Plate with a Hole

Problem Specification

Consider the square plate of uniform thickness with a circular hole with dimensions shown in the figure below. The thickness of the plate is 1 mm. The Young's modulus E =10⁷ MPa and the Poisson ratio is 0.3. A uniform pressure p=1 MPa acts on the boundary of the hole. Assume that plane stress conditions prevail. The stress and displacement fields are to be determined using ANSYS. This problem is taken from section 6.14, p. 240-244 of Cook et al.

Step 1: Start-up and preliminary set-up

Create a folder

Create a folder called plate at a convenient location. We'll use this folder to store files created during the ANSYS session.

Start ANSYS

Start > Programs > Lab Apps > ANSYS 10.0 > ANSYS Product Launcher

In the window that comes up, enter the location of the folder you just created as your Working directory by browsing to it. All files generated during the ANSYS run will be stored in this directory.

Specify plate as your Initial jobname. The jobname is the prefix used for all files generated during the ANSYS session. For example, when you perform a save operation in ANSYS, it'll store your work in a file called plate.db in your working directory.

For this tutorial, we'll use the default values for the other fields. Click on Run. For this tutorial, we'll use the default values for the other fields. Click on Run. This brings up the ANSYS interface. To make best use of screen real estate, move the windows around and resize them so that you approximate this screen arrangement. This way you can read instructions in the browser window and implement them in ANSYS.

You can resize the text in the browser window to your taste and comfort.

In Internet Explorer: Menubar > View > Text Size, then choose the appropriate font size.

In Netscape: Menubar > View > Increase Font or Menubar > View > Decrease Font.

Set Preferences

As before, we'll more or less work our way down the Main Menu.

Main Menu > Preferences

In the Preferences for GUI Filtering dialog box, click on the box next to Structural so that a tick mark appears in the box. Click OK.

Recall that this is an optional step that customizes the graphical user interface so that only menu options valid for structural problems are made available during the ANSYS session.

Enter Parameters

For convenience, we'll create scalar parameters corresponding to the plate half-width a, hole radius r, pressure p, and material properties E and v.

Utility Menu > Parameters > Scalar Parameters

Enter the parameter value for a:
a=10e-3
Click Accept.

Similarly, enter the other parameter values and click Accept after each.

r=7e-3
p=1e6
E=1e13
nu=0.3

Close the Scalar Parameters window.

We can now enter these variable names instead of the corresponding values as we set up the problem in ANSYS. This is also helpful in carrying out parametric studies where one looks at the effect of changing a parameter.

Main Menu > Preprocessor> Element Type > Add/Edit/Delete > Add...

Pick Structural Solid in the left field and Quad 4 node 42 in the right field. Click OK to select this element.

You'll now see the Element Types menu with PLANE42 as the only defined element type.

Let's take a look at the online help pages to learn about the properties of this element.

Utility Menu > Help > Help Topics

Select the Search tab, type in pictorial summary as the keyword and click List Topics. You should see Pictorial Summary as one of the topics listed; double-click on this. This brings up the Pictorial Summary of Element Types help page. Scroll down to Plane42 under Structural 2-D Solid. Note that the PLANE42 element is defined by four nodes with two degrees of freedom at each node: translations UX and UY in the (nodal) x and y-directions.

Click on the PLANE42 box to bring up the help page for this element. Read the Element Description and take a look at the figure of the element. Think about why this element is appropriate for the problem at hand. Minimize the help window.

If you actually read the Element Description for PLANE42, you'd have noticed that this element can also be used for axisymmetric problems also. In the axisymmetric case, you would choose Options for the element in the Element Types menu. Note that in the PLANE42 element type options menu that comes up, under Element behavior, you have the option of Axisymmetric. For the current problem, we'll of course use the default of Plane stress. Click Cancel to exit the PLANE42 element type options menu retaining the defaults.

Close the Element Types menu.

Main Menu > Preprocessor> Real Constants > Add/Edit/Delete > Add

This brings up the Element Type for Real Constants menu with a list of the element types defined in the previous step. We have only one element type and it is automatically selected.

Click OK.

You should get a note saying "Please check and change keyopt setting for element PLANE42 before proceeding." Close the yellow warning window and the Real Constants menu. To see what this message implies, let's again take a look at the help pages for PLANE42.

Under PLANE42 Input Summary, the documentation says that there are no real constants for this element when KEYOPT(3)=0, 1, 2.

To see what the value of KEYOPT(3) is, bring up the Element Type menu again:

Main Menu > Preprocessor> Element Type > Add/Edit/Delete > Options

K3 i.e. KEYOPT(3) is set to Plane stress. In the help page, under PLANE42 Input Summary, you can check that plane stress corresponds to KEYOPT(3)=0. Thus, there are no real constants to be specified. That's why we got the "Please check and change keyopt settings..." warning message. Of course, the ANSYS warning could have been less cryptic but what fun would that be.

Cancel the PLANE42 element type options menu, Close the Element Types menu and close the Element Type sticky menu.

Save your work

Toolbar > SAVE_DB

Step 3: Specify material properties

Main Menu > Preprocessor >Material Props > Material Models ....

In the Define Material Model Behavior menu, double-click on Structural, Linear, Elastic, and Isotropic.

We'll use the previously defined parameter names while specifying the material properties. Enter E for Young's modulus EX, nu for Poisson's Ratio PRXY. Click OK.

To double-check the material property values, double-click on Linear Isotropic under Material Model Number 1 in the Define Material Model Behavior menu. This will show you the current values for EX and PRXY. Cancel the Linear Isotropic Properties window.

