Introduction
This document is a tutorial on the use of ANSYS 5.2 to solve a simple 3D space frame problem. The problem to be solved in this example is the analysis of a bicycle frame.
Preprocessing: Defining the Problem
The problem to be modeled in this example is a simple bicycle frame shown in the following figure. The frame is to be built of hollow aluminum tubing having an outside diameter of 25mm and a wall thickness of 2mm.
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikesketch.jpg
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/important.gif Note that it is the responsibility of the user to ensure that a consistent set of units are used for the problem; thus making any conversions where necessary!
Begin by giving the example a title. In the 'Utility menu bar' select the 'File' menu and the 'Change Title' submenu. This title will appear in the 'Graphics Window' when plots are generated. Select 'OK' when done.
Defining Some Variables
We are going to define the vertices of the frame using variables. These variables represent the various lengths shown in the above figure. Notice that by using variables like this, it is very easy to set up a parametric description of your model. This will enable us to quickly redefine the frame should changes be necessary. The quickest way to enter these variables is via the 'ANSYS Input window'. Move your mouse to the lower half of the window and then left click. Then type in each of the following lines followed by an Enter or Return. All lengths are given in mm.
x1 = 500 x2 = 825 y1 = 325 y2 = 400 z1 = 50
Keypoints
The overall geometry is defined in ANSYS using keypoints which simply specify various principal coordinates to define the body. For this space frame example, these keypoints are the frame vertices.
Start the preprocessor by selecting 'Preprocessor' in the 'ANSYS Main Menu'.
From the 'Preprocessor' menu, select 'Create' (under the '-Modeling-' title).
Then select 'Keypoints' from this 'Create' menu.
Select 'In Active CS...' on the 'Keypoints' menu. This permits you to define keypoints in the active Coordinate System.
We are going to define 6 keypoints for this structure as given in the following table (these keypoints are depicted by the circled numbers in the above figure):
keypointcoordinatexyz10y1020y203x1y204x1005x20z16x 20-z1
We are going to define the first keypoint which has the coordinates x = 0, y = y1 and z = 0. In the window that appears, enter keypoint number 1 in the appropriate box, and enter the x,y,z coordinates: 0, y1, 0 in their appropriate boxes.
Click 'Apply' to accept what you have typed. You may now see a small point in the 'Graphics window' showing the location of this keypoint.
Enter the second keypoint by typing 2 and the coordinates 0, y2, 0 in the their appropriate boxes.
Click 'Apply' to accept this second keypoint.
Continue with the remaining keypoints as defined in the above table.
Note: When entering the final data point, click on 'OK' to indicate that you are finished entering keypoints. If you first press 'Apply' and then 'OK' for the final keypoint, you will have defined it twice!
If you did press 'Apply' for the final point, simply press 'Cancel' to close this dialog box.
In this example, we have defined the keypoints by making use of previously defined variables like y1 = 325. This was simply used for conveniance. To define keypoint #1, for example, we could have alternatively used the coordinates x = 0, y = 325, z = 0.
Correcting Mistakes
When defining keypoints, lines, areas, volumes, elements, constraints and loads you are bound to make mistakes. Fortunately these are easily corrected so that you don't need to begin from scratch every time an error is made! Every 'Create' menu for generating these various entities also has its complimentary 'Delete' menu for fixing things up. Their use is pretty much intuitive.
Plotting Keypoints
We would now like to see a better view of these keypoints.
To plot the keypoints, select 'Utility menu bar'/'Plot'/'Keypoints'.
To see the keypoint numbers, select 'Utility menu bar'/'PlotCtrls'/'Numbering...'
Click on the button beside 'Keypoint numbers' so that it changes colour, and says 'On' beside it. Click on 'OK' and the box will close and the keypoints will be plotted with their numbers.
To get a better view of our view of our model, we'll view it in an isometric view:
Select 'Utility menu bar'/'PlotCtrls'/'Pan, Zoom, Rotate...' In the window that appears, you have many controls. Try experimenting with them. By turning on the dynamic mode (click on the button beside 'Dynamic Mode' so that it turns yellow) you can use the mouse to drag the image, translating and rotating it on all three axes.
To get an isometric view, click on 'Iso' (at the top right). You can either leave the 'Pan, Zoom, Rotate' window open and move it to an empty area on the screen, or close it if your screen is already cluttered.
