Fall 2002, METBD 440/451 - FEA Dynamics Applications

Prof. Dave Johnson, dhj1@psu.edu, Penn State - Erie, The Behrend College

General Transient Analysis Template

Reference:  ANSYS Structural Analysis Guide, Chapter 5: Transient Dynamic Analysis

• Any nonlinearities, such as plasticity, large deflections, and contact (gap) elements, are INCLUDED

• Applied loads may have ANY form: impulse, saw-tooth, sq. wave, harmonic, etc. 
  [M]{d²x/dt²} + [C]{dx/dt} + [K]{x} = {Fo(t)}

• Transient or start-up effects ARE computed.

• Solution is performed in the Time Domain

1) Build the model (remember, you must have stiffness & mass)

General Transient analyses can include plasticity, contact elements, large deformation, stress stiffening, (i.e., nonlinear behavior), as well as, transient response (start-up or shut down) simulations

2) Enter the ANSYS Solution processor

3) (Optional) Use 'Reset Options..' if you have used this model for a previous analysis.

4) Pick 'New Analysis' - set it for 'Transient' Analysis

5) Pick 'Analysis Options..' - choose Solution Method (Default is Full)

• usually take default on lumped mass option
• take the defaults for Full Transient Analysis Options, unless you want large deformation, stress stiffening, or other solver options.

6) Define any constraints on the system

7) Define any forces, pressure, or imposed, non-zero displacements for the first solution step
    Establishing the proper INITIAL CONDITIONS is important.

8) Under 'Time/Frequenc>' set up the 'Time & Time Step...'

• Specify the time at the end of this load step
• Define the time step size
• Choose Stepped or Ramped B.C.'s
• Activate Automatic time stepping, if appropriate
  for Automatic time stepping: Define the min. and max. time step size
• In the Full Transient analysis, you are integrating over time.  The time step size effects the accuracy of the numeric integration.

9) Under 'Time/Frequenc>' set up the 'Time Integration..'

• Set Time Integration ON or OFF, as needed
• usually, take defaults for integration parameters

10) Under 'Output Ctrls > DB/Results File...' to control the output for postprocessing

11) 'Write LS File ...'

12) Specify any CHANGES in B.C.'s or loads for the next load step

13) Repeat Steps 8-12 for all solution load steps

14) Solve from LS Files

15) Postprocessing (General Postproc>):

• Use 'Results Summary' to see what solutions are available.
• Use 'First Set' to look at the first solution (displacements, stresses, etc.)
• Use 'By Time/Freq...' to look at a particular solution

16) Use 'TimeHist Postpro' to graph results vs. time

• Using the "Variable Viewer" in ANSYS 6.1
• Add Data, 'Nodal Solution,' 'DOF Solution' or 'Stress', etc.
• Add Data, 'Reaction Forces,' 'Structural Forces,' and the force component direction
• Give each variable a short, descriptive name
• May need to pick a node, give the node number [or use node(x,y,z)]
• Pick the result you want to use.
• Graph or List the response vs. frequency
• use PlotCtrls > Style > Graphs > ... to format axes, scales, labels, etc. on graphs
• Operate on the data with 'Math Operations>' and plot with 'Graph Variables...'