When you enter parameter names, ANSYS substitutes the corresponding parameter values as soon as you click OK or Apply.

This completes the specification of Material Model Number 1. When we mesh the geometry later on, we'll use the reference no. 1 to assign this material model. Close the Define Material Model Behavior menu.

Save your work

Toolbar > SAVE_DB

Step 4: Specify geometry

Since the geometry, material properties and loading are all symmetric with respect to the horizontal and vertical centerlines, we need to model only a quarter of the plate. We will take the origin of the coordinate system to be at the center of the hole and model only the top right quadrant. We'll create the geometry by creating a square area of side a and subtracting the circular sector of radius r from it.

Create the Square

Main Menu > Preprocessor > Modeling >Create > Areas >Rectangle > By Dimensions

X1 and X2 are the x-coordinates of the left and right edges of the square, respectively. Enter 0 for X1, a for X2.

Y1 and Y2 are the y-coordinates of the bottom and top edges of the square, respectively. Enter 0 for Y1, a for Y2.

Click OK. You should see a square appear in the graphics window.

Create the Circular Sector

Main Menu > Preprocessor > Modeling > Create > Areas > Circle > Partial Annulus

WP X and WP Y are the x- and y-coordinates of the center of the circular arc. So enter 0 for both WP X and WP Y. (WP refers to the Working Plane which by default coincides with the global Cartesian coordinate system. We won't have to worry about the working plane in this friendly example.)

Rad-1 is the radius of the inner circular arc. We want to create a solid rather than an annular arc. Enter 0 for Rad-1 to create a solid arc.

Rad-2 is the (outer) radius of the arc. Since we had defined the hole radius as parameter r earlier, enter r for Rad-2.

Theta-1 and Theta-2 are the starting and ending angles of the arc, respectively. These angles need to be specified in degrees. Enter 0 for Theta-1 and 90 for Theta-2. Click OK.

This will create and draw the circular sector. You'll see a white line denoting the circular sector.

Subtract Circular Sector from Square

Main Menu > Preprocessor >Modeling > Operate > Booleans > Subtract > Areas

In the Input window, ANSYS tells you to "pick or enter base areas from which to subtract". So we pick the square area as follows: Hold down the left mouse button, move the cursor over the areas until the square is selected (it will change color) and release the left mouse button. Click OK.

In the Input window, ANSYS now tells you to "pick or enter areas to be subtracted". So select the circular sector by holding down and releasing the left mouse button. Click OK.

If you did this correctly, you will see that the circular sector has been subtracted out from the square area.

You can also select areas during the Boolean subtract operation by simply clicking on them but it becomes difficult to select areas (and other components) in this fashion in more complicated geometries. That's why I made you use the "holding-down-the-mouse-and-releasing" technique.

If you picked an area incorrectly, you can unpick it by clicking the right mouse button and selecting the area. The cursor changes to a downward arrow during an unpick operation. Right-click to return to pick mode.

Save Your Work

Toolbar > SAVE_DB

Step 5: Mesh geometry

Bring up the MeshTool:

Main Menu > Preprocessor > MeshTool

The MeshTool is used to control and generate the mesh.

Set Meshing Parameters

We'll now specify the element type, real constant set and material property set to be used in the meshing. Since we have only one of each, we can assign them to the entire geometry using the Global option under Element Attributes.

Make sure Global is selected under Element Attributes and click on Set.

This brings up the Meshing Attributes menu. You will see that the correct element type and material number are already selected since we have only one of each. Recall that no real constants need to be defined for PLANE42 element type with the plane stress keyoption.

Click OK. ANSYS now knows what element type and material type to use for the mesh.

Set Mesh Size

Instead of setting the mesh size at each boundary, we'll use the SmartSize option which enables automatic element sizing. Click on the SmartSize checkbox so that a tickmark appears in it.

The only input necessary for the SmartSize option is the overall element size level for meshing. The element size level determines the fineness of the mesh. Its value is controlled by the slider shown in the above picture. Change the setting for the overall element size level to 5 by moving the slider under SmartSize to the left.

Mesh Areas

In the MeshTool, make sure Areas is selected in the drop-down list next to Mesh. This means the geometry components to be meshed are areas (as opposed to lines or volumes). We'll use quadrilateral elements. So make sure the default option of Quad is selected under Shape. We'll also use the default of Free meshing.

Click on the Mesh button. This brings up the pick menu.

In the Input window, ANSYS tells you to "pick or enter areas to be meshed". Since we have only one area to be meshed, click on Pick All. The geometry has been meshed and the elements are plotted in the Graphics window. Close the MeshTool.

The mesh statistics are reported in the Output window (usually hiding behind the Graphics window):

** AREA 3 MESHED WITH 79 QUADRILATERALS, 0 TRIANGLES **
** Meshing of area 3 completed ** 79 elements.
NUMBER OF AREAS MESHED = 1
MAXIMUM NODE NUMBER = 104
MAXIMUM ELEMENT NUMBER = 79

Save Your Work

Toolbar > SAVE_DB

Step 6: Specify boundary conditions

Next, we step up to the plate to define the displacement constraints and loads. Recall that in ANSYS terminology, the displacement constraints are also "loads". As in the truss tutorial, we'll apply the loads to the geometry rather than the mesh. That way we won't have to reapply the loads on changing the mesh.

Apply Symmetry Boundary Conditions

ANSYS provides the option of applying a "symmetry boundary condition" along lines of symmetry.

Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > Symmetry B.C. > On Lines

Select the straight lines corresponding to the left and bottom edges (which are the lines of symmetry for this problem) by clicking on them. Click OK in the pick menu. The symbol s appears along these lines indicating that the symmetry B.C. is applied along these lines.

