9.2  ANSYS

 

9.2.1        Brief Introduction To Ansys

 

The ANSYS has 6 windows at the beginning. These are shown in the following figure. Typical steps to perform finite element analysis are shown in the table below in sequence.

 

Table 6.3-1Typical ANSYS procedure

Preferences

Disciplines in Application

Structural

Choose one

Thermal

Ansys Fluid

Flotran CFD

Magnetic-Nodal

Magnetic-Edge

High Frequency

Electric

Structural Discipline

h-method

Choose one

p-method

Preprocessor

Element Type

 

 

Real Constants

Material Properties

Sections

Modelling

Attributes

Mesh Tools

Meshing

Controls …

Coupling / Ceqn

Flotran Setup

Loads

Physics Environment

Solution

Analysis Type

 

 

Analysis Options

 

 

Loads

Settings

 

Apply

 

Delete

 

Operate

 

Load Step Options

 

 

Physics Environment

 

 

Solve

Current LS

 

Flotran Setup

 

 

Run Flotran

 

 

General Postprocessing

 

 

 

Others …

 

 

 

 

Figure 9.2.1-1   Typical ANSYS 7.1 display window

 

 

 


Example 9.2-1 A L-shaped beam is to be modeled with three-dimensional solid. The size is 1 in x 1 in x 5 in and the thickness is 0.5 in. Use Copy and Skinning to create the areas, and then volume from areas.

Figure 9.2-2  Volume created by skinning

Solution:

 

1.                  Create a section by starting with keypoints [Create > Keypoints > On Working Plane > click on “WP Coordinates” in the dialog > enter the points in the input window like 0,0 > CR > repeat this for all points]. Now lines are created by keypoints [Create > Lines > Straight Line > pick on two keypoints for a line > repeat this for all lines]. Next create an area [Create > Area > Arbitrary > By Lines > select all lines]

2.                  Copy this area to the other end [Modeling / Copy > Areas > pick on the area > Ok > enter the offset distance Z-offset distance in active CS = 5 > Ok]

3.                  Having two sections created, connect the lines to create surface areas [Create > Areas > Arbitrary > By Skinning > pick on two lines, one each from both areas > Apply > repeat this to create all surface areas]

4.                  Now create the volume [Create > Volume > Arbitray > By Areas > Pick All]. You may want to display the volume by [Utility Menu / Plot > Volumes].

 

 


Example 9.2-2 A L-shaped beam is to be modeled with three-dimensional solid. The size is 1 in x 1 in x 5 in and the thickness is 0.5 in. Use Extrude to create the mesh.

Figure 9.2-3 Extruded mesh of a L-shape beam

Solution:

 

  1. First add two element types, one for area on a section and the other for volume.  [Preprocessor > Element Types > Add / Edit /Delete > Add > Solid / Plane42 > Apply > Solid / Sold45 > Ok].
  2. Create a section by starting with keypoints [Create > Keypoints > On Working Plane > click on “WP Coordinates” in the dialog > enter the points in the input window like 0,0 > CR > repeat this for all points]. Now lines are created by keypoints [Create > Lines > Straight Line > pick on two keypoints for a line > repeat this for all lines]. Next create an area [Create > Area > Arbitrary > By Lines > select all lines]
  3. A free mesh on the created section will be used. Let’s first clear the size controls if any to have free mesh shape (not regular shape) as the figure [Meshing > Shape & Size > Lines / Ctlr Size > Pick All > Ok]. Then, create free mesh with Plane42 element. This is the first element type added and the default element type now. [Mesh > Areas / Free > select the area > Ok]. The mesh may be too coarse. Refine it [Mesh > Refine > Elements > pick the area > just accept the default values for refine in the dialog > Ok]. You should see a similar free  mesh on the section.
  4. Now, change the attribute (i.e., element type in this case) to Solid45 before volume mesh [Meshing / Attributes > Default Attributes > change the element type to 2 for Solid45 > Ok]. Extrude the area mesh by [Modeling / Operate > Extrude / Sweep > (now specify size attribute for extruded direction) Elem Ext Opts > No. Element Division = 5 (or Default Attributes / Size in old version of Ansys > NDIV = 5) > Ok > Areas / Along Normal > pick on the area with mesh > Ok > specify the length of extrusion, say 5 > Ok].
  5. You may want to display element by [Utility Menu / Plot > Elements]. The resulting mesh is the figure above.
  6. Clear the area mesh that may cause wrong results before any analysis [Meshing / Clear > Areas > Select All].

