// // Leave a Comment

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


  1. Give example a TitleUtility Menu > File > Change Title ...
    /title, Cross-Sectional Results of a Simple Cantilever Beam
  2. Open preprocessor menuANSYS Main Menu > Preprocessor
    /PREP7
  3. Create BlockPreprocessor > Modeling > Create > Volumes > Block > By 2 Corners & Z
    BLC4,0,0,Width,Height,Length
    Where:Width:40mm
    Height:60mm
    Length:400mm
  4. Define the Type of Element
  5. 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).
  6. Define Element Material PropertiesPreprocessor > 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
  7. Define Mesh SizePreprocessor > Meshing > Size Cntrls > ManualSize > Global > Size
    esize,20For this example we will use an element size of 20mm.
  8. Mesh the volumePreprocessor > Meshing > Mesh > Volumes > Free > click 'Pick All'
    vmesh,all

Solution: Assigning Loads and Solving


  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Static
    ANTYPE,0

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

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

  7. Solve the System
  8. 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.
    TypeDescriptionVisual 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)

  1. 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
  2. Equivalent StressAgain, let's view stresses within the entire model.
      First we need to realign the working plane with the active coordinate system. Select: Utility Menu > WorkPlane > Align WP with > Active Coord Sys (NOTE: To check the position of the WP, select Utility Menu > WorkPlane > Show WP Status)
      Next we need to change /TYPE to the default setting(no hidden or section operations). Select: Utility Menu > PlotCtrls > Style > Hidden Line Options... And change the 'Type of Plot' to 'Non-hidden'

    • 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:
  3. 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.

0 comments:

Post a Comment