Apply Pressure

Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Pressure > On Lines

Select the circular arc and click OK. This brings up the Apply Pressure on Lines menu. Enter p for Value and click OK. A single red arrow denotes the pressure and the direction in which it is acting.

Check Loads

Let's check that the displacement constraints have been applied correctly.

Utility Menu > List > Loads > DOF constraints > On All Lines

Symmetry BCs are applied on lines 8 and 9. Turn on line numbering:

Utility Menu > PlotCtrls > Numbering

Turn on Line numbers and click OK. Are lines L8 and L9 the ones on which you want the symmetry BCs?

Similarly, check that the pressure is applied correctly using Utility Menu > List > Loads > Surface Loads > On All Lines. Note that VALI and VALJ would be different if the applied pressure were linearly varying along the line.

Turn off line numbering: Utility Menu > PlotCtrls > Numbering. Turn off Line numbers and click OK.

Save Your Work

Toolbar > SAVE_DB

Step 7: Solve!

Enter solution module:

Main Menu > Solution

Enter check in the Input window and press Enter.

If the problem has been set up correctly, there will be no errors or warnings reported. If you look in the Output window, you should see the message: The analysis data was checked and no warnings or errors were found.

Main Menu > Solution > Solve > Current LS

Recall from the truss tutorial that this solves the current load step (LS) i. e. the current loading conditions. In this problem also, there is only one load step.

Review the information in the /STATUS Command window. Close this window.

Click OK in Solve Current Load Step menu.

ANSYS performs the solution and a yellow window should pop up saying "Solution is done!". Congratulations! Close the yellow window.

Verify that ANSYS has created a file called plate.rst in your working directory. This file contains the results of the (previous) solve.

Step 8: Postprocess the Results

Enter the postprocessing module to analyze the solution.

Main Menu > General Postproc

Plot Deformed Shape

Main Menu > General Postproc > Plot Results > Deformed Shape

Select Def + undeformed and click OK.

This plots the deformed and undeformed shapes in the Graphics window. The maximum deformation DMX is 0.232E-08m as reported in the Graphics window. Note that the deformation is magnified in the plot so as to be visible.

The deformation would be better visible if the foreground and background were not of the same color. Turn off the background:

Utility Menu > PlotCtrls > Style > Background > Display Picture Background

To get the background back, you just have to select this again.

Animate the deformation:

Utility Menu > PlotCtrls > Animate > Deformed Shape...

Select Def + undeformed and click OK. Select Forward Only in the Animation Controller.

The left and bottom edges move parallel to themselves which means that the full deformed plate is also symmetric about these edges. This shows that the symmetry boundary condition at these edges is imposed correctly. The circular edge of the hole moves outward which is what one would expect from the outward pressure acting along it. Thus, the deformation of the structure agrees with the applied boundary conditions and matches with what one would expect from intuition.

Close the Animation Controller.

Plot Nodal Solution of von Mises Stress

To display the von Mises stress distribution as continuous contours, select

Main Menu > General Postproc > Plot results > Contour Plot > Nodal Solu

Select Nodal Solution > Stress > von Mises stress and click OK.

(Click picture for larger image)

The contour plot will show you the locations of the maximum and minimum values with the labels MX and MN, respectively. Are these locations where you expect them? SMX and SMN values reported in the Graphics window are the corresponding maximum and minimum stress values.

The diagonal is an additional line of symmetry. How symmetric is your result about the diagonal?

Save this plot to a file:

Utility Menu > PlotCtrls > Hard Copy > To File

Select the file format you want and type in a filename of your choice under Save to: and click OK. Check that the file has been created in your working directory.

When you plot the "Nodal Solution", ANSYS obtains a continuous distribution as follows:
1. It determines the average at each node of the values of all elements connected to the node.
2. Within each element, it linearly interpolates the average nodal value obtained in the previous step.

Plot Element Solution of von Mises Stress

To obtain results without nodal averaging, select

Main Menu > General Postproc > Plot results > Contour Plot > Element Solu

Select Element Solution > Stress > von Mises stress and click OK. This displays the von Mises stress results as discontinuous element contours.

(Click picture for larger image)

Save this plot to a file: Utility Menu > PlotCtrls > Hard Copy > To File

Element solution contours are determined by linear interpolation within each element but no nodal averaging is performed. The discontinuity between contours of adjacent elements is an indication of the gradient across elements. The inter-element discontinuities in our solution are relatively small compared to the stress levels. This indicates that the mesh resolution is reasonably good.

Query Results

To determine the value of the first principal stress sigma1 at a selected location, select

Main Menu > General Postproc > Query Results > Subgrid Solu

This brings up the Query Subgrid Solution Data menu. Select Stress from the left list, 1st principal S1 from the right list and click OK.

This brings up the pick menu. You can click on any location in the geometry and ANSYS will print the sigma1pick menu. value at that location. Try querying the values at a few locations. Note that the coordinates of the picked location and the corresponding solution value are reported in the

Cancel the pick menu.

Step 9: Validate the results

It is very important that you take the time to check the validity of your solution. This section leads you through some of the steps you can take to validate your solution.

Simple Checks

Does the deformed shape look reasonable and agree with the applied boundary conditions? We checked this in step 8.

Do the reactions at the supports balance the applied forces for static equilibrium? To check this, select

Main Menu > General Postproc > List Results > Reaction Solu

Select All struc forc F for Item to be listed and click OK.

The total reaction force in the x-direction is -7000 N.