Forming Lines
We must now connect the various keypoints together by lines to form the frame. We will be joining the following keypoints together:
linekeypoint1st2nd112223334414535645736846
We will use the mouse to select the keypoints to form the lines.
First close the last menu that was used to create the keypoints by double clicking in the upper left-hand corner of the 'Keypoints menu'. This will return you to the 'Create menu'.
Select the 'Lines' item (under '-Lines-') in this menu.
Select 'Straight Line'.
Use the mouse to pick keypoint #1 (i.e. click on it). It will now be marked by a small yellow box.
Now move the mouse toward keypoint #2. A line will now show on the screen joining these two points.
Left click and a permanent line will appear.
Continue to form the other lines until you get a picture like that shown below.
Note that the order of joining the keypoints to form lines is not important.
When you're done, click on 'OK' in the 'Create Straight Line' window.
Now close the 'Lines' menu and the 'Create' menu as earlier described.
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikelines.jpg
Element Formation
It is now necessary to create elements on these lines. This is called 'meshing'. ANSYS first needs to know what kind of elements to use for our problem:
Select 'Element Type' in the 'Preprocessor' menu.
Select 'Add/Edit/Delete...'
Click on the 'Add...' button in the 'Element Types' window.
There are two types of elements that could be considered here:
3D beam element: This element is a uniaxial element with tension, compression, torsion and bending capabilities. It has six degrees of freedom at each node: 3 translations and 3 rotations. You may define its cross-sectional area as well as its moments of interia about two axes.
3D pipe element: This element is based on the 3D beam element so it too has same degrees of freedom at each node and the same calculational abilities. Where it differs is that it is specialized for symmetrical, circular pipe geometries. All we need specify are the pipe diameter and wall thickness.
For this example, we will use the simpler pipe element.
Under the 'Structural' section, in the middle of the dialog box, Select 'Pipe'.
Then in the next box to the right, select 'Elast straight16'. This specifies an elastic straight pipe element.
Finally click on 'OK' to close the dialog box. You should see 'Type 1 PIPE16' in the 'Element Types' window.
Click on the 'Options...' button.
In the 'PIPE16 element type options' window, click and hold the K6 button (second from the bottom), and select 'Include Output'. This gives us extra force and moment output.
Click on 'OK'.
Click on 'Close' in the 'Element Types' dialog box.
Close the 'Element Type' menu.
Element Geometric Properties
We now need to specify geometric properties for our elements:
Select 'Real Constants...' in the 'Preprocessor' menu.
Click on 'Add...'
Select 'Type 1 PIPE16' (actually it is already selected). Click on 'OK'.
In the 'Real Constants for PIPE16' window, enter the following geometric properties:
Outside diameter OD: 25 Wall thickness TKWALL: 2
This defines an ouside pipe diameter of 25mm and a wall thickness of 2mm.
Click on 'OK'.
'Set 1' now appears in the dialog box. Click on 'Close' in the 'Real Constants' window.
Element Material Properties
You then need to specify material properties:
Select 'Material Props' in the 'Preprocessor' menu.
Select 'Isotropic...' under '-Constant-'
Click 'OK' in the 'Isotropic Material Properties' window to select material number 1.
In the window that appears, there are many properties that may be specified. We are going to give the properties of Aluminum. Change the following fields:
Young's modulus EX: 70000 Poison's ratio NUXY: 0.33 Shear modulus GXY: 26000
Set these properties and click on 'OK'.
Close the 'Material Props' menu.
Mesh Size
The last step before meshing is to tell ANSYS how big the elements should be.
Select 'Shape & Size' under '-Meshing-' in the 'Preprocessor' menu.
In the 'Shape & Size' menu, select 'Global Elem Size...'
In the size 'SIZE' field, we could now enter the desired element lengths. For example if we wanted an element length of 2cm, we could enter '20' (i.e 20mm) and then click on 'OK'.
For this example however, we'll let ANSYS determine the element size automatically. So simply 'Cancel' out of this dialog box.
Close the 'Shape & Size' menu.
Meshing
Now you can tell ANSYS to mesh the frame:
Select 'Mesh' under '-Meshing-' in the 'Preprocessor' menu.
Select 'Lines' in the 'Mesh' menu.
