Based on the geometry just created, perform CFX analysis. (e) Use the CFX results to perform static stress analysis based on the pressure due to the flow. Figure Water tank structure Solution. 1. Add Component System/Geometry [Geometry] 2. Sketching tab> create the closed section for the tank with Polyline 3. Modeling tab > Revolve > pick the axis of rotation / Apply > Generate 4. Click XYPlane > New Plane > Transformation 1 = Offset Z, FD1 = 10 m > Generate 5. Sketching tab > create the circle 6. Modeling tab >Extrude > Direction = Reversed > Depth = To Next > Generate 7. Tools > Thin > ctrl + pick both top and exit surfaces > Details/Selection Type=Faces to Remove / Direction=Outward / Thickness = 0.05 m > Generate 8. Assume that user forgot to add the round around the joint edge. Tree Outline/right click Thin feature just added > Insert > Fixed Radius > pick the joint edge/apply and enter the radius in Details > Generate

4 9. Tools > Fill > Extraction Type = By Cavity > pick all three surfaces (the blended surface is not used in Fill) > Generate 10. Click Solid body created by Fill operation and see Fluid/Solid = Fluid 11. Select the Solid body> right click > Suppress (no need) 12. Drag and drop Fluid Flow (CFX) in Analysis Systems (not in Component Systems that does not have Geometry) on Geometry cell [Mesh] 13. Generate mesh and see as (right now, just accept the default mesh). User should try to use Inflation for mesh controls at inlet and outlet. See below the original and inflated meshes. [Setup] 14. Double click Default Domain in Outline or right click and Edit a. Basic Settings tab >Material = Water, Reference Pressure = 1 atm > OK 15. Boundary> enter a name inlet > OK b. Basic Settings tab Boundary Type = Inlet

5 Click Location > pick the top surface c. Boundary Details tab Mass and Momentum / Normal Speed = 1 m/s d. OK 16. Boundary> enter a name outlet > OK a. Basic Settings tab Boundary Type = Outlet Click Location > pick the end surface of the pipe b. Boundary Details tab Mass and Momentum > Option = Average Static Pressure, Relative Pressure = 1 atm c. OK 17. Double click Solution 18. Define Run dialog appears >Start Run> see the convergence plot as 19. Close the Solution window > back to Project [Results] 20. The initial wireframe may show much. Double click Wireframe in Outline a. Definition tab > drag the slider and make Edge Angle = 5 > Apply 21. Contour > OK (accept the default name) > double click the contour in Outline a. Geometry tab > Variable = Pressure > Apply

6 b. Uncheck Wireframe in Outline (see above right) 22. Vector > OK for name > double click the vector in Outline a. Geometry tab > Variable = Velocity b. Symbol tab > Symbol Size = 2 (just adjust seeing the results) > Apply 23. Clip Plane > OK for name > double click the clip plane in Outline a. Geometry tab > Method = YZ Plane, X = 0 m, check Flip Normal (depends on your model orientation) > Apply b. Right click in Graphics window > Clip Scene > select the clip plane (see above right) 24. Streamline > OK for name > double click the streamline in Outline a. Uncheck all others in Outline not to display them excep the streamline b. Geometry tab > accept all defaults > Preview Seed Points > Apply

7 25. Right click Geometry component > Duplicate 26. Double click the copy of Geometry a. Unsuppress solid body b. Suppress the fluid body 27. Drag and drop Static Structural analysis on Geometry cell of copied Geometry 28. Drag Fluid Flow/Solution and drop it on Structural Analysis/Setup [Static Structural / Model] 29. Click Static Structural in Outline 30. Supports > Fixed Support > pick the bottom surface > Apply 31. Right click Imported Load> Insert > Pressure a. In Details, select three inner surfaces for Geometry> Apply b. CFD Surface = Default Domain Default 32. Add Total Deformation and Equivalent Stress in Solution 33. Solve 34. Right click in Graphics window > View > Front 35. New Section Pane > draw a vertical line through the pipe > rotate the results

8