 

 


Example 9.2-3 A pipe has an inner radius 4.75 in, thickness 0.25 in, and the length 200 in. Assuming thate a structural analysis is required in the middle of the pipe (for 20 in long span), create a model and mesh it with brick element.

Figure 9.2-4 Hollow cylinder and dialog

Solution:

 

Since the pipe is long, but an analysis can be done only in the middle section, the model will be created in three sections longitutinally: (-100,-10), (-10,10), (10,100). Then, surface mesh will be created with mesh controls that will be swept to create volume mesh.

1.                  Create the pipe [Preprocessor > Modeling > Create > Volumes > Cylinder > By Dimensions > enter values for middle section as in the dialog above > Apply > enter the left section values with z = (-100,-10) > Apply > z = (10,100) for right section > OK]. Note the z2 must be greater than z1 in the dialog. z = (10, -100) will be interpreted as (10, 100).

2.                  Glue the volumes [Modeling > Operate > Boolean > Glue > Volumes > Pick All > OK]. This glues the volumes (i.e., common areas and lines will be merged at interfaces).

3.                  Add element types [Element Types > Add > Solid > Quad 4 node (PLANE42) > Apply > Brick 8 node (SOLID45) > OK]

4.                  Display the display control menu by [Util Menu: PlotCtrls > Pan, Zoom, Rotate > the menu appears on the right side of the window > click zoom menu  and zoom in the middle section as

   

 

5.                  Specify the mesh attributes for surface element and volume element [Meshing > Mesh Attributes]

a.                               [Picked Areas > pick both end surfaces of the middle pipe > OK > Element type number (TYPE) = 1 PLANE42 > OK]

b.                              [All Volumes > TYPE = 2 SOLID45 > OK]

6.                  Control the surface and volume meshes of the middle section. [Meshing > Size Controls > Manual Size > Lines[> Picked Lines]

a.                               [pick all lines defining the end surfaces of the middle pipe as below (there are eight lines on each surface) > OK > enter number of element division (NDIV) 20 > OK]

b.                              [pick axial lines defining the middle pipe (there are four lines) as shown below > OK > enter number of element division (NDIV) 40 > OK]

           

 

c.                               Zoom out and pick axial line division for outer pipes and specify NDIV = 80

7.                  Create surface mesh [Mesh > Areas > Free > pick both surfaces > OK]

8.                  Create the volume mesh [Mesh > Volume Sweep > Sweep > pick middle pipe > Apply (see the mesh generation) > pick one of outer pipe > Apply > pick the last pipe > OK]. Note all volumes could have been picked all at the same time. The mesh appears

Figure 9.2-5 Volume mesh created by [Volume Sweep]

9.                  Clear the area mesh that may cause wrong results before any analysis [Meshing / Clear > Areas > Select All].

 

 


Example 9.2-4 A 10 in long I-beam is subjected to a shear force 3000 lbf at one end section and fixed at the other end. Analyze the deformation, stresses, forces, and moments in the beam. Also, compare the numerical results with analytical solution by strength of materials. The material is AISI C1020 Steel (E =  30.023 x 106 psi and ν = 0.29). The thickness of the beam t is 1/2 in, b 1 in, W 2.5 in, and the height H 4 in.