Use the mouse to pick all the lines in the graphics window. Each line will be surrounded by a yellow box when picked.
Click on 'OK' in the 'Mesh Lines' Box.
Close the 'Mesh' menu.
Plotting Elements
Plot your elements by:
Select 'Numbering' in the 'PlotCtrls' Menu.
Turn off Keypoint numbering so that the plot does not become confusing.
Click on the 'Elem & Attrib numbering' box, and select 'Element numbers'.
Click on 'OK'.
From the 'Plot' menu, select 'Elements' and you will then see the elements plotted in multiple colours, with their element numbers.
Saving Your Job
Save the model at this time, so if you make some mistakes later on, you will at least be able to come back to this point. To do this, select 'Utility Menu Bar'/'File'/'Save As Jobname.db'. Your model will be saved in a file called 'jobname.db', where 'jobname' is the name that you specified in the 'Launcher' when you first started ANSYS.
It is a good idea to save your job at different times throughout the building and analysis of the model to backup your work incase of a system crash or what have you.
Solution Phase: Assigning Loads and Solving
You have now defined your model. It is now time to apply the load(s) and constraint(s) and solve the the resulting system of equations.
Close the 'Preprocessor' menu and open up the 'Solution' menu (from the same 'ANSYS Main Menu'). Analysis Type
First you must tell ANSYS how you want it to solve this problem:
Select 'New Analysis'.
Ensure that 'Static' is selected; i.e. you are going to do a static analysis on the frame as apposed to a dynamic analysis, for example.
Click 'OK'.
Now you must apply some loads and constraints:
Constraints
It is necessary to apply constraints to the model otherwise the model is not tied down or grounded and a singular solution will result. In mechanical structures, these constraints will typically be fixed, pinned and roller-type connections.
Select 'Apply >' under '-Loads-' title.
We will start with constraints, so select 'Displacement >' under the '-Structural-' title.
Select 'On Keypoints' for this example. As you recall, these keypoints were defined at the vertices of the frame.
Use the mouse to pick the first keypoint defined (just above the x,y,z triad)
Click on 'Apply' in the 'Apply U,ROT' window.
Now we select what degrees of freedom are to be constrained. In this example, we will pin this location which means that all translational DOF's are constrained.
Select 'UX', 'UY' and 'UZ' by clicking on them.
Enter '0' in the Value field and click on 'OK'.
You will see some blue triangles in the graphics window indicating the displacement contraints.
Note that if you had wanted to completely fix this point you would have selected to constrain 'ALL DOF' in this dialog box for this point.
We want to apply two more constraints at the rear wheel attachment locations...
So once again select 'On Keypoints'.
Now pick both of the wheel attachment locations. These should be indicated by yellow boxes.
Select 'OK'
Now we select what degrees of freedom are to be constrained at these two keypoints In this case, we will fix the UY and UZ degrees of freedom to simulate the wheel attachment:
Turn off the 'UX' box by clicking on it.
Ensure that the 'UY' and 'UZ' boxes are still highlighted.
Make sure that the value field is still set to '0'.
Select 'OK'
Note the blue triangles at these points indicating their fixed directions.
Close the 'Displacement' menu.
Loading
It's time to apply some loads. We will apply a vertically downward load of 600N at the seat post location and a load of 200N at the pedal crank location.
If you still have the 'Apply' menu open, select 'Force/Moment >'. (If you don't have 'Apply' open, its under '-Loads-' in the 'Solution' menu.)
Choose 'On Keypoints'
Pick the vertex at the seat post location.
Click on 'Apply' in the 'Apply F/M' window.
In the next dialog box to appear:
Click on the button at the top and select FY. This indicate that we will be applying the load in the 'y' direction
Enter a value of -600 in the box below.
Click on 'OK'. The force will appear in the graphics window as a red arrow.
Once again select 'On Keypoints'.
Select the pedal crank position.
Press 'OK' and enter a force of -200 in the ensuing dialog box.
Click on 'OK'. The second force will appear below the crank location.
Close the 'Force/Moment' menu and the 'Apply' menu.
The applied loads and constraints should now appear as shown below.
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikeloads.jpg
Solving the System
We now tell ANSYS to find the solution:
In the 'Solution' menu under the '-Solve-' title, select 'Current LS' This indicates that we desire the solution under the current Load Step (LS).
