![[Bracket Geometry]](./images/bracket1.gif)
| | Verification Example | | Preprocessing | | Solution | | Postprocessing | | Command Line | |
| | Bracket Example | | Preprocessing | | Solution | | Postprocessing | | Command Line | |
This tutorial is the second of three basic tutorials created to illustrate commom features in ANSYS. The plane stress bracket tutorial builds upon techniques covered in the first tutorial (3D Bicycle Space Frame), it is therefore essential that you have completed that tutorial prior to beginning this one.
The 2D Plane Stress Bracket will introduce boolean operations, plane stress, and uniform pressure loading.
The problem to be modeled in this example is a simple bracket shown in the following figure. This bracket is to be built from a 20 mm thick steel plate. A figure of the plate is shown below.
This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right.
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 flat rectangular plate with a hole shown in the following figure:
Boolean operations provide a means to create complicated solid models. These procedures make it easy to combine simple geometric entities to create more complex bodies. Subtraction will used to create this model, however, many other Boolean operations can be used in ANSYS.
Instead of creating the geometry using keypoints, we will create an area (using GUI)
(Alternatively, the command line code for the above command is BLC4,0,0,200,100)
(Alternatively, the command line code for the above command is CYL4,100,50,20 )
Now we want to subtract the circle from the rectangle. Prior to this operation, your image should resemble the following:
You should now have the following model:
(Alternatively, the command line code for the above step is ASBA,1,2)
It is now necessary to define the type of element to use for our problem:
Preprocessor Menu > Element Type > Add/Edit/Delete
PLANE82 is a higher order version of the two-dimensional, four-node element (PLANE42). PLANE82 is an eight noded quadrilateral element which is better suited to model curved boundaries.
For this example, we need a plane stress element with thickness, therefore
(Alternatively, the command line code for the above step is ET,1,PLANE82 followed by KEYOPT,1,3,3)
(Alternatively, the command line code for the above step is R,1,20)
We are going to give the properties of Steel. Enter the following when prompted:
| EX 200000 | |
| PRXY 0.3 |
(Alternatively, the command line code for the above step is MP,EX,1,200000 followed by MP,PRXY,1,0.3)
To tell ANSYS how big the elements should be, Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas
(Alternatively, the command line code for the above step is AESIZE,ALL,25,)
Now the frame can be meshed.
(Alternatively, the command line code for the above step is AMESH,ALL)
You should now have the following:
Saving Your Job
Utility Menu > File > Save as...
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.
(Alternatively, the command line code for the above step is ANTYPE,0)
As shown previously, the left end of the plate is fixed.
You will see some blue triangles in the graphics window indicating the displacement contraints.
(Alternatively, the command line code for the above step is DL,4,,ALL,0)
The applied loads and constraints should now appear as shown below.
![[Loads & Constraints]](./images/Constrained.gif)
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 on the right hand side of the plate and was calculated to be 0.001 mm - neglecting the effects of the hole in the plate (ie - just a flat plate). The actual deflection of the plate is therefore expected to be greater but in the same range of magnitude.
Stress: The maximum stress occurs at the top and bottom of the hole in the plate and was found to be 3.9 MPa.
At this point we need to find whether or not the final result has converged. We will do this by looking at the deflection and stress at particular nodes while changing the size of the meshing element.
Since we have an analytical solution for the maximum stress point, we will check the stress at this point. First we need to find the node corresponding to the top of the hole in the plate. First plot and number the nodes
The equivalent stress was found to be 2.9141 MPa at this point. We will use smaller elements to try to get a more accurate solution.
Note the shapes of both the deflection and stress curves. As the number of elements in the mesh increases (ie - the element edge length decreases), the values converge towards a final solution.
The von Mises stress at the top of the hole in the plate was found to be approximatly 3.8 MPa. This is a mere 2.5% difference between the analytical solution and the solution found using ANSYS.
The approximate maximum displacement was found to be 0.0012 mm, this is 20% greater than the analytical solution. However, the analytical solution does not account for the large hole in the center of the plate which was expected to significantly increase the deflection at the end of the plate.
Therefore, the results using ANSYS were determined to be appropriate for the verification model.
Now we will return to the analysis of the bracket. A combination of GUI and the Command line will be used for this example.
The problem to be modeled in this example is a simple bracket shown in the following figure. This bracket is to be built from a 20 mm thick steel plate. A figure of the plate is shown below.
This plate will be fixed at the two small holes on the left and have a load applied to the larger hole on the right.
Again, Boolean operations will be used to create the basic geometry of the Bracket.
The main rectangular shape has a width of 80 mm, a height of 100mm and the bottom left corner is located at coordinates (0,0)
BLC4, XCORNER, YCORNER, WIDTH, HEIGHT BLC4, X coord (bottom left), Y coord (bottom left), width, height
The center of the circle is located at (80,50) and has a radius of 50 mm
The following code is used to create a circular area:
CYL4, XCENTER, YCENTER, RAD1 CYL4, X coord for the center, Y coord for the center, radius
| parameter | circle 2 | circle 3 |
|---|---|---|
| XCENTER | 0 | 0 |
| YCENTER | 20 | 80 |
| RADIUS | 20 | 20 |
| XCORNER | -20 |
| YCORNER | 20 |
| WIDTH | 20 |
| HEIGHT | 60 |
Your screen should now look like the following...
We now want to add these five discrete areas together to form one area.
(Alternatively, the command line code for the above step is AADD,ALL)
You should now have the following model:
| parameter | circle 1 | circle 2 | circle 3 |
|---|---|---|---|
| WP X | 80 | 0 | 0 |
| WP Y | 50 | 20 | 80 |
| radius | 30 | 10 | 10 |
(Alternatively, the command line code for the above step is ASBA,6,ALL)
Now you should have the following:
As in the verification model, PLANE82 will be used for this example
(Alternatively, the command line code for the above step is ET,1,PLANE82 followed by KEYOPT,1,3,3)
(Alternatively, the command line code for the above step is R,1,20)
We are going to give the properties of Steel. Enter the following when prompted:
| EX 200000 | |
| PRXY 0.3 |
(The command line code for the above step is MP,EX,1,200000 followed by MP,PRXY,1,0.3)
(Alternatively, the command line code for the above step is AESIZE,ALL,5,)
(Alternatively, the command line code for the above step is AMESH,ALL)
Saving Your Job
Utility Menu > File > Save as...
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.
(Alternatively, the command line code for the above step is ANTYPE,0)
As illustrated, the plate is fixed at both of the smaller holes on the left hand side.
As shown in the diagram, there is a single vertical load of 1000N, at the bottom of the large bolt hole. Apply this force to the respective keypoint ( Solution > Define Loads > Apply > Structural > Force/Moment > On Keypoints Select a force in the y direction of -1000)
The applied loads and constraints should now appear as shown below.
Solution > Solve > Current LS
As shown previously, it is necessary to prove that the solution has converged. Reduce the mesh size until there is no longer a sizeable change in your convergence criteria.
The graphic should be similar to the following