Applied force = (pressure) x (projected distance in x-direction of the line along which the constant pressure acts) = (p) (r) = 7000 N in positive x-direction.

So the reaction cancels out the applied force in the x-direction. Similarly, you can check that this is true in the y-direction also.

Refine Mesh

Let's repeat the calculations on a mesh with overall element size level under SmartSize set to 4 instead of 5 and compare the results on the two meshes. Delete the current mesh:

Main Menu > Preprocessor > Mesh Tool

Select Clear under Mesh: and Pick All in the pick menu. The mesh is deleted.

Set the overall element size level under SmartSize to 4 by dragging the slider to the left. Click on Mesh and Pick All.

In the Output window, check how many elements are contained in this mesh? Your new mesh should have 276 quadrilateral elements.

Obtain a new solution: Main Menu > Solution > Solve > Current LS

Plot nodal solution of the von Mises stress:

Main Menu > General Postproc > Plot results > Contour Plot > Nodal Solu

Select Nodal Solution > Stress > von Mises stress and click OK.

Compare this with the von Mises contours for the previous mesh:

The two results compare well with the finer mesh contours being smoother as expected. Compare the maximum stress and displacement values:

.	Coarser Mesh	Finer Mesh
DMX	0.232e-8m	0.234e-8m
SMX	3.64MPa	3.74MPa

The maximum displacement value changes by less than 1% and the maximum von Mises stress value by less than 3%. This indicates that the meshes used provide adequate resolution.

Exit ANSYS

Utility Menu > File > Exit

Select Save Everything and click OK.

Reference

Cook, R.D., Malkus, D.S., Plesha, M.E., and Witt, R.J., Concepts and Applications of Finite Element Analysis, Fourth Edition, John Wiley and Sons, Inc., 2002.

Problem Statement

We used a 4-node quad element (PLANE42) in the tutorial. ANSYS also offers a 8-node quad element (PLANE82). Re-solve the tutorial problem using the PLANE82 element. Compare plots of the nodal and element solution of the von Mises stress for the two cases. You may use either mesh for this problem (although the final results presented here are done using the coarser mesh).

Hints

Look at the steps and think about which ones you have to change.

When you remesh the object, notice the following changes:

The number of nodes has increased!

To see why, do:

Main Menu > PlotCtrls > Multi-plot Ctrls ...

Click OK. Then on the Multi-Plotting Window that comes up, deselect everything but Nodes and Elements.

Click OK.

In the Graphics Window, you will now see the nodes in between the lines. There are 8 points for each quadrilateral area instead of the four we had before!

Final Result

Here are the Nodal and Element Solutions you should have gotten:

Nodal Solution

(Click picture for larger image)

Element Solution

(Click picture for larger image)

2-D Static Truss

Problem Specification

Determine the force in each member of the following truss. Indicate if the member is in tension or compression. The cross-sectional area of each member is 0.01 m, the Young's modulus is 200x10⁹ N/m² and Poisson ratio is 0.3.

The solution in ANSYS for this and subsequent tutorials is divided into the nine steps listed above. Note that you'll need to follow these same nine steps for solving almost any problem in ANSYS or a comparable finite-element analysis package.

Step 1: Start-up & preliminary set-up

Take a few minutes to review the conventions used in the tutorials which are given on the main page.

Create a folder

Create a folder called ansys at a convenient location. We'll use this folder to store files created during the session.

Start ANSYS

Start > Programs > Lab Apps > ANSYS 10.0 > ANSYS Product Launcher
In the window that comes up, enter the location of the folder you just created as your Working directory by browsing to it. If you specify, say, C:\ansys as your working directory, all files generated during the ANSYS run will be stored in this directory.
Specify truss as your Initial jobname. The jobname is the prefix used for all files generated during the ANSYS run. For example, when you perform a save operation in ANSYS, it'll store your work in a file called truss.db in your working directory.
For this tutorial, we'll use the default values for the other fields. Click on Run. This brings up the ANSYS interface. To make the best use of screen real estate, move the windows around and resize them so that you approximate this screen arrangement. This way you can read instructions in the browser window and implement them in ANSYS.
You can resize the text in the browser window to your taste and comfort as follows:
In Internet Explorer: Menubar > View > Text Size, then choose the appropriate font size.

In Netscape: Menubar > View > Increase Font or Menubar > View > Decrease Font.
The ANSYS interface consists of the following:

• Utility Menu:
  
  Note that the jobname truss appears in parenthesis in the title bar of the Utility Menu.
  
• ANSYS Main Menu:
  
  We'll more or less work our way down the Main Menu as we go through the solution steps.
  
• ANSYS Graphics
  
  This is the window where the geometry, mesh, applied boundary conditions, and results such as stress values are displayed.
  
• ANSYS Toolbar:
  
  The Toolbar contains shortcuts to often used commands such as save and can be customized by the user for convenience.
  
• ANSYS 10.0 Output Window:
  
  This is the window to which output from ANSYS commands is written and which provides feedback on the actions taken by ANSYS as you navigate the menus. If, at some point, you are not sure you clicked the right button or entered a value correctly, this is where to look first to figure out what you just did.
  

Set Preferences

We'll more or less work our way down the Main Menu.
Main Menu > Preferences
In the Preferences for GUI Filtering dialog box, click on the box next to Structural so that a tick mark appears in the box.

The effect of selecting the structural preference is that only menu options applicable to structural mechanics are shown in the graphical user interface; options related to other disciplines such as thermal, fluid and electromagnetics are grayed out. This helps a little while navigating the vast menu options within ANSYS.
Click OK to close the Preferences dialog box.