 

   

Figure 9.2-6 Dimensions of an I-beam and sample meshes

Solution:

 

q       Preparation

 

1.      Select preferences [Preferences > Structure / h-method > Ok]

2.      Add two element types, one for volume and the other for area [Preprocessor > Element Type > Add/Edit/Delete > Add > Solid / Brick 8node 45 > Apply > Solid / Quad 4node 42 > Ok]

3.      Import material properties from the Ansys library [Material Properties > (if you want, specify Library Path if not done before) > Import > pick Steel AISI C1020 > Ok]

 

q       Modeling

 

4.      Create the rectangular section and subtract two flank rectangles.

a.       [Modeling / Create > Areas > Rectangle > By 2 Corners > enter values for –W/2,–H/2 and W/2, H/2  > Apply > enter two corners of the left flank rectangle > Apply > repeat this for the other flank rectangle > Ok]

b.      [Modeling / Operate > Booleans / Subtract > pick on the full section > Apply > pick on two flank rectangles > Ok]

5.      For meshing the current irregular area is divided into smaller rectangles. For this operation, some lines are needed.

a.                   [Modeling / Operate > Extend Line / pick on a line to extend > Apply > pick on one end to extend > Apply > enter the length to exten > Apply]. Repeat this for other lines.

b.                  [Modeling / Operate > Booleans / Divide > Area by Line > pick on an area > Apply > pick a dividing line > Apply]. Repeat this for other areas.

6.      Now, there may be multiple lines and keypoints at the same positions. Merge them by [Preprocessor / Numbering Ctrls > Merge Items > All > Ok]

7.      If you have created areas separately, they should be now joined to make one piece for FEM analysis. One method is [Modeling / Operate > Glue > Areas > Pick All]

 

Note that the areas can be created starting with keypoints, then creating lines with keypoints, and finally creating areas by lines. When creating an area by lines and skinning, the sequence of lines defines the area normal and must be selected accordingly. The second figure below shows two areas extruded in the directions of two opposite area normals. Before extrusion of an area, check the sequence of lines that make up the area to find out the direction of area normal.

 

q       Meshing

 

8.      Select the right attributes for area by [Meshing / Attributes > All Areas > Element Type = 2 > Ok].

9.      Control the meshing on the edges as you like [Meshing / Shape & Size > Lines / Picked Lines > pick lines > Apply > specify number of divisions on the selected lines > Apply]. Repeat this for other lines as needed. Also, know that the divisions can be cleared to default any time by [Shape & Size > Manual Size / Lines / Ctlr Size or Keypoints / Ctlr Size]. The number of divisions on lines can be displayed any time by [Util Menu / Plot > Lines]

10.  Mesh the areas by [Meshing / Mesh > Areas / Mapped or Free (since the area is regular shape, either will give same results) > pick on the middle section first > Apply]. Repeat this for other areas. [Pick All] could have been used to pick all at the same time, but sometimes, it is wiser to begin with most complicated shape of domain and move to less complicated domains for meshing.

11.  Extrude the area mesh to make volume mesh

a.                   Specify the attributes first by [Meshing / Attributes > Default Attributes > Element Type = 1 > Ok]. Since there is no volume yet that is to be created, this default attribute is only one to be used.

b.                  Specify the number of elements to be used in the extruded direction by [Modeling / Operate > Extrude / Sweep > Areas > Default Attribs / Size > NDIV = 5 > Ok]

c.                   Now extrude the area (this automatically extrude with mesh) by [Operate > Extrude / Sweep > Areas > Along Normal > pick an area > Apply > enter length of extrusion 10 > Apply]. Repeat this for all areas.

d.                  Merge iterms once again by [Preprocessor > Numbering Ctrls > Merge Items > All > Ok]. The mesh may look similar to the following.

