20ME68_Analysis of Trusses BY ANSYS .pptx

Analysis of Trusses BY FEM USING ANSYS

1. Computer Aided Modelling and Analysis Laboratory 20ME68 Exercises 4. Analysis of Truss 01 Prepared by: Vinayaka G P Course Coordinator, CAMA Lab Department of Mechanical Engineering Vidyavardhaka College of Engineering, Mysuru

2. Analysis of: “Trusses”

3. A truss structure consists of only two force members. Therefore, every truss element is in direct tension or compression. Loads are applied only at joints. The joints are assumed to be frictionless. i.e., pin joints. FEM can easily handle truss problems whether statically determinate and indeterminate. Also, it can provide joint deflection and handle temperature changes. Boundary conditions for different supports: Truss

4. A small railroad bridge is constructed of steel members, all of which have a cross sectional area of 3250mm 2 A train stops on the bridge and the loads applied to the truss on one side of the bridge are as shown in the figure. Determine the nodal deflections, reaction forces, and stress for the truss system. Consider Young’s modulus = 200GPa, cross section area and poisons ratio of 0.3. Problem Statement

5. Problem Statement Analysis Problem Domain: Structural Element type & its geometry: Truss (Link 180) Youngs Modulus: 200GPa Poisson’ Ratio: 0.3 Cross Sectional Area: 3250mm 2 Magnitude & Nature of the Load: Compressive Loads of 280kN, 210kN, 280kN and 360kN, on nodes 1,3,5 and 7respectively.

6. Parameters to be Determined

7. Problem Solution through ANSYS

8. ANSYS-APDL Procedure Ansys Utility Menu File – Clear and Start New-Read File – ok –Verify –Yes File- Change Title-Enter “Analysis of Truss 01”- Ok File – Save as- Save Database to- Type file name as “Analysis of Truss 01”-Ok. Main Menu: Material Properties Preferences- Structural-Ok. Preprocessor- Element type –Add/Edit/Delete-Element types-Add-Beam-2node188-Close. Preprocessor-Material Props-Material Model 1- Structural –Linear-elastic-Isotropic-EX: 200e3(Youngs Modulus) –PRXY: 0.3(Poisson’s ratio)- Close. Preprocessor-Sections-Link-Add-Section ID :1-Link Area: 3250-Tension Key-Both Tension and Compression.

9. ANSYS-APDL Procedure Main Menu: Model Creation Preprocessor- Modelling-Create-Keypoints-In Active CS: Keypoint Number: 01-Location in Active CS: 0,0,0 (X,Y,Z) Keypoint Number: 02-Location in Active CS: 1750,3000,0 (X,Y,Z) Keypoint Number: 03-Location in Active CS: 3500,0,0 (X,Y,Z) Keypoint Number: 04-Location in Active CS: 5250,3000,0 (X,Y,Z) Keypoint Number: 05-Location in Active CS: 7000,0,0 (X,Y,Z) Keypoint Number: 06-Location in Active CS: 8750,3000,0 (X,Y,Z) Keypoint Number: 06-Location in Active CS: 10500,0,0 (X,Y,Z) Preprocessor-Modelling-Create-Lines-In Active CS- Pick Keypoints-1-2, 2-3,3-4,4-5,5-6,6-7,1-3,3-5,5-7,2-4,4-6.

10. Truss Design after defining the keypoints and lines through keypoints

11. ANSYS-APDL Procedure Main Menu: Meshing Preprocessor-Meshing-size controls-manual size-lines-all lines-No. of element divisions-1-ok. Preprocessor-Meshing-Mesh-Lines-Pick all. Meshed view of the truss structure

12. ANSYS-APDL Procedure Plot Controls-Numbering-Turn on Keypoint, Line and Node numbers. Main Menu: Load Application Preprocessor-Loads-Define Loads-Apply-Structural-Displacement-On Keypoints-Pick Keypoint 1 -DOFs to be constrained-All DOF-Displacement Value: 0- Ok. Preprocessor-Loads-Define Loads-Apply-Structural-Displacement-On Keypoints-Pick Keypoint 7 -DOFs to be constrained-UZ and UY=Displacement Value: 0- Ok. Command Prompt-fk,1,FY,-280000. Command Prompt-fk,3,FY,-210000. Command Prompt-fk,5,FY,-280000. Command Prompt-fk,7,FY,-360000. Truss with load and support conditions

13. ANSYS-APDL Procedure Solution Solution-Analysis Type-New Analysis-Static-Ok. Solve-Current LS-Ok-Solution is Done-Close. General Post Processor Plot Results- Deformed Shape- Def+Undeformed -Ok- Record deformation Value :DMX = 7.27045 Command Prompt: SET -Enter Element Table-Define Table-Add-Label: STRESS-By sequence number-LS,1-Ok. Plot Results-Contour Plot-Elem Table-STRESS-Yes Average-Ok-Record the stress value from the plot.

