This tutorial was created using ANSYS 5.7.1. This tutorial will introduce:
A 1000N vertical load will be applied to a catapult as shown in the figure below. The catapult is built from steel tubing with an outer diameter of 40 mm, a wall thickness of 10, and a modulus of elasticity of 200GPa. The springs have a stiffness of 5 N/mm.
For this problem, 3 types of elements are used: PIPE16, COMBIN7 (Revolute Joint), COMBIN14 (Spring-Damper) . It is therefore required that the types of elements are defined prior to creating the elements. This element has 6 degrees of freedom (translation along the X, Y and Z axis, and rotation about the X,Y and Z axis).
In the 'Element Types' window, there should now be three types of elements defined.
Real Constants must be defined for each of the 3 element types.
'Set 1' will now appear in the dialog box
Five of the degrees of freedom (UX, UY, UZ, ROTX, and ROTY) can be constrained with different levels of flexibility. These can be defined by the 3 real constants: K1 (UX, UY), K2 (UZ) and K3 (ROTX, ROTY). For this example, we will use high values for K1 through K3 since we only expect the model to rotate about the Z axis.
Note: The constants that we define in this problem refer to the relationship between the coincident nodes. By having high values for the stiffness in the X-Y plane and along the Z axis, we are essentially constraining the two coincident nodes to each other.
In the 'Element Types' window, there should now be three types of elements defined.
We are going to define 13 Nodes for this structure as given in the following table (as depicted by the circled numbers in the figure above):
| Node | Coordinates (x,y,z) |
|---|---|
| 1 | (0,0,0) |
| 2 | (0,0,1000) |
| 3 | (1000,0,1000) |
| 4 | (1000,0,0) |
| 5 | (0,1000,1000) |
| 6 | (0,1000,0) |
| 7 | (700,700,500) |
| 8 | (400,400,500) |
| 9 | (0,0,0) |
| 10 | (0,0,1000) |
| 11 | (0,0,500) |
| 12 | (0,0,1500) |
| 13 | (0,0,-500) |
The following window will appear. Ensure that the 'Element type number' is set to 1 PIPE16, 'Material number' is set to 1, and 'Real constant set number' is set to 1. Then click 'OK'.
Create the following elements joining Nodes 'a' and Nodes 'b'.
Note: because it is difficult to graphically select the nodes you may wish to use the command line (for example, the first entry would be: E,1,6).
| Node a | Node b |
|---|---|
| 1 | 6 |
| 2 | 5 |
| 1 | 4 |
| 2 | 3 |
| 3 | 4 |
| 10 | 8 |
| 9 | 8 |
| 7 | 8 |
| 12 | 5 |
| 13 | 6 |
| 12 | 13 |
| 5 | 3 |
| 6 | 4 |
You should obtain the following geometry (Oblique view)
When defining a joint, three nodes are required.
Two nodes are coincident at the point of rotation.
The elements that connect to the joint must reference each of the coincident points.
The other node for the joint defines the axis of rotation.
The axis would be the line from the coincident nodes to the other node.
Create the following lines joining Node 'a' and Node 'b'
| Node a | Node b | Node c |
|---|---|---|
| 1 | 9 | 11 |
| 2 | 10 | 11 |
Create the following lines joining Node 'a' and Node 'b'
| Node a | Node b |
|---|---|
| 5 | 8 |
| 8 | 6 |
NOTE: To ensure that the correct nodes were used to make the correct element in the above table, you can list all the elements defined in the model. To do this, select Utilities Menu > List > Elements > Nodes + Attributes.
Because we have defined our model using nodes and elements, we do not need to mesh our model. If we initially defined our model using keypoints and lines, we would have had to create elements in our model by meshing the lines. It is the elements that ANSYS uses to solve the model.
You may also wish to turn on element numbering and turn off keypoint numbering
Because the model is expected to deform considerably, we need to include the effects of large deformation.
The applied loads and constraints should now appear as shown in the figure below.
Note: To have the constraints and loads appear each time you select 'Replot' in ANSYS, you must change some settings under Utility Menu > Plot Ctrls > Symbols.... In the window that appears check the box beside 'All Applied BC's' in the 'Boundary Condition Symbol' section.
Note: During the solution, you will see a yellow warning window which states that the "Coefficient ratio exceeds 1.0e8". This warning indicates that the solution has relatively large displacements. This is due to the rotation about the joints.
In this problem, we would like to find the vertical displacement of node #7. We will do this using the GET command.
Therefore the vertical displacement of Node 7 is 323.78 mm. This can be repeated for any of the other nodes you are interested in.