Step 2: Specify element type and constants

Enter the Preprocessor module

Main Menu > Preprocessor
This is the module where you create the geometry, specify appropriate displacement constraints and loading, and mesh the geometry. We are more or less going to march down this menu to set up the problem. You will find yourself negotiating through a series of menus as you work off the Main Menu.

Specify Element Type

Main Menu > Preprocessor> Element Type > Add/Edit/Delete > Add...
Pick Structural Link in the left field and 2D spar 1 in the right field. Click OK to select this element.

Now you will see the following in the Element Types dialog box:


LINK1 appears as the only defined element type in the Element Types dialog box. To view the help pages for this element type, click on Help in the Element Types dialog box. This brings up the Help window. Click on Search in the left pane and type in LINK1. (If the left pane is hidden, click the Show button in the toolbar) The first search result is the help page for the LINK1 element. Note that this is a two-dimensional spar element that supports uniaxial tension and compression but not bending, so it is appropriate for modeling a truss structure. There are two degrees of freedom at each of its two nodes: translations in the nodal x and y directions. The "1" in the element name is the internal reference number for this element type in ANSYS' list of available element types.
Before proceeding, let's take a quick peek at the pictorial summary of the element types available in ANSYS. Click on Release 10.0 Documentation for ANSYS > Element Reference > Element Characteristics > Pictorial Summary in the left part of the Help window. Our own humble LINK1 element is listed at the top of the pictorial summary. Clicking on the LINK1 box will take you to the help page for the element that we just visited. In general, you need to take the time to understand the element types and pick the appropriate one(s) for your problem. The pictorial summary is a good place to start for identifying the appropriate element for your problem. Your choice of element type has a significant effect on the speed and accuracy of the solution.
Minimize the Help window.
Close the Element Types window by clicking Close.

Specify Element Constants

Main Menu > Preprocessor > Real Constants > Add/ Edit/ Delete
This opens up the Real Constants dialog box. Click Add.... This brings up the Element Type for Real Constants dialog box with a list of the element types defined in the previous step. We have only one element type, LINK1, defined and it's automatically selected. Click OK.
We now enter the constants needed for the LINK1 element. For AREA, enter 0.01 which is the cross-sectional area of the element. We'll work in SI units. Leave the Initial strain field blank since it's not applicable to our problem.

It is the responsibility of the ANSYS user to make sure that the values entered are in consistent units. Click OK.
We see in the Real Constants menu that the constant set that we just created is "Set 1". So, when we mesh the geometry later on, we'll use the reference no. 1 to assign this constant set.

Click Close in the Real Constants dialog box.

Step 3: Specify material properties

Main Menu > Preprocessor > Material Props > Material Models
In the Material Models Available Frame of the Define Material Model Behavior window, double-click on Structural, Linear, Elastic, and Isotropic.

Enter 200e9 for Young's Modulus EX.
Enter 0.3 for Poisson's Ratio PRXY.

Click OK. This completes the specification of Material Model Number 1. When we mesh the geometry later on, we'll use the reference no. 1 to assign this material model. Close the Define Material Model Behavior menu.

Save your work

Utility Menu > File > Save as Jobname. db
This saves all the relevant data into one file called truss. db in your working directory, truss being taken from the jobname and db being an abbreviation for database. Verify that ANSYS has created this "database file" in your working directory. You can restart from your last save at any time using Utility Menu > File > Resume Jobname. db or ANSYS Toolbar > RESUM_DB. Each time you successfully finish a series of steps, you should save your work. Unfortunately, ANSYS doesn't have an undo button (though that is the first thing I needed while learning ANSYS!) and one way to recover from mistakes is to resume from your last save.

Step 4: Specify geometry

Overview

Since we are using the 2D Spar element, we can represent each truss member by a line. A line can be created by joining two keypoints (ANSYS terminology for vertices). So we'll need three keypoints, located at A, B and C in the figure below. We'll locate the origin of the coordinate system at C and number the keypoints at A, B and C as 1, 2 and 3, respectively.

Create Keypoints

Main Menu > Preprocessor > Modeling > Create > Keypoints > In Active CS
The active CS (i.e. Coordinate System) is the global Cartesian system by default and we'll work only in this coordinate system in our friendly introduction. ANSYS offers the capability to switch between various types of coordinate systems which will be necessary when you move on to solving super-duper problems.
In the Create Keypoints in Active Coordinate System dialog box,
Enter 1 for Keypoint number
Enter 0 for X and 2.8 for Y
(The Z value defaults to zero)
Click Apply (which accepts the input and then brings back the dialog box for further input)

Note that you can move to the next field using the Tab key.
Enter 2 for Keypoint number
Enter 1.5 for X and 2.0 for Y
Click Apply
Enter 3 for Keypoint number
Enter 0 for X and 0 for Y
Click OK (which accepts the input and then closes the dialog box)
Note the difference between Apply and OK which holds throughout ANSYS.
The keypoints will now be displayed in the Graphics window along with a triad that indicates the origin of the coordinate system (coincident with keypoint 3 in our case) and the axes.

Check Keypoints

To check if the keypoints have been created correctly:
Utility Menu > List > Keypoints > Coordinates only
This brings up a window listing the coordinates and rotation angles for the keypoints. Verify that you have the following:

You can rotate the coordinate system associated with each keypoint and that is what the rotation angles THXY, THYZ and THZX refer to. In our case, we don't need to rotate the keypoint coordinate system and so the rotation angles are identically zero.
Close the window listing the keypoints.
Close the Keypoints and Create menus.
Modifying Keypoints (If Necessary)
If you are like me, you made a mistake while creating keypoints and cursed that there is no undo button. To correct your mistake(s), you can delete keypoints and re-create them. In case you need to delete a keypoint, do the following:
Main Menu > Preprocessor > Modeling >Delete > Keypoints

This brings up the so-called pick menu.