12.  Clear the area mesh that may cause wrong results before any analysis [Meshing / Clear > Areas > Select All].

 

 

q       Boundary Conditions and Solution

 

13.  Apply the boundary conditions

a.                   At fixed end by [Solution > Loads / Apply > Displacement > On Nodes > rotate the model and click Box in the dialog for box picking > pick all nodes at fixed end > Ok > All DOF > Ok]

b.                  Apply the shearing force at the free end by distributing the total force to all nodes. At this point, try to learn how to use a utility menu Select as [Util / Select > Entities > Areas / By Num/Pick / From Full > Ok > select all areas at the free end > Apply]

c.                   Now, select all nodes on these active areas by [Nodes / Attached to / Areas all / Reselect > Select All]. The selected nodes can be displayed by [Util / Plot > Nodes]

d.                  [Apply > Force / Moment > On Nodes > Pick All > Fy / enter value 100 (for coarse mesh, there are 30 nodes)]

e.                   Reselect everything to be active by [Uitl / Select > Everything]

f.                   [Util / Plot > Elements]. The plot should show mesh and boundary conditions as

 

14.  Solve the problem by [Solve / Current LS > Ok > close the dialog and data]

 

q       Postprocessing

 

15.   [General Postprocessing / Plot Results > Contour Plot / Nodal Solution > Stress / SX / Def + Undef edge > Ok]. The solution is shown below for bending stress SZ, von Mises stress, and shear stress on the section.

 

 

Figure 9.2-7 Bending stress, von Mises stress, and shear stress on the beam section

 

q       Discussion

 

The solution may not be accurate yet due to coarse mesh. Try it again with refined mesh and compare the results with the previous to see if the solution has converged. Repeat this until two successive solutions are close enough to stop.

 

The analytical solution by strength of materials can be roughtly obtained by

 

            ,

 

where the bending moment was calculated by nodal force (100 lbf / node) times the number of applied nodes times the beam length. The numerical bending and shear stresses, 5564 and 1896 psi, respectively, compare very well with the analytical values.

 

 

 


Example 9.2-5 A hollow pipe is fixed at one end and subjected to a twisting moment at the other end. Model the pipe with half section as shown below, mesh with 8 elements, and extrude 10 in with 5 elements and again with 1 in with one element, then use reflection to complete the meshing. Apply the twisting load on the last cylindrical surface of length 1 in. Solve the problem and display the tangential displacements and stresses. Compare the results with analytical results.  The pipe has outer radius 1 in, thickness 0.2 in, and length 11 in. The material is AISI C1020 Steel (E =  30.023 x 106 psi and ν = 0.29).

 

 

Figure 9.2-8 Mesh on half section and extruded mesh

Solution:

 

q       Preparation

 

1.      Preferences > Structure / h-method > Ok

2.      Add two element types for extruded volume and section area by [Preprocessor > Element Type > Add/Edit/Delete > > Add > Solid / Quad 4node 42 > Apply > Add > Solid / Brick 8node 45 > Ok]

3.      Material Properties > Import Library > BIN > Ok > Browse > find the Ansys installation directory and its subdirectory “matlib” and pick on “Stl_AISI_C1020.BIN_MPL” > Open > Ok

 

q       Modeling and Meshing

 

4.      First, create the half section by [Modeling > Create > Areas > Circle > Partial Annulus > enter 0, 0, 0.8, 90, 1, 270 > Ok]

5.      Before meshing this area, control the size by [Meshing > Shape & Size > Lines / Picked Lines > pick two arcs > enter NDIV=8 > Apply > pick two end lines > NDIV = 1 > Ok]

6.      Change the attributes and mesh the section

a.                   [Meshing > Attributes > Default Attr > Element Type = 1 (i.e., PLANE42) > Ok]

b.                  [Meshing > Mesh > Areas > Free > Pick All]. Now the mesh on the half section should be like the one above.

7.      Create volume and mesh

a.                   [Meshing / Attribute > Default Attribute > Element Type = 2 (i.e., SOLID45) > Ok]

b.                  [Modeling / Operate > Extrude / Sweep > Default Attribute / Size > NDIV=5 > Ok > Areas / Along Normal > pick an area > Apply > Length of extrusion = 10 > Apply].

8.      Clear the area mesh that may cause wrong results [Meshing / Clear > Areas > Select All].

9.      Extrude once more from the end of the extruded volume for the area on which a twisting load is to be applied.

a.                   [Modeling / Operate > Extrude / Sweep > Default Attribute / Size > NDIV=1 > Ok > Areas / By XYZ Offset* > pick the section area at end of extruded volume > Apply > Length of extrusion = 1 > Apply]. * Along Normal option yields distorted mesh in.

