Stress and Deformation in 2D Steel Plate

Here are the steps for setting up the model:

    ansys -g -j 2Dsolid &

    1. Set Preference:
       Preferences - Structural = on - OK

    2. Key Points:
       Preprocessor - Modeling.Create - Keypoints - In Active CS 
       Keypoint number = 1,        X,Y,Z = 0., -3., 0.  --  > Apply
       Keypoint number = 2,        X,Y,Z = 0., 3., 0.  --  > Apply
       Keypoint number = 3,        X,Y,Z = 24, 1.5, 0.  --  > Apply
       Keypoint number = 4,        X,Y,Z = 24, -1.5, 0.  --  > OK 

    3. Lines:
       Preprocessor - Modeling.Create - Lines/lines - Straight line 
       Now left click points 1 and 2;
       Then left click points 2 and 3;
       Then left click points 3 and 4;
       Then left click points 4 and 1;
       -> Cancel

    4. Surface:
       Preprocessor - Modeling.Create - Areas/Arbitrary - By lines
       Pick (by left click) the four lines
       Apply - Cancel 

    5. Define materials
       Preprocessor - Material props - Material models 
               - Structural - Linear  - Elastic - Isotropic - OK
       Young's modulus EX = 30e6
       Poisson's Ratio PRXY = 0.3

               - Density
       Density DENS = 0.2836
       OK
       
       Material - Exit

    6. Select Mesh Type:
       Preprocessor - Element Type - /Add/edit/Delete - Add 
       Select "Structral Solid" and "Quad 4node 42"
       OK 
       Options - Element behavior = Plane strs w/thk - OK 
       Close

       Preprocessor - Real Constants - /Add/edit/Delete - Add - OK 
       THK = 1.0 - OK - Close

    7. Meshing:
       Preprocessor - Meshing/size Cntrls - Lines/Picked lines 
       Pick two long lines - Apply - NDIV = 32 - OK 
       Preprocessor - Meshing/size Cntrls - Lines/Picked lines 
       Pick two short lines - Apply - NDIV = 8 - OK
       Close "the size Cntrls window"

       Preprocessor - Meshing/Mesh - Areas/Free 
       Pick the area - OK 

    8. Apply BCs and loads:

       Solution -Loads/Apply - Displacement - On nodes
       Pick all the nodes at x=0
       OK - Lab2 = All DOF & Value =0.0 - OK
       
       Solution -Loads/Apply - Force/Moment - On nodes
       Pick the three nodes in the middle at x=12
       OK 
       Lab = FX, Value = 25 - OK

       Solution -Loads/Apply - Force/Moment - On nodes
       Pick the two nearby nodes at x=12
       OK
       Lab = FX, Value = 12.5 - OK
       
       Solution -Loads/Apply - Gravity
       ACELX= - 1.0, ACELY=0.0, ACELZ=0.0
       OK
      
       PlotCtrls/numbering - NODE=on - OK 
      
       Plot/nodes
     
       PlotCtrls/Pan,Zoom,Rotate
       (To zoom into any region, say, around x=12. 
         This allows me to find out the node numbers at points A and B)

       (An alternative method is to select the subset of nodes at y=0 by:
         Select - Entities - Nodes - By Location, with Y coordinates from -0.01 to 0.01,
         Then List - Nodes - Sort first by X Coordinate.

        You may also give a name to this subset of nodes by
        Select - Comp/Assembly - Create Component, and name it "cline".) 

    9. Solve:
       Solution - Solve/Current LS - OK - Close - Close

    10. See the solution:
 
       Select - Nodes/By number/Pick - Input the node numbers for A and B (e.g. 189,46), 
       Return - OK

       General Postproc - List Results - Nodal Solution
       OK
  
       Plot Results - Deformed Shape - Def + undeformed


Modify the load distribution or the poisson ratio to see how the results vary.