Click on the keypoint you want to delete. A square appears around that keypoint indicating that it is selected. (Repeat for other keypoints as necessary.)
Click OK in the pick menu.
You should see the keypoint disappear in the Graphics window. You can also check that the keypoint has been deleted using Utility Menu > List > Keypoints. You can then re-create the keypoint.

Save your work

Once you have successfully created the keypoints, save your work using
Toolbar > SAVE_DB
This is a short-cut for
Utility Menu > File > Save as Jobname. db

Create Lines from Keypoints

Main Menu > Preprocessor > Modeling > Create > Lines > Lines >In Active Coord
This will bring up the Lines in Active Coord pick menu.
To create the line between keypoints 1 and 3, click on keypoint 1 and then keypoint 3. Similarly, create lines between keypoints 1 & 2 and keypoints 2 & 3.

Close the Lines in Active Coord pick menu by clicking on Cancel.
Close the Lines and Create menus.

Check Lines

Take a look at the list of lines that have been created:
Utility Menu > List > Lines
Click OK to accept the default output format.
The first four columns in the list should be:

The order of the keypoints for a line doesn't matter i.e. line l1 could go from keypoint k1 to k2 or equivalently, k2 to k1.
Close the window listing lines.

Modifying Lines (If Necessary)

If a line doesn't look right, you can delete and re-create it. To delete a line:
Main Menu > Preprocessor > Modeling > Delete > Lines Only
This brings up the pick menu.
Click on the line you want to delete in the Graphics window. Click OK. This deletes the line.

Save your work

Once you have successfully created the lines, click on Toolbar > SAVE_DB to save the database.

Step 5: Mesh geometry

Each truss member can be represented as a 2D Spar element. We'll use the MeshTool to mesh the geometry with this element.
To bring up the MeshTool, select
Main Menu > Preprocessor > Meshing > MeshTool
The MeshTool is used to control and generate the mesh.

Set Meshing Parameters

We'll now specify the element type, real constant set and material property set to be used in the meshing. Since we have only one of each, we can assign them to the entire geometry using the Global option under Element Attributes.
Make sure Global is selected under Element Attributes and click on Set.

This brings up the Meshing Attributes menu. You will see that the correct element type, material number and real constant set are already selected since we have only one of each.

Click OK. ANSYS now knows what element type (and associated constants) and material type to use for the mesh.

Set Mesh Size

Since a LINK1 element is equivalent to a truss member, we will specify that we want only one element per line. This is a subtle point and also very unusual; in most problems, you want to subdivide your part into many elements.
In the MeshTool, under Size Controls and Lines , click Set.
In the pick menu that comes up, click Pick All (since we want the specification of mesh size to apply to all lines in the geometry). This brings up the Element Sizes on Picked Lines menu. Specify No. of element divisions to be 1. Click OK. ANSYS will now use 1 element to mesh each line.

Mesh Lines

In the MeshTool, make sure Lines is selected in the drop-down list next to Mesh. This means the geometry components to be meshed are lines (as opposed to areas or volumes, as we'll see later). Click on the Mesh
button.
This brings up the pick menu. Since we want to mesh all lines, click on Pick All. The lines have been meshed. This is reported in the Output Window (usually hiding behind the Graphics Window):
NUMBER OF LINES MESHED = 3
MAXIMUM NODE NUMBER = 3
MAXIMUM ELEMENT NUMBER = 3
Close the MeshTool.

View Element List

Utility Menu > List > Elements > Nodes + Attributes

This table says that Element 1 is of material type 1 and element type 1 and is attached to nodes 1 and 2 and so on. In this element list, the order of the two nodes for each element doesn't matter. For example, element 3 can be attached to nodes 2 and 3 or equivalently, nodes 3 and 2. Also, the order of element numbering is not important since it is for internal bookkeeping.
Close the window listing the elements.

View Node Location

In order to see where the nodes are located, you can look at the list of nodes.
Utility Menu > List > Nodes
In Sort NODE Listing menu, click OK to accept defaults.

My list of nodes looks like this:

From the node and element lists, one can conclude that in this case:
Node 1 is pin A
Node 2 is pin C
Node 3 is pin B
Element 1 is member AC
Element 2 is member AB
Element 3 is member BC
Your own node and element numbering might be different from this and you would have to account for this while interpreting results in the postprocessing step.
Close the window listing the nodes.

Save your work

Toolbar > SAVE_DB

Step 6: Specify boundary conditions

Next, we step up to the plate to define the boundary conditions, namely, the displacement constraints and loads. Note that in ANSYS terminology, the displacement constraints are also "loads". We can apply the loads either to the geometry model or to the finite-element model (that is to the elements and nodes directly). The advantage of the former is that one doesn't have to re-specify the constraints on changing the mesh. So we'll apply the constraints to the geometry i.e. to the keypoints.

You can see from the diagram that the pin at A is constrained in x and y directions; or equivalently, keypoint 1 is constrained such that its UX and UY displacements are zero. Similarly, keypoint 3 is constrained such that its UX displacement is zero.

Apply Displacement Constraints

Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Keypoints

This brings up the Apply U, ROT on KPs pick menu.

In the Graphics window, click on keypoint 1;
This will draw a small square around keypoint 1 to indicate that it's been picked.
In the pick menu, click Apply. The following menu shows up.

