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