p1: Viewing X-Sectional Results using ansys

Introduction

This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to view cross sectional results (Deformation, Stress, etc.) of the following example.

Preprocessing: Defining the Problem

Give example a TitleUtility Menu > File > Change Title ...
/title, Cross-Sectional Results of a Simple Cantilever Beam
Open preprocessor menuANSYS Main Menu > Preprocessor
/PREP7
Create BlockPreprocessor > Modeling > Create > Volumes > Block > By 2 Corners & Z
BLC4,0,0,Width,Height,Length
Where: Width: 40mm
Height: 60mm
Length: 400mm
Define the Type of Element

Preprocessor > Element Type > Add/Edit/Delete...For this problem we will use the SOLID45 (3D Structural Solid) element. This element has 8 nodes each with 3 degrees of freedom (translation along the X, Y and Z directions).

Define Element Material Properties
Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > IsotropicIn the window that appears, enter the following geometric properties for steel:
1. Young's modulus EX: 200000
2. Poisson's Ratio PRXY: 0.3
Define Mesh SizePreprocessor > Meshing > Size Cntrls > ManualSize > Global > Size
esize,20For this example we will use an element size of 20mm.
Mesh the volumePreprocessor > Meshing > Mesh > Volumes > Free > click 'Pick All'
vmesh,all

Solution: Assigning Loads and Solving

Define Analysis Type

Solution > Analysis Type > New Analysis > Static
ANTYPE,0

Apply Constraints

Solution > Define Loads > Apply > Structural > Displacement > On Areas
Fix the left hand side (should be labeled Area 1).

Apply Loads

Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints
Apply a load of 2500N downward on the back right hand keypoint (Keypoint #7).

Solve the System

Solution > (-Solve-) Current LS
SOLVE

Postprocessing: Viewing the Results

Now since the purpose of this tutorial is to observe results within different cross-sections of the colume, we will first outline the steps required to view a slice.

Offset the working plane for a cross section view (WPOFFS)

Select the TYPE of display for the section(/TYPE). For this example we are trying to display a section, therefore, options 1, 5, or 8 are relevant and are summarized in the table below.

Type	Description	Visual Representation
SECT or (1)	Section display. Only the selected section is shown without any remaining faces or edges shown
CAP or (5)	Capped hidden diplay. This is as though you have cut off a portion of the model and the remaining model can be seen
ZQSL or (8)	QSLICE Z-buffered display. This is the same as SECT but the outline of the entire model is shown.

Align the cutting plane with the working plane(/CPLANE)

DeflectionBefore we begin selecting cross sections, let's view deflection of the entire model.
- Select: General Postproc > Plot Results > Contour Plot > Nodal Solu
  From this one may wish to view several cross sections through the YZ plane.
To illustrate how to take a cross section, let's take one halfway through the beam in the YZ plane
- First, offset the working plane to the desired position, halfway through the beam
  Select: Utility Menu > WorkPlane > Offset WP by Increments
  In the window that appears, increase Global X to 30 (Width/2) and rotate Y by +90 degrees
- Select the type of plot and align the cutting plane with the working plane (Note that in GUI, these two steps are combined)
  Select: Utility Menu > PlotCtrls > Style > Hidden-Line OptionsFill in the window that appears as shown below to select /TYPE=ZQSL and /CPLANE=Working Plane
  
  As desired, you should now have the following:
  
  This can be repeated for any slice, however, note that the command lines required to do the same are as follows:
```
WPOFFS,Width/2,0,0      ! Offset the working plane for cross-section view
WPROTA,0,0,90           ! Rotate the working plane
/CPLANE,1               ! Cutting plane defined to use the WP
/TYPE,1,8
PLNSOL,U,SUM,0,1
    
```
  Also note that to realign the working plane with the active coordinate system, simply use: WPCSYS,-1,0
Equivalent StressAgain, let's view stresses within the entire model.
- Select: General Postproc > Plot Results > Contour Plot > Nodal Solu > Stress > von Mises
  Let's say that we want to take a closer look at the base of the beam through the XY plane. Because it is much easier, we are going to use command line:
```
WPOFFS,0,0,1/16*Length    ! Offset the working plane
/CPLANE,1                 ! Cutting plane defined to use the WP
/TYPE,1,5                 ! Use the capped hidden display
PLNSOL,S,EQV,0,1
    
```
  Note that we did not need to rotate the WP because we want to look at the XY plane which is the default). Also note that we are using the capped hidden display this time.
  You should now see the following:
AnimationNow, for something a little more impressive, let's show an animation of the Von Mises stress through the beam. Unfortunately, the ANSYS commands are not as user friendly as they could be... but please bear with me.
- Select: Utility Menu > PlotCtrls > Animate > Q-Slice Contours
- In the window that appears, just change the Item to be contoured to 'Stress' 'von Mises'
- You will then be asked to select 3 nodes; the origin, the sweep direction, and the Y axis. In the graphics window, select the node at the origin of the coordinate system as the origin of the sweep (the sweep will start there). Next, the sweep direction is in the Z direction, so select any node in the z direction (parallel to the first node). Finally, select the node in the back, bottom left hand side corner as the Y axis.You should now see an animated version of the contour slices through the beam. For more information on how to modify the animation, type help ancut into the command line.