14. ANSYS-APDL Procedure List Results-Nodal Solution-DOF Solution-Displacement Vector Sum-ok NODE UX UY UZ USUM 1 0.0000 0.0000 0.0000 0.0000 2 3.0293 -3.4381 0.0000 4.5823 3 0.73291 -6.4487 0.0000 6.4902 4 1.5635 -7.1003 0.0000 7.2705 5 2.2720 -6.8542 0.0000 7.2209 6 -0.48860E-001 -3.6622 0.0000 3.6625 7 3.0782 0.0000 0.0000 3.0782 MAXIMUM ABSOLUTE VALUES NODE 7 4 0 4 VALUE 3.0782 -7.1003 0.0000 7.2705 List-Results-Reaction Solu-All Items-ok NODE FX FY FZ 1 0.20373E-009 0.51333E+006 0.0000 7 0.61667E+006 0.0000 TOTAL VALUES VALUE 0.20373E-009 0.11300E+007 0.0000

15. ANSYS-APDL Procedure List Results-Nodal Solution-Stress-Von Misses Stress-ok NODE S1 S2 S3 SINT SEQV 1 0.0000 0.0000 -20.618 20.618 20.618 2 0.0000 0.0000 -27.920 27.920 27.920 3 51.159 0.0000 0.0000 51.159 51.159 4 0.0000 0.0000 -43.974 43.974 43.974 5 58.439 0.0000 0.0000 58.439 58.439 6 0.0000 0.0000 -30.712 30.712 30.712 7 0.0000 0.0000 -22.680 22.680 22.680 MINIMUM VALUES NODE 1 1 4 1 1 VALUE 0.0000 0.0000 -43.974 20.618 20.618 MAXIMUM VALUES NODE 5 1 3 5 5 VALUE 58.439 0.0000 0.0000 58.439 58.439

16. Results:

17. Results: Problem Type Parameters ANSYS Approach Railroad Truss System 1.Reaction Force 2.Deformation 3.Stress Node 1: FX: 0.20373E-009 FY:0.51333E+006 Node 7: FY: 0.61667E+006 7.27045 SMX:92.1367MPa SMN:8.31172MPa

18. Computer Aided Modelling and Analysis Laboratory 20ME68 Exercises 5. Analysis of Truss 02 Prepared by: Vinayaka G P Course Coordinator, CAMA Lab Department of Mechanical Engineering Vidyavardhaka College of Engineering, Mysuru

19. Find the deflections, nodal reactions and elemental stresses for the truss structure shown in the figure. Consider area to be 5000mm 2 and Youngs Modulus of 200GPa and Poisson Ratio to be 0.3 Problem Statement

20. Problem Statement Analysis Problem Domain: Structural Element type & its geometry: Truss (Link 180) Youngs Modulus: 200GPa Poisson’ Ratio: 0.3 Cross Sectional Area: 5000mm 2 Magnitude & Nature of the Load: Compressive Loads of 1000kN on nodes 5 and 8 respectively. KP 1: All DOF KP 2: UY=UZ=0 (roller support)

21. Parameters to be Determined

22. Problem Solution through ANSYS

23. ANSYS-APDL Procedure Ansys Utility Menu File – Clear and Start New-Read File – ok –Verify –Yes File- Change Title-Enter “Analysis of Truss 02”- Ok File – Save as- Save Database to- Type file name as “Analysis of Truss 01”-Ok. Main Menu: Material Properties Preferences- Structural-Ok. Preprocessor- Element type –Add/Edit/Delete-Element types-Add-Beam-2node188-Close. Preprocessor-Material Props-Material Model 1- Structural –Linear-elastic-Isotropic-EX: 200e3(Youngs Modulus) –PRXY: 0.3(Poisson’s ratio)- Close. Preprocessor-Sections-Link-Add-Section ID :1-Link Area: 5000-Tension Key-Both Tension and Compression.

