Chapter 4: An Overview of Postprocessing
Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index
Chapter 1 *
Chapter 2 *
Chapter 3 *
Chapter 4 *
Chapter 5 *
Chapter 6 *
Chapter 7 *
Chapter 8 *
Chapter 9 *
Chapter 10 *
Chapter 11 *
Chapter 12 *
Chapter 13 *
Chapter 14 *
Chapter 15 *
Chapter 16 *
Chapter 17 *
Chapter 18 *
Chapter 19
4.1 What Is Postprocessing?
After building the model and obtaining the solution, you will want answers to some
critical questions: Will the design really work when put to use? How high are the
stresses in this region? How does the temperature of this part vary with time? What
is the heat loss across this face of my model? How does the magnetic flux flow
through this device? How does the placement of this object affect fluid flow? The
postprocessors in the ANSYS program can help you answer these questions and
others.
Postprocessing means reviewing the results of an analysis. It is probably the
most important step in the analysis, because you are trying to understand how the
applied loads affect your design, how good your finite element mesh is, and so on.
Two postprocessors are available to review your results: POST1, the general
postprocessor, and POST26, the time-history postprocessor. POST1 allows you
to review the results over the entire model at specific load steps and substeps (or
at specific time-points or frequencies). In a static structural analysis, for example,
you can display the stress distribution for load step 3. Or, in a transient thermal
analysis, you can display the temperature distribution at time = 100 seconds. The
contour plot in Figure 4-1 is a typical POST1 plot.
Figure 4-1 A typical POST1 contour display
POST26 allows you to review the variation of a particular result item at specific
points in the model with respect to time, frequency, or some other result item. In a
transient magnetic analysis, for instance, you can graph the eddy current in a
particular element versus time. Or, in a nonlinear structural analysis, you can
graph the force at a particular node versus its deflection. The graph in Figure 4-2
is a typical POST26 plot.
Figure 4-2 A typical POST26 graph
It is important to remember that the postprocessors in ANSYS are just tools for
reviewing analysis results. You still need to use your engineering judgment to
interpret the results. For example, a contour display may show that the highest
stress in the model is 37,800 psi. It is now up to you to determine whether this
level of stress is acceptable for your design.
4.2 The Results Files
The ANSYS solver writes results of an analysis to the results file during solution.
The name of the results file depends on the analysis discipline:
Jobname.RST for a structural analysis
Jobname.RTH for a thermal analysis
Jobname.RMG for a magnetic field analysis
Jobname.RFL for a FLOTRAN analysis
For a FLOTRAN analysis, the file extension is .RFL. For other fluid analyses, the
file extension is .RST or .RTH, depending on whether structural degrees of
freedom are present. (Using different file identifiers for different disciplines helps
you in coupled-field analyses where the results from one analysis are used as
loads for another. The ANSYS Coupled-Field
Analysis Guide presents a complete description of coupled-field analyses.)
4.3 Types of Data Available for
Postprocessing
The solution phase calculates two types of results data:
- Primary data consist of the degree-of-freedom solution calculated at each
node: displacements in a structural analysis, temperatures in a thermal
analysis, magnetic potentials in a magnetic analysis, and so on (see Table
4-1). These are also known as nodal solution data.
- Derived data are those results calculated from the primary data, such as
stresses and strains in a structural analysis, thermal gradients and fluxes in
a thermal analysis, magnetic fluxes in a magnetic analysis, and the like.
They are typically calculated for each element and may be reported at any
of the following locations: at all nodes of each element, at all integration
points of each element, or at the centroid of each element. Derived data
are also known as element solution data, except when they are averaged
at the nodes. In such cases, they become nodal solution data.
Table 4-1 Primary and derived data for different disciplines
| Discipline
|
Primary Data
|
Derived Data
|
| Structural
|
Displacement
|
Stress, strain, reaction, etc.
|
| Thermal
|
Temperature
|
Thermal flux, thermal gradient, etc.
|
| Magnetic
|
Magnetic Potential
|
Magnetic flux, current density, etc.
|
| Electric
|
Electric Scalar Potential
|
Electric field, flux density, etc.
|
| Fluid
|
Velocity, Pressure
|
Pressure gradient, heat flux, etc.
|
Go to the beginning of this chapter