This tutorial was created using ANSYS 7.0 to solve a simple 3D space frame problem.
The problem to be solved in this example is the analysis of a bicycle frame. 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.
The first step is to simplify the problem. Whenever you are trying out a new analysis type, you need something (ie analytical solution or experimental data) to compare the results to. This way you can be sure that you've gotten the correct analysis type, units, scale factors, etc.
The simplified version that will be used for this problem is that of a cantilever beam shown in the following figure:
1. Give the Simplified Version a Title (such as 'Verification Model').
Utility Menu > File > Change Title
For this simple example, these keypoints are the ends of the beam.
o We are going to define 2 keypoints for the simplified structure as given in the following table
keypoint
coordinate
x
y
z
1
0
2
500
o From the 'ANSYS Main Menu' select:Preprocessor > Modeling > Create > Keypoints > In Active CS
The two keypoints must now be connected to form a bar using a straight line.
o Select: Preprocessor > Modeling> Create > Lines > Lines > Straight Line.
o Pick keypoint #1 (i.e. click on it). It will now be marked by a small yellow box.
o Now pick keypoint #2. A permanent line will appear.
o When you're done, click on 'OK' in the 'Create Straight Line' window.
It is now necessary to create elements on this line.
o From the Preprocessor Menu, select: Element Type > Add/Edit/Delete.
o Click on the 'Add...' button. The following window will appear:
o For this example, we will use the 3D elastic straight pipe element as selected in the above figure. Select the element shown and click 'OK'. You should see 'Type 1 PIPE16' in the 'Element Types' window.
o Click on the 'Options...' button in the 'Element Types' dialog box. The following window will appear:
o Click and hold the K6 button (second from the bottom), and select 'Include Output' and click 'OK'. This gives us extra force and moment output.
o Click on 'Close' in the 'Element Types' dialog box and close the 'Element Type' menu.
We now need to specify geometric properties for our elements:
o In the Preprocessor menu, select Real Constants > Add/Edit/Delete
o Click Add... and select 'Type 1 PIPE16' (actually it is already selected). Click on 'OK'.
o Enter the following geometric properties:
o Outside diameter OD: 25
o Wall thickness TKWALL: 2
This defines an outside pipe diameter of 25mm and a wall thickness of 2mm.
o Click on 'OK'.
o 'Set 1' now appears in the dialog box. Click on 'Close' in the 'Real Constants' window.
You then need to specify material properties:
o In the 'Preprocessor' menu select Material Props > Material Models...
o Double click Structural > Linear > Elastic and select 'Isotropic' (double click on it)
o Close the 'Define Material Model Behavior' Window.
We are going to give the properties of Aluminum. Enter the following field:
EX 70000
PRXY 0.33
o Set these properties and click on 'OK'.
o In the Preprocessor menu select Meshing > Size Cntrls > ManualSize > Lines > All Lines
o In the size 'SIZE' field, enter the desired element length. For this example we want an element length of 2cm, therefore, enter '20' (i.e 20mm) and then click 'OK'. Note that we have not yet meshed the geometry, we have simply defined the element sizes.
(Alternatively, we could enter the number of divisions we want in the line. For an element length of 2cm, we would enter 25 [ie 25 divisions]).
8. NOTEIt is not necessary to mesh beam elements to obtain the correct solution. However, meshing is done in this case so that we can obtain results (ie stress, displacement) at intermediate positions on the beam.
Now the frame can be meshed.
o In the 'Preprocessor' menu select Meshing > Mesh > Lines and click 'Pick All' in the 'Mesh Lines' Window
Utility Menu > File > Save as.... Select the name and location where you want to save your file.
o From the Solution Menu, select 'Analysis Type > New Analysis'.
o Ensure that 'Static' is selected and click 'OK'.
o In the Solution menu, select Define Loads > Apply > Structural > Displacement > On Keypoints
o Select the left end of the rod (Keypoint 1) by clicking on it in the Graphics Window and click on 'OK' in the 'Apply U,ROT on KPs' window.
o This location is fixed which means that all translational and rotational degrees of freedom (DOFs) are constrained. Therefore, select 'All DOF' by clicking on it and enter '0' in the Value field and click 'OK'.
As shown in the diagram, there is a vertically downward load of 100N at the end of the bar
o In the Structural menu, select Force/Moment > on Keypoints.
o Select the second Keypoint (right end of bar) and click 'OK' in the 'Apply F/M' window.
o Click on the 'Direction of force/mom' at the top and select FY.
o Enter a value of -100 in the 'Force/moment value' box and click 'OK'.
o The force will appear in the graphics window as a red arrow.
The applied loads and constraints should now appear as shown below.
We now tell ANSYS to find the solution:
o Solution > Solve > Current LS
Now, since the purpose of this exercise was to verify the results - we need to calculate what we should find.
Deflection:
The maximum deflection occurs at the end of the rod and was found to be 6.2mm as shown above.
Stress:
The maximum stress occurs at the base of the rod and was found to be 64.9MPa as shown above (pure bending stress).
Deformation
o from the Main Menu select General Postproc from the 'ANSYS Main Menu'. In this menu you will find a variety of options, the two which we will deal with now are 'Plot Results' and 'List Results'
o Select Plot Results > Deformed Shape.
o Select 'Def + undef edge' and click 'OK' to view both the deformed and the undeformed object.
o Observe the value of the maximum deflection in the upper left hand corner (shown here surrounded by a blue border for emphasis). This is identical to that obtained via hand calculations.
Deflection
For a more detailed version of the deflection of the beam,
o From the 'General Postproc' menu select Plot results > Contour Plot > Nodal Solution.
o Select 'DOF solution' and 'USUM'. Leave the other selections as the default values. Click 'OK'.
o You may want to have a more useful scale, which can be accomplished by going to the Utility Menu and selecting Plot Controls > Style > Contours > Uniform Contours
o The deflection can also be obtained as a list as shown below. General Postproc > List Results > Nodal Solution ... select 'DOF Solution' and 'ALL DOFs' from the lists in the 'List Nodal Solution' window and click 'OK'. 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'.
o Are these results what you expected? Again, the maximum deflection occurs at node 2, the right end of the rod. Also note that all the rotational and translational degrees of freedom were constrained to zero at node 1.
o 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'.
Stresses
For line elements (ie beams, spars, and pipes) you will need to use the Element Table to gain access to derived data (ie stresses, strains).
o From the General Postprocessor menu select Element Table > Define Table...
o Click on 'Add...'
o As shown above, in the 'Item,Comp' boxes in the above window, select 'Stress' and 'von Mises SEQV'
o Click on 'OK' and close the 'Element Table Data' window.
o Plot the Stresses by selecting Plot Elem Table in the Element Table Menu
o The following window will appear. Ensure that 'SEQV' is selected and click 'OK'
o If you changed the contour intervals for the Displacement plot to "User Specified" you may need to switch this back to "Auto calculated" to obtain new values for VMIN/VMAX.
Utility Menu > PlotCtrls > Style > Contours > Uniform Contours ...
Again, select more appropriate intervals for the contour plot
o List the Stresses
§ From the 'Element Table' menu, select 'List Elem Table'
§ From the 'List Element Table Data' window which appears ensure 'SEQV' is highlighted
§ Click 'OK'
...
jarhal