Since we want to constrain UX as well as UY to zero at keypoint 1, select both UX and UY from items in DOFs to be constrained list. Since the Displacement value is zero by default, leave that field empty. Click on Apply.
You will see triangle symbols appear in the Graphics window indicating that both UX and UY DOFs are constrained at keypoint 1.
Next we apply the displacement constraint at keypoint 3. In the Graphics window, click on keypoint 3. In the pick menu, click Apply. Select only UX from items in DOFs to be constrained list. Click OK.
You will see a triangle symbol appear indicating that only the UX DOF is constrained at keypoint 3.

Close the Displacement and Apply menus.

List Displacement Constraints

You can verify the displacement constraints on the model by listing them.
Utility Menu > List > Loads > DOF constraints > On All Keypoints
This brings up a window with the constraint information.


If you made a mistake in applying a constraint, you can delete and reapply it. You can delete a constraint using Main Menu > Preprocessor > Loads > Define Loads >Delete > Structural > Displacement > On Keypoints. Alternately, you can resume from your last save and continue from there.
Close the window listing the constraint information.
Save the database: Toolbar > SAVE_DB

Apply Loading

We have only one load to apply on the structure, namely, the 2800 N force in the negative y-direction at keypoint 2 (see figure 1).
Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural >Force/Moment > On Keypoints

This brings up the Apply F/M on KPs pick menu.
In the Graphics window, click on keypoint 2; then in the pick menu, click OK.
In the menu that appears, select FY for Direction of force/ mom.

Enter -2800 for Force/ moment value. Click OK.

The negative sign for the force indicates that it is in the negative y-direction. You'll see a vector indicating the applied force in the Graphics window.
Close the Force/ Moment, Apply, Loads and Preprocessor menus.
Save the database: Toolbar > SAVE_DB

Step 7: Solve!

Enter Solution Module

Main Menu > Solution > Solve > Current LS
This solves the current load step (LS) i. e. the current loading conditions. In our problem, there is only one load step; ANSYS allows for multiple load steps that can be solved sequentially without leaving the Solution module.

Review the Problem

Review the information in the /STAT Command window. This is a summary of the problem that ANSYS is about to solve.

Close this window.

Perform Solution

Click OK in Solve Current Load Step menu.

ANSYS performs the solution and a yellow window should pop up saying "Solution is done!". Congratulations! You just obtained your first ANSYS solution.
Close the yellow window.
In preparation for the postprocessing step to be undertaken next, exit the solution module by closing the Solution menu.
Verify that ANSYS has created a file called truss.rst in your working directory. This file contains the results of the (previous) solve. The rst extension in the filename stands for results from a structural analysis. The truss.dbjobname.db file and then read in the results from the jobname.rst file using file contains only steps 1-6. To resume your work subsequent to exiting ANSYS, you'll have to first resume from the
Main Menu > General Postproc > Read Results > First Set

Step 8: Postprocess the results

Postprocessing is the step where we look at and analyze the results obtained from the ANSYS solution.
Enter the General Postprocessing module:
Main Menu > General Postproc

Plot Deformed Shape

Main Menu > General Postproc > Plot Results > Deformed Shape
Select Def + undeformed and click OK.

This plots the deformed and undeformed shapes in the Graphics window.

The deformed shape is shown as a solid line and the undeformed shape as a dotted line. The maximum displacement DMX is 0.583E-05m as reported in the Graphics window. This is small but plausible. Note that the deformation is magnified in the plot so as to be easily visible.
To save the deformation plot in a file, use Utility Menu > PlotCtrls > Hard Copy > To File. Select the file format you want and type in a filename of your choice under Save to: and click OK. The file will be created in your working directory. You can print out this file as necessary.
Animate the deformation:
Utility Menu > PlotCtrls > Animate > Deformed Shape
Select Def + undeformed and click OK. Select Forward Only in the Animation Controller.
Node 1 (Pin A) doesn't move and node 2 (Pin C) moves only in the vertical direction. Node 3 (Pin B) moves more or less in the direction of the applied force. The deformation of the structure agrees with the applied boundary conditions and matches with what one would expect from intuition.

Turn On Node and Element Numbers

In order to interpret the results that ANSYS reports, it's useful to turn on the node and element numbers in the Graphics window.
Utility Menu > PlotCtrls > Numbering
The Plot Numbering Controls menu is used to control the numbering of the various entities in a finite-element model.
Turn on Node numbers. Under Elem/Attrib numbering, select Element numbers. Click OK.

The node and element numbers will now appear in the Graphics window.

List Forces in Truss Members: Method 1

Main Menu > General Postproc > List Results > Element Solution

From the list, under Element Solution, select All Available force items . Click OK.


This brings up a window listing the forces that the elements apply on each of their nodes:

These element forces reported by ANSYS are forces ON its environment BY the element, not the converse. For example, Element 2 (or member AB) applies a force of 1500 N in the x-direction and 800 N in the negative y-direction on node 1 (or pin A). This means that the total force in AB is . The resultant acts from A to B i.e. the member is pulling on pin A. So it must be in tension. Similarly, the force in Element 1 (AC) is 2000 N (tension) and in Element 3 (BC) is 2500 N (compression). Note that your node and element numbers might be different from the above since they depend on the order in which the lines were created.
Close the PRESOL Command window.