10.  Reflect the volume (mesh is automatically reflected together) by [Modeling > Reflect > Volumes > pick the volume > Ok > plane of symmetry = YZ plane (i.e., along X-axis) > Ok].

11.  Join two meshed volumes. Also, there may be multiple points, lines, nodes at the same positions along the joint areas. [Number Ctrls > Merge Items > Type of items to mover = All > Ok]

 

q       Boundary Conditions

 

12.  First apply the fixed boundary conditions at one end by [Solution / Loads > Apply > Dispalcement > On Nodes > rotate the model and select all nodes on the end surface by Box picking them > All DOF > Ok]

13.  The twisting force will be applied on all nodes on the last cylindrical surface.

a.                   First select all nodes on that surface by [Util / Select > Areas > By Num/Pick / From Full > Ok > pick all areas on the last outer cylindrical surface > Ok]

b.                  Type in [nsla,,1 > CR] in the input window to select all nodes on the selected active areas. Or use [Util / Select > Nodes / Attached to / Areas all / Reselect > Select All > Ok]. You may plot all selected nodes to check by [Util / Plot > Nodes].

c.                   The applied twisting loads must be tangent to the cylindrical surface. Change the active coordinate system by [Uitl / WorkPlane > Active Coordinate System > Global Cylindridal]. Now, the x, y, z directions represent r,q, z directions.

d.                  [Solution / Loads > Apply > Force/Moment > On Nodes > Pick All > FY = 100 > Ok].

e.                   Now, align the nodal coordinate system to global cylindrical coordinate system [Preprocessor / Modeling > Move / Modify > Rotate Node CS > To Active CS > Pick All]. You can replot the graph. The load should appear like the first figure below.

 

 

 

14.  Select back everything to be active by [Util / Select > everything] and plot elements.

15.  Plot the boundary conditions by [Util / Plot Ctrls > check Applied B.C.s  > Ok]. The boundary conditions appear on the mesh as in the second figure above.

16.  Solve the problem [Solve > Current LS > Ok]

 

q       Results and Discussion

 

17.  [General Postprocessing > Plot Results > Contour Plots > Nodal DOF > Displacement / UY / def + org edge > Ok]. The following figures (a) and (b) show results of displacement UY and stress SYZ in global Cartesian coordinate. These do not tell much for analysis.

18.  Change the results coordinate system to global cylindrical system by [Postprocessing > Options for Output > Results coordinate system = Global Cylindrical System > Ok]

19.  Now, the results can be reploted by [Util / Plot > Replot]. The figures (c) and (d) show the displacement Uq and and stress gzq in global cylindrical coordinate system. The last figure shows the von Mises stresses that does not depend on any coordinate system.

 

 

                                (a)                                                                  (b)

    

                                (c)                                                                  (d)

                                (e)

Figure 9.2-9 (a) UY and (b) SYZ in Cartesian coordinate system, (c) UY (i.e., uq) and (d) SYZ (i.e., gzq) in cylindrical coordinate system, (e) von Mises stresses

 

The approximate analytical solution for tangential shear stress can be obtained first by force equilibrium (i.e, internal and external forces)

 

 

The tangential displacement then is obtained by

 

 in.

 

where q is the angle of twist, g shear strain, and G shear modulus. The numerical results of tangential stress 3144 psi and tangential displacement 0.00328 are quite comparable to approximate analytical solutions.

 

 

 


Example 9.2-6 A disc in the automotive brake is model by T-shaped beam bent along a 90o arc of radius 10 inch through the centrod. The disc is subjected to the pressure of 200 psi on the external surface. (a) Create finite element mesh with 8-node brick elements by extrusion. With appropriate boundary conditions solve the problem and display the hoop stress along the circumference of the disc. The section is three inch wide at the base, total four inch high, and one inch thick. Material is steel AISI C1020.

