Objectives:
 

• Important things to know about ANSYS

 
• Two-dimensional modeling of the Plate using ANSYS

 
• Two-dimensional modeling of heat conduction using ANSYS

Important things to know about ANSYS:
 

• Starting an ANSYS Session in interactive, graphics mode:
  

        ansys -g -j jobname
  
        For other start-up options,  
        see Chapter 3 of Operation Guide.
      
  

• On-line documentations: You can find all on-line hypertext-based documentations by clicking Help - Table of Contents.  A text window will appear to allow you navigate through a selected document.
• Analysis Guides:   give procedures for performing an analysis, i.e., How to build a model, how to apply loads and obtain a solution, how to review the results.
• Commands manual: A list of ANSYS commands (in alphabetical order) and their descriptions of use.
• Element manual: A detailed description of all types of ANSYS elements
• Theory manual: Theoretical descriptions of procedures, elements, and commands
• Operations Guide: nuts and bolts of running ANSYS and using its graphical user interface (GUI)
• Verification manual: Comparing ANSYS numerical solutions with theoretical solutions
• Ansys file types and file formats:
  

  --------------------------------------------------------
  FILE TYPE           FILE NAME          FILE FORMAT
  
  Log file            jobname.log        ASCII
  
  Error file          jobname.err        ASCII
  
  Output file         jobname.out        ASCII
  
  Database file       jobname.db         Binary
  
  Results file:                          Binary
   Solid/Structural   jobname.rst
   Thermal            jobname.rth
   Fluid              jobname.rfl
  
  ------------------------------------------------------
  The log file is the most important file. It keeps a complete log 
    of an ANSYS session (list all commands you execute). You can 
    read the log file, view it while in ANSYS,  edit it, 
    and input it later.
    Note: use ! for comments
  
  To input a log file: FILE - Read input from ... 
  
  The error file lists all the errors and warnings. You may use 
    this to edit your log file.
  
  Output file: 
    containing:
        -- Load summary information, 
        -- mass and moments of inertia of the model
        -- solution summary information 
        -- total CPU time, 
        -- data requested by the OUTPR output control command
            e.g., General Postprocesser - list results - modal -
             - print output
    If you run the solution interactively, the output
    file is actually your screen (window). By doing the following
    before issuing SOLVE, you can divert the output
    to a file instead of the screen:
      File - Switch Output to - File 
  
  Database file: Contains all model information
  
  Results file: contains solution data generated during SOLVE steps
  

• To verify the geometry input graphically:
  

  PlotCtrls - Style - Size and Shape
  Plot - Elements
  

• Reviewing results in POST1 (General postprocessing):
  

  -- graphical display: contour, deformed shape, reaction force..
  
  -- tabular listings (can be saved in the output file)
  

• Graphics functions:
  

  (1) PlotCtrls: changing graphics specifications
       Plot: select graphics action
  
  (2) Replot and Erase:
         Plot - Replot
         PlotCtrls - Erase Options - Erase Screen
  
  (3) Multi-Plotting Techniques
        (a) PlotCtrls - MultiWindow Layout
        (b) PlotCtrls - Multi-Plot Controls
  
  (4) Storing a graphics display on a file:
       PlotCtrls - Redirect Plots - to Graphics File
  

Two-dimensional modeling of the Steel Plate using ANSYS

You can use ANSYS to answer the question:
To what extent is one-D solution adequate?

The two-D solid-element model for the Steel Plate problem: 

Mesh resolution:  32x8, namely 32 elements in X and 8 elements in Y

Objective: (1) Study the effect of external load distribution
           
           (2) Study the effect of different Poisson ratio
     
Model Development (for Poisson ratio=0.3, Load over 1/2 of width):

    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 x=12. This allows me to find out the node numbers at x=12)

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

    10. See the solution:
 
       Select - Nodes/By number/Pick - Input 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.

Two-dimensional modeling of heat conduction using ANSYS

Consider heat conduction in an aluminum plate (12in x 12in x 2in thick or
30.5 cm x 30.5 cm x 5.1 cm) 
subject to the following boundary conditions:
  
  Two edges are heated using thermally bonded electrical resistance strip 
   heaters (assume constant heat flux boundary condition)

  The other two edges are cooled using thermally bonded heat exchanger
   plates supplied with cooling water from a chiller 
   (assume constant temperature boundary condition)

  The bottom face is insulated with glass wool

  The top face is separated from the surroundings by an air gap trapped 
  underneath a glass plate

Assume: T1 = 20 C, T2=30 C, q1 = 10000 W/m^2, q2=15000 W/m^2.
Material properties: conductivity = 200 W/m.k.

Treat this as a 2D heat conduction problem. Solve for temperature 
distribution.

 
Model Development:

ansys -g -j thermal &

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

2. Define a square region:
   Preprocessor - Modeling.Create - Rectangle - By Dimension
   X1=0.,X2=0.305
   Y1=0.,Y2=0.305
   OK

3. Define materials
 Preprocessor - Material props - isotropic - OK
 Thermal conductivity = 200.0
 OK

4. Select Mesh Type:
   Preprocessor - Element Type - /Add/edit/Delete - Add 
   Select "Thermal Solid" and "Quad 4node 55"
   OK 
   Close

5. Meshing:

  Preprocessor - MeshTool - 
  Size controls/ lines/Set  - 
  Pick x=0 and y=o lines - NDIV = 16 - OK 

  set Mesher = Map
  Mesh - Pick the area - OK 

6. Apply BCs and loads:
 
Solution - Loads/Apply - Temperature - On Lines
Left click the x=L line - OK
Value = 20 - OK
On Lines - Left click the y=L line - OK
Value = 30 - OK

Loads/Apply - Heat Flux - On lines
Left click the x=0 line - OK 
Value = 10000 - OK 
On Lines - Left click the y=0 line - OK
Value = 15000 - OK

7. Solve

Solution - Solve/Current LS - OK

8. Plot temperature distribution on a line for comparison
    with analytical solution

Define a path:
-------------

General Postproc>Path Operations>Define Path>By location>Name=y0.25, nDiv=16,OK
  >NPT=1, X=0.,y=0.25, z=0, OK> NPT=2, X=.305,y=0.25, z=0, OK> Cancel

Map the variable to be plotted on the path:
------------------------------------------

General Postproc>Path Operations>Map onto Path>Lab=T, Selection=Temperature>OK

Plot the results:
------------------

Utility Menu>Plot>Results>Path Plot>Select T>OK

Save the data for comparision with analytical results:
------------------------------------------------------

Utility Menu>List>Results>Path Data>Select XG,T>OK
File>Save as>results16.dat>OK>close

9. Contour plot

General Postproc>Plot Results>Contour Plot/Nodal Solu >OK

Note: For line contours, use 
    /show,x11,,1

Note that you can perform a full three-D solution with ANSYS and compare that with the 2D results.