List Forces in Truss Members: Method 2

Bring up the help page for LINK1 element:
Utility Menu > Help > Help Topics
Under the Contents tab, select
Release 10.0 Documentation for ANSYS > Element Reference > Element Library > LINK1
In the LINK1 help page, scroll down to LINK1 Element Output Definitions. You'll see the item
MFORX: Member force in the element coordinate system X direction
The figure at the top of the LINK1 help page shows that the x-direction in the element coordinate system is along the line. So MFORX is basically the axial force in the element.
So how do we get the MFORX values for our three elements from ANSYS? ANSYS has a quirky way of doing this as we shall see. If you scroll down the help page further, you'll see the LINK1 Item and Sequence Numbers:
MFORX SMISC 1
The output data is broken down into item groups with SMISC being one of the groups. Each item within an item group has an identifying "sequence" number. So MFORX is the item with sequence number 1 in the SMISC group.
Minimize the help window. To list MFORX values:
Main Menu > General Postproc > List Results > Element Solution
Under Element Solution, select Miscellaneous Items > Summable data (SMISC,1). Since MFORX is sequence number 1 in the SMISC group, enter 1 next to Sequent number SMIS in the editable field. Click OK. Click OK in the List Element Solution window.

This brings up a window with the axial forces in the elements. Positive values indicate tension and negative values compression. Do these values match what we got in method 1?

You can also plot the items listed under Element Output Definitions using the sequence number.
In most cases, you plot stresses using Main menu > General Postproc > Plot Results > Contour Plot >Nodal Solu. But for line elements like LINK1, this doesn't work and you'll get zero values for the stresses. So you'll have to use the sequence numbers to make stress plots for line elements.

List Reaction Forces at Nodes

Main Menu > General Postproc > List Results > Reaction Solu
Select All struc forc F for Item to be listed and click OK.

This brings up a window with the reaction forces at the nodes.

The sum of the reaction forces balances the applied load as should be the case for static equilibrium.
Close the PRRSOL Command window.

Step 9: Validate the results

Do not assume that if you are able to obtain a solution from ANSYS, it is bound to be correct. It is very important that you take the time to check the validity of your solution. This section leads you through some of the steps you can take to validate your solution.

Simple Checks

• Does the deformed shape look reasonable and agree with the applied boundary conditions? We checked this in step 8.
  
• Do the reactions at the supports balance the applied forces for static equilibrium? We checked this also in step 8.
  

Refine Mesh

The results obtained from FEA analysis depend on the mesh. An important step in the analysis is to make sure that the mesh resolution is adequate for the desired level of accuracy. This is done by refining the mesh and comparing results obtained with different levels of mesh resolution.
In our truss example, however, a truss member has to be modeled as a single LINK1 element. If we use multiple LINK1 elements to model a single truss member, these elements can rotate freely with respect to each other since they are essentially linked through pin joints. This violates physical reality and is one of the few cases where we'll avoid refining the mesh since it leads to an incorrect result.

Compare with Theory

Results should be compared with appropriate theoretical results whenever possible. In most cases, one would use theory to obtain order-of-magnitude estimates rather than to make a head-to-head comparison since presumably FEA is being used because a theoretical solution is not available. In this case, however, one can easily determine the forces in the truss members using the method of joints from statics. I'd recommend that you take a few minutes during commercials on your favorite TV show to calculate the forces and compare them with your ANSYS results.

Exit ANSYS

Utility Menu > File > Exit

Select Save Everything and click OK.
This is just a quick introduction to ANSYS to give you a flavor of what a full-fledged engineering package looks like. If it felt unfriendly or cumbersome, you are not alone; I went through this myself (otherwise, congratulations! you are a genius). It takes some getting used to. Believe it or not, it gets a lot easier to use with time. You have a lot of years ahead of you to gain the experience necessary to harness the power of finite-element analysis. All the ANSYS features including the underlying theory are documented online and can be accessed using Utility Menu > Help. There are tutorials available in the documentation which are also useful.

Problem Set 1

Resume the ANSYS Tutorial and make modifications to it as discussed below. To resume the ANSYS tutorial:
Start ANSYS; Specify the same directory but use a different jobname. Once ANSYS comes up, in the Utility Menu, click on:
Utility Menu > File > Resume from
Choose truss.db and click OK.
Consider the case where the displacement constrains at A and C are interchanged i.e.

• at A, only UX is set to zero
  
• at C, both UX and UY are set to zero
  

1. How would you expect the reaction forces at the supports A and C to change?
2. What can you say about how the x-component of the forces in the truss will change?
Re-solve the truss problem with the modified constraints. You can delete constraints using:
Main Menu > Preprocessor > Loads > Define Loads > Delete
It works similar to how you apply loads.
Tip: You can plot the displacement constraints in the Graphics window as follows:
Utility Menu > Pltctrls > Symbols
Select All Applied BCs for Boundary condition symbol. Click OK.
You might have to use :
Utility Menu > Plot > Replot
or
Utility Menu > Plot > Multi-plots
for the constraint symbols to appear in your plot.
Determine the following results from your ANSYS solution:
1. List the reactions. Note that you can save the reaction listing as follows: in the window that comes up with the listing of the reaction forces, click on:
File > Save As
2. List the element forces. From this determine the force in each member and whether the member is in tension or compression.

Problem Set 2

Determine the force in each member of the following truss using ANSYS. Indicate if the member is in tension or compression. Use the same LINK1 element as in the tutorial. The cross-sectional area of each member is 0.02 m², Young's modulus is 200x10⁹ N/m² and Poisson's ratio is 0.3. Verify your results by calculating the forces manually.

Results

Determine the following:
1. Listing of the reactions from the ANSYS solution.
2. Listing of the element forces from the ANSYS solution. Calculate and determine the forces in each member and whether the member is in tension or compression from this ANSYS result.
3. Using your pencil-and-paper calculations verifying the ANSYS results for the member and reaction forces.