| | Verification Example | | Preprocessing | | Solution | | Postprocessing | | Command Line | |
| | Bicycle Example | | Preprocessing | | Solution | | Postprocessing | | Command Line | |
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:
Utility Menu > File > Change Title
For this simple example, these keypoints are the ends of the beam.
| keypoint | coordinate | ||
|---|---|---|---|
| x | y | z | |
| 1 | 0 | 0 | 0 |
| 2 | 500 | 0 | 0 |
The two keypoints must now be connected to form a bar using a straight line.
It is now necessary to create elements on this line.
We now need to specify geometric properties for our elements:
Outside diameter OD: 25
Wall thickness TKWALL: 2
This defines an outside pipe diameter of 25mm and a wall thickness of 2mm.
You then need to specify material properties:
We are going to give the properties of Aluminum. Enter the following field:
| EX 70000 | |
| PRXY 0.33 |
(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]).
NOTE
It 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.
Utility Menu > File > Save as.... Select the name and location where you want to save your file.
As shown in the diagram, there is a vertically downward load of 100N at the end of the bar
The applied loads and constraints should now appear as shown below.
![[Loads & Constraints]](./images/SimpleLoads.gif)
We now tell ANSYS to find the solution:
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
Deflection
For a more detailed version of the deflection of the beam,
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).
Again, select more appropriate intervals for the contour plot
Note that a maximum stress of 64.914 MPa occurs at the fixed end of the beam as predicted analytically.
Bending Moment Diagrams
To further verify the simplified model, a bending moment diagram can be created. First, let's look at how ANSYS defines each element. Pipe 16 has 2 nodes; I and J, as shown in the following image.
To obtain the bending moment for this element, the Element Table must be used. The Element Table contains most of the data for the element including the bending moment data for each element at Node I and Node J. First, we need to obtain obtain the bending moment data.
This will save all of the bending moment data at the left hand side (I side) of each element. Now we need to find the bending moment data at the right hand side (J side) of each element.
Now, you can double check these solutions analytically. Note that the line between the I and J point is a linear interpolation.
Table 1. PIPE16 Item, Sequence Numbers, and Definitions for the ETABLE Commands
| node I | |||
|---|---|---|---|
| name | item | e | Definition |
| MFORX | SMISC | 1 | Member forces at the node |
| MFORY | SMISC | 2 | |
| MFORZ | SMISC | 3 | |
| MMOMX | SMISC | 4 | Member moments at the node |
| MMOMY | SMISC | 5 | |
| MMOMZ | SMISC | 6 | |
Note that SMISC 6 (which we used to obtain the values at node I) correspond to MMOMZ - the Member moment for node I. The value of 'e' varies with different Element Types, therefore you must check the ANSYS Documentation files for each element to determine the appropriate SMISC corresponding to the plot you wish to generate.
Copy the following code into the command line, then hit enter. Note that the text following the "!" are comments.
/PREP7 ! Preprocessor K,1,0,0,0, ! Keypoint, 1, x, y, z K,2,500,0,0, ! Keypoint, 2, x, y, z L,1,2 ! Line from keypoint 1 to 2 !* ET,1,PIPE16 ! Element Type = pipe 16 KEYOPT,1,6,1 ! This is the changed option to give the extra force and moment output !* R,1,25,2, ! Real Constant, Material 1, Outside Diameter, Wall thickness !* MP,EX,1,70000 ! Material Properties, Young's Modulus, Material 1, 70000 MPa MP,PRXY,1,0.33 ! Material Properties, Major Poisson's Ratio, Material 1, 0.33 !* LESIZE,ALL,20 ! Element sizes, all of the lines, 20 mm LMESH,1 ! Mesh the lines FINISH ! Exit preprocessor /SOLU ! Solution ANTYPE,0 ! The type of analysis (static) !* DK,1, ,0, ,0,ALL ! Apply a Displacement to Keypoint 1 to all DOF FK,2,FY,-100 ! Apply a Force to Keypoint 2 of -100 N in the y direction /STATUS,SOLU SOLVE ! Solve the problem FINISH
Note that you have now finished Postprocessing and the Solution Phase with just these few lines of code. There are codes to complete the Postprocessing but we will review these later.
Now we will return to the analysis of the bike frame. The steps which you completed in the verification example will not be explained in great detail, therefore use the verification example as a reference as required. We will be combining the use of the Graphic User Interface (GUI) with the use of command lines.