24. ANSYS-APDL Procedure Main Menu: Model Creation Preprocessor- Modelling-Create-Keypoint-In Active CS: Keypoint Number: 01-Location in Active CS: 0,0,0 (X,Y,Z) Keypoint Number: 02-Location in Active CS: 12000,0,0 (X,Y,Z) Keypoint Number: 03-Location in Active CS: 2400,6000,0 (X,Y,Z) Keypoint Number: 04-Location in Active CS: 9600,6000,0 (X,Y,Z) Keypoint Number: 05-Location in Active CS: -3000,12000,0 (X,Y,Z) Keypoint Number: 06-Location in Active CS: 3000,12000,0 (X,Y,Z) Keypoint Number: 07-Location in Active CS: 9000,12000,0 (X,Y,Z) Keypoint Number: 08-Location in Active CS: 15000,12000,0 (X,Y,Z) Keypoint Number: 09-Location in Active CS: 3000,16500,0 (X,Y,Z) Keypoint Number: 10-Location in Active CS: 9000,16500,0 (X,Y,Z) Preprocessor-Modelling-Create-Lines-In Active CS- Pick Keypoints-1-2, 2-4,1-4,1-3,3-6,6-4,4-7,6-7,7-8,8-10,6-10,10-9,7-10,6-9,9-5.

25. Truss Design after defining the keypoints and lines through keypoints

26. ANSYS-APDL Procedure Main Menu: Meshing Preprocessor-Meshing-size controls-manual size-lines-all lines-No. of element divisions:1-ok. Preprocessor-Meshing-Mesh-Lines-Pick all. Meshed view of the truss structure

27. ANSYS-APDL Procedure Plot Controls-Numbering-Turn on Keypoint, Line and Node numbers. Main Menu: Load Application Preprocessor-Loads-Define Loads-Apply-Structural-Displacement-On Keypoints-Pick Keypoint 1 -DOFs to be constrained-All DOF-Displacement Value: 0- Ok. Preprocessor-Loads-Define Loads-Apply-Structural-Displacement-On Keypoints-Pick Keypoint 2 -DOFs to be constrained-UZ and UY=Displacement Value: 0- Ok. Command Prompt-fk,5,FY,-1000000. Command Prompt-fk,8,FY,-1000000. Truss with load and support conditions

28. ANSYS-APDL Procedure Solution Solution-Analysis Type-New Analysis-Static-Ok. Solve-Current LS-Ok-Solution is Done-Close. General Post Processor Plot Results- Deformed Shape- Def+Undeformed -Ok- Record deformation Value :DMX = 69.6175 Command Prompt: SET -Enter Element Table-Define Table-Add-Label: STRESS-By sequence number-LS,1-Ok. Plot Results-Contour Plot-Elem Table-STRESS-Yes Average-Ok-Record the stress value from the plot. SMN: -238.583MPa SMX: 133.333MPa

29. List Results-Nodal Solution-DOF Solution-Displacement Vector Sum-ok NODE UX UY UZ USUM 1 0.0000 0.0000 0.0000 0.0000 2 4.8000 0.0000 0.0000 4.8000 3 4.7081 -7.5329 0.0000 8.8832 4 6.8681 -10.243 0.0000 12.333 5 -2.4458 -15.402 0.0000 15.595 6 -7.2236 -19.902 0.0000 21.173 7 -11.046 -15.199 0.0000 18.788 8 0.77641 -19.699 0.0000 19.714 9 -19.046 -66.962 0.0000 69.617 10 5.5542 -57.773 0.0000 58.039 MAXIMUM ABSOLUTE VALUES NODE 9 9 0 9 VALUE -19.046 -66.962 0.0000 69.617 List-Results-Reaction Solu-All Items-ok NODE FX FY FZ 1 -0.10630E-008 0.10000E+007 0.0000 2 0.10000E+007 0.0000 TOTAL VALUES VALUE -0.10630E-008 0.20000E+007 0.0000

30. Results:

31. Results: Problem Type Parameters ANSYS Approach Mobile Tower Truss System 1.Reaction Force 2.Deformation 3.Stress Node 1: 1000kN Node 2: 1000kN 69.6175mm SMN: -238.583MPa SMX: 133.333MPa