Click on 'OK' in the window that comes up after a few seconds. You may close the solution 'STAT window' that has appeared from the solution phase.
Close the 'Solution' menu.
<A name=postprocessing>
Postprocessing: Viewing the Results
You will now want to view the results. To do this you must enter the post-processor and select the desired solution:
Select 'General Postproc' from the 'ANSYS Main Menu'.
Read the results by selecting 'Last Set' under '-Read Results-'.
Deformed Shape
Let's plot the deformed shape of this loading:
Select 'Plot Results' in the 'General Postprocessor' menu.
Select 'Deformed Shape...'
Select what you want to plot (e.g. 'Def+ undeformed') and click on 'OK'.
Your should see a plot like the figure below...
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikedefliso.jpg
You may want to try plotting this from differenct angles to get a better idea what's going on by using the 'Pan-Zoom-Rotate' menu that was earlier outlined.
Try the 'Front' view button (Note that the views of 'Front', 'Left', 'Back', etc depend on how the object was first defined).
Your screen might look like the plot below...
Close the 'Plot Results' menu when you are done.
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikedeflside.jpg
Deflections
Now let's take a look at some actual deflections in the frame. The deflections have been calculated at the nodes of the model, so the first thing we'll do is plot out the nodes and node numbers, so we know what node(s) we're after.
Go to 'Utility menu bar'/'PlotCtrls'/'Numbering...' and turn on 'Node numbers'. Turn everything else off.
Now plot the nodes by 'Utility menu bar'/'Plot'/'Nodes'. Note the node numbers of interest. Of particular interest are those nodes where the constraints were applied to see if their displacements/rotations were indeed fixed to zero. Also node the node numbers of the seat and crank locations.
Select 'Main Menu'/'General Postproc'/'List Results'
Select 'Nodal Solution...' from the 'General Postprocessor' menu.
You can now select what you want to see. To begin with, we will select 'DOF Solution' and 'ALL DOFs' from the lists in the 'List Nodal Solution' window. This means that we want to see a listing of all translational and rotational degrees of freedom from the solution. If we had only wanted to see the displacements for example, we would have chosen 'ALL Us' instead of 'ALL DOFs'.
Click on 'OK'. The nodal results are now displayed. Use the scroll bars to move through the results. Are the displacements and rotations as you expected?
If you wanted to save these results to a file, use the mouse to go to the 'File' menu (at the upper left-hand corner of this list window) and select 'Save as'.
Close this listing window when you're done by double clicking in the upper left-hand window corner or by selecting 'File'/'Close'.
Element Forces
We could now take a look at the forces in the elements in much the same way:
Select 'Element Solution...' from the 'List Results' menu.
Select 'Nodal force data' and 'All forces' from the lists displayed.
Click on 'OK'.
For each element in the model, the force/moment values at each of the two nodes per element will be displayed.
Close this list window when you are finished browsing.
Then close the 'List Results' menu.
Stresses
Now lets see some information about stresses in the frame:
Close the 'List Results' menu if it is still open.
Select 'Element Table' from the 'General Postprocessor' menu.
Select 'Define Table...'
Click on 'Add...'
In the user label box ('Lab'), type 'VonMis'
In the 'Item,Comp' boxes, select 'Stress' and 'von Mises'
Click on 'Apply'.
You may choose to label and select other stress componants as well.
When you are done, click on 'OK'.
Close the 'Element Table Data' window.
Let's get a plot of these stresses:
Close the 'Element Table' Menu.
Select 'Plot Results' from the 'General Postproc' menu.
Select 'Elem Table..'
If you defined more that one stress component in the element table, select it in the 'Item to be plotted' list.
Click on 'Apply' and observe the stress contour plot in the 'Graphics Window'. It should appear similar to the plot below:
When you've finished seeing what you want here, click on 'OK'.
Close any open menus that you don't require.
http://www.kkiem.agh.edu.pl/dydakt/fem/3DFrame_pliki/bikestress.jpg
Quitting ANSYS
To quit ANSYS, select 'QUIT' from the ANSYS Toolbar or select 'Utility Menu'/'File'/'Exit...'. In the dialog box that appears, click on 'Save Everything' (assuming that you want to) and then click on 'OK'.