Recall the geometry and dimensions of the bicycle frame:
We are going to define the vertices of the frame using variables. These variables represent the various lengths of the bicycle members. 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 which was used above to input the command line codes for the verification model. Type in each of the following lines followed by Enter.
x1 = 500
x2 = 825
y1 = 325
y2 = 400
z1 = 50
For this space frame example, these keypoints are the frame vertices.
| keypoint | coordinate | ||
|---|---|---|---|
| x | y | z | |
| 1 | 0 | y1 | 0 |
| 2 | 0 | y2 | 0 |
| 3 | x1 | y2 | 0 |
| 4 | x1 | 0 | 0 |
| 5 | x2 | 0 | z1 |
| 6 | x2 | 0 | -z1 |
K, NPT, X, Y, Zwhere, each Abbreviation is representative of the following:
Keypoint, Reference number for the keypoint, coords x/y/zFor a more detailed explanation, type help k into the command line
For example, to enter the first keypoint type:
K,1,0,y1,0into the command line followed by Enter.
As with any programming language, you may need to add comments. The exclamation mark indicates that anything following it is commented out. ie - for the second keypoint you might type:
K,2,0,y2,0 ! keypoint, #, x=0, y=y2, z=0
KDELE,#where # corresponds to the number of the keypoint.
In this example, we defined the keypoints by making use of previously defined variables like y1 = 325. This was simply used for convenience. To define keypoint #1, for example, we could have alternatively used the coordinates x = 0, y = 325, z = 0.
 |
|
We will be joining the following keypoints together:
|
Again, we will use the command line to create the lines. The command format to create a straight line looks like: L, P1, P2 Line, Keypoint at the beginning of the line, Keypoint at the end of line For example, to obtain the first line, I would write: ' L,1,2 ' Note: unlike 'Keypoints', 'Lines' will automatically assign themselves the next available reference number. | |||||||||||||||||||||||||||||
You should obtain the following:
As in the verification model, define the type of element (pipe16). As in the verification model, don't forget to change Option K6 'Include Output' to obtain extra force and moment output.
Now specify geometric properties for the elements
Outside diameter OD: 25 Wall thickness TKWALL: 2
To set Young's Modulus and Poisson's ratio, we will again use the command line. (ensure that the preprocessor menu is still open - if not open it by clicking Preprocessor in the Main Menu)
MP, LAB, MAT, C0 Material Property,Valid material property label, Material Reference Number, value
As in the verification model, set the element length to 20 mm
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines
Now the frame can be meshed.
Saving Your Job
Utility Menu > File > Save as...
Close the 'Preprocessor' menu and open up the 'Solution' menu (from the same 'ANSYS Main Menu').
Once again, we will use the command line. We are going to pin (translational DOFs will be fixed) the first keypoint and constrain the keypoints corresponding to the rear wheel attachment locations in both the y and z directions. The following is the command line format to apply constraints at keypoints.
DK, KPOI, Lab, VALUE, VALUE2, KEXPND, Lab2, Lab3, Lab4, Lab5, Lab6 Displacement on K, K #, DOF label, value, value2, Expansion key, other DOF labelsNot all of the fields are required for this example, therefore when entering the code certain fields will be empty. For example, to pin the first keypoint enter:
DK,1,UX,0,,,UY,UZ
The DOF labels for translation motion are: UX, UY, UZ. Note that the 5th and 6th fields are empty. These correspond to 'value2' and 'the Expansion key' which are not required for this constraint. Also note that all three of the translational DOFs were constrained to 0. The DOFs can only be contrained in 1 command line if the value is the same.
To apply the contraints to Keypoint 5, the command line code is:
DK,5,UY,0,,,UZ
Note that only UY and UZ are contrained to 0. UX is not constrained. Again, note that the 5th and 6th fields are empty because they are not required.
If you need to delete any of the constraints use the following command: 'DKDELE, K, Lab' (ie 'DKDELE,1,UZ' would delete the constraint in the 'z' direction for Keypoint 1)
We will apply vertical downward loads of 600N at the seat post location (keypoint 3) and 200N at the pedal crank location (keypoint 4). We will use the command line to define these loading conditions.
FK, KPOI, Lab, value, value2 Force loads at keypoints, K #, Force Label directions (FX, FY, FZ), value1, value2 (if req'd)
To apply a force of 600N downward at keypoint 3, the code should look like this: ' FK,3,FY,-600 '
Apply both the forces and list the forces to ensure they were inputted correctly (FKLIST).
If you need to delete one of the forces, the code looks like this: 'FKDELE, K, Lab' (ie 'FKDELE,3,FY' would delete the force in the 'y' direction for Keypoint 3)
The applied loads and constraints should now appear as shown below.
![[Bike Loads & Constraints]](./images/BikeLoads.gif)
To begin Postprocessing, open the 'General Postproc' Menu
![[Bike Deflection]](./images/BikeDeform.gif)
![[Bike Deflection - side view]](./images/BikeDeform2.gif)
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.
We could also take a look at the forces in the elements in much the same way:
As shown in the cantilever beam example, use the Element Table to gain access to derived stresses.
As shown previously, the bending moment diagram can be produced.
Select Element Table > Define Table... to define the table (remember SMISC,6 and SMISC,12)
And, Plot Results > Line Elem Res... to plot the data from the Element Table