Figure 9.2-10 Extruded mesh of a T-shape beam

Solution:

 

q                   Modeling

 

  1. First add two element types, one for area on a section and the other for volume.  [Preprocessor > Element Types > Add / Edit /Delete > Add > Solid / Plane42 > Apply > Solid / Sold45 > Ok].
  2. Create two rectangles by [Create > Areas > Rectangle > By Dimensions > enter the min/max x, y-coordinates > Apply > repeat this for the other area > Ok].
  3. Merge common entities by [Preprocessor /  Numbering Ctrls > Merge Items > All > Ok]. This will merge all common entities at same positions including nodes and has effect of glueing two separate extruded meshes for finite element analysis.
  4. Three keypoints are created, from which an arc for Extrude will be created

a.                   [Create > Keypoints > In Acitve CS > enter keypoint number 11 and the coordinates 0, 0, 0 > Apply > repeat this with keypoint number 12 and coordinates 0, 10, 10 > Apply > keypoint 13 and 0, 10, 0 > Ok]

b.                  [Create > Lines / Arc > By End KPs & Rad > pick on two keypoints for two end keypoints > Ok > pick a keypoint on the side of center of arc > Ok]

  1. Create area mesh [Meshing > Mesh > Areas / Mapped > 3 or 4 sided > Pick All]
  2. Create volume mesh by extrusion

a.                   For Ansys 6.x and old,

                                i.                                    [Meshing / Attribute > Default Attribute > change the element type to 2 (i.e., Solid45) > Ok]

                              ii.                                    [Modeling / Operate > Extrude / Sweep > Default Attribute / Size > enter NDIV = 6 > Areas > Along Lines > pick both areas > Apply > pick the arc > Ok]

b.                  For Ansys 7.x

                                i.                                    [Modeling / Operate > Extrude

a.       [Elem Ext Opts > in the dialog shown below select SOLID45 for Element Type (TYPE) and enter 6 for number of element divisions > Ok]

 

b.      [Areas > Along Lines > pick the areas > Ok > pick the arc > Ok]

 

  1. [Operate > Extrude > Mesh > Areas / Mapped > 3 or 4 sided > Pick All]
  2. Merge common entities by [Preprocessor /  Numbering Ctrls > Merge Items > All > Ok].
  3. Clear the area mesh by [Meshing > Clear > Area > pick the areas meshed at the beginning]. If the area mesh is not cleared, the results near this meshed area may not be right.

 

q                   Solution

 

  1. Apply the boundary conditions [Solution > Define Loads > Apply > Structural]

a.                   [Displacement > Symmetric B.C. / On Areas > pick areas on both end sections > Ok]

b.                  [Pressure > Areas > pick on the outer surface > enter value 200]

c.                   The model still can move in the third direction. Apply symmetric boundary condition at bottom front face.

  1. Solve the problem [Solution > Solve > Current LS > Ok]

 

q                   Postprocessing and Discussion

 

  1. Since the circumferential direction is not aligned with any existing axes, create a local coordinate system [Util Menu : WorkPlane > Local Coordinate Systems > Create Local CS > By 3 Keypoints > pick a keypoint at (0, 10, 0) for origin, next keypoint for x-axis at (0, 10, 10), and select the last at (0, 0, 0) for y-axis > enter Reference number 11 and choose Cylindrical for Type of coordinate system > Ok]
  2. Change the results coordinate system for results display by [General Postprocessor > Options for Output > choose Local Coordinate System for Results coordinate system and enter 11 for Local system reference no. > Ok]
  3. [Plot Results > Contour Plot > Nodal Solution > Stress / SY (i.e., θ-direction in local coordinate system) and pick Def + undef edge > Ok]. Also, examine the von Mises stress.

 

  

Figure 9.2-11 Hoop stress and von Mises stress

 

Note that if you don’t see the expected axisymmetric results, look closely at the joint of two volumes. There may be separate deformations due to separate volumes. Go back and merge them all and re-solve the problem.