Feed

Tutorial - Solving 2D Truss problem using Mechanical APDL (ANSYS)?

Tutorial by Sudhir Gill
Small

In general, a finite element solution may be broken into the following three stages.

1. Preprocessing: defining the problem;
- Define keypoints/lines/areas/volumes
- Define element type and material/geometric properties
- Mesh lines/areas/volumes as required

2. Solution: assigning loads, constraints and solving;

3. Postprocessing:
- Lists of nodal displacements
- Element forces and moments
- Deflection plots
- Stress contour diagrams

We will go through these and solve the problem. I will suggest you to go through this tutorial before solving this problem. http://grabcad.com/questions/tutorial-2d-truss-analysis-in-mechanical-apdl-ansys-part-1

  1. Step 1:

    Start ANSYS Mehchanical APDL.

  2. Step 2:

    Click Preferences and select Structural & click OK.

  3. Step 3:

    Now we have the first step i.e. Preprocessing. Goto Modeling >> Create >> Keypoints >> In active CS. We will now create Keypoints for the problem.

  4. Step 4:

    Input keypoints
    x y z
    1. 0 0 0
    2. 3000 3000 0
    3. 6000 0 0
    4. 0 3000 0
    5. 6000 3000 0
    6. 3000 6000 0
    7. 0 6000 0
    8. 6000 6000 0
    9. 0 9000 0
    10. 3000 9000 0
    11. 6000 9000 0
    12. 0 12000 0
    13. 3000 12000 0
    14. 6000 12000 0
    15. 3000 15000 0

  5. Step 5:

    We have the keypoints plotted.

  6. Step 6:

    We have to create the lines. Goto Modeling >> Create >> Lines >> Lines >> in active Coord.

  7. Step 7:

    Create lines. Click OK.

  8. Step 8:

    Now we have to Define the mesh size. Goto >> Meshing >> Size Cntrls >> Manual Size >> Lines >> All Lines.

  9. Step 9:

    Input number of element divisions = 1 and click OK.

  10. Step 10:

    Now we have to define the element type. Goto Element type >> Add/Edit/Delete.

  11. Step 11:

    Click Add and then select Link >> 3D finit stn 180. This is link 180. Click OK and then close.

  12. Step 12:

    Now we have to define the cross section of the truss. Goto Real Constants >> Add/Edit/Delete.

  13. Step 13:

    Click Add and then define Cross-sectional area = 3500.

  14. Step 14:

    Now we will create the mesh of this truss. Goto Meshing >> Mesh >> Lines.

  15. Step 15:

    Click Pick all.

  16. Step 16:

    Now we have to define the material properties. Goto Material Props >> Material models.

  17. Step 17:

    Goto Structural >> Linear >> Elastic >> Isotropic.

  18. Step 18:

    Input EX=200000, PRXY=0. Click OK and then close.

  19. Step 19:

    Now the second step i.e. Solution. Goto Solution >> Analaysis Type >> New Analysis.

  20. Step 20:

    Select Static and then click OK.

  21. Step 21:

    Now we will define the fixed supports. Goto Define loads >> Apply >> Structural >> Displacement >> On Keypoints.

  22. Step 22:

    Select two fixed lower keypoints.

  23. Step 23:

    Click OK and then select ALL DOF and click OK.

  24. Step 24:

    Now Define Loads >> Apply >> Structural >> Force/Moment >> On keypoints.

  25. Step 25:

    Select top keypoints. Click OK.

  26. Step 26:

    Input force value = 5000N. Click OK.

  27. Step 27:

    Now save the project.

  28. Step 28:

    Now second step i.e. Solution. Solution >> Solve >> Current LS.

  29. Step 29:

    Click OK.

  30. Step 30:

    Click Close.

  31. Step 31:

    Now third step i.e. Post proecessing. General postproc >> List results >> Reaction Solu.

  32. Step 32:

    Click OK.

  33. Step 33:

    Now we have the reaction on the 1st and 2nd node which are fixed.

  34. Step 34:

    Under Plot Results >> Deformed shape.

  35. Step 35:

    Select Def+Undeformed and click OK.

  36. Step 36:

    We have deformation plot.

Comments

Please log in to add comments