Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
NAFEMS Selected Benchmarks for Natural Frequency Analysis "Simply Supported "Solid" Square Plate", Test No FV52.
We solve the problem of modal analysis of a square plate.
The picture represents a geometric model of the problem and a mesh:
The size of the plate is 10 m × 10 m × 1 m. Displacements along z-axis are constrained for the edges of the plate bottom side. The material parameters are E = 200 hPa, ν = 0.3, ρ = 8000 kg/m3.
Eigenmodes from 4 to 10 are to be compared.
1. Create the plate.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
Select Brick in the list of geometric elements.
Set the brick dimensions:
X (width): 10;
Y (height): 10;
Z (depth): 1.
Click Apply.
A mesh of 4*4*1 linear hexahedral elements is to be generated (as shown at the picture with the problem setting).
1. On the command bar, select the mesh module (Mode - Mesh, Entity - Curve, Action - Mesh).
Specify the parameters of mesh refinement:
Select Curves: 1 2 3 4 5 6 7 8 (using space after each of them);
Select the way of meshing: Equal;
Select splitting settings: Interval;
Interval: 4 (see the figure).
Click Apply Size.
2. On the command bar, select the mesh module (Mode - Mesh, Entity - Curve, Action - Mesh).
Specify the parameters of mesh refinement:
Select Curves: 9 10 11 12 (using space after each of them);
Select the way of meshing: Equal;
Select splitting settings: Interval;
Interval: 1.
Click Apply Size.
3. On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action - Mesh).
Specify the parameters of mesh refinement:
Select Meshing Scheme: Automatically Calculate;
Select Volumes: 1 (or by the command all).
Click Apply Scheme.
Click Mesh.
1. Fix the bottom side edges along Z.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity - Displacement, Action - Create).
Set the following parameters:
Entity List: Curve;
Entity ID(s): 5 6 7 8 (using space after each of them);
Degrees of Freedom: Z.
Click Apply.
1. Create the material.
In the command bar, select the module for specifying material properties (Mode - Material, Entity - Materials Manegment).
In the Materials Management window that opens, in the second column, click on the caption Enter the name of the material and write "Material 1".
Click the ENTER key.
In the left column, select Elasticity - Isotropic Material. Select with the mouse the characteristic Young's modulus. Hold down the left mouse button and drag the label to Material Properties. Double-click in the Value field next to Young's modulus and enter the number 2e+11. Similarly, from the Isotropic Material section add the Poisson ratio 0.3. Density: 8000.
Click Apply.
Close the Materials management window.
2. Create a block of one type of the material.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Add).
Set the following parameters:
Block ID: 1;
Entity List: Volume;
Entity ID(s): 1 (or by the command all).
Click Apply.
3. Set the block parameters.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Block properties/parameters).
Set the following parameters:
Block ID(s): 1;
Category: Solid;
Material: Material 1;
Coordinate System: Global Cartesian;
Order: 2.
Click Apply.
1. Set the type of the problem to be solved.
On the command bar, select the calculation settings module (Mode - Calculation Settings, Calculation Settings - Mode Frequency Analysis, Mode Frequency - General).
Specify the following settings:
Dimension: 3D;
Number of Eigenmodes: 10.
Click Apply.
Click Start Calculation.
2. In a pop-up window select a folder to save the result and enter the file name.
3. In the case of a successful calculation, the console displays the message: Calculation finished successfully at "date" "time", as well as the required eigen values and frequencies.
1. Compare the obtained results with those in the given table.
№* |
NAFEMS |
CAE FIDESYS |
Error, % |
4 |
44.762 |
44.796 |
0.08% |
5 |
110.52 |
110.54 |
0.02% |
6 |
110.52 |
110.54 |
0.02% |
7 |
169.08 |
169.10 |
0.01% |
8 |
193.93 |
193.92 |
0.005% |
9 |
206.64 |
206.64 |
0.0% |
10 |
206.64 |
206.64 |
0.0% |
*Since the model is not fixed, the first three natural frequencies must be zero. In this problem, an interval was used to find the natural frequencies that cut off zero values.
2. Open the file with the results. There are three ways to do that.
Click Ctrl+E.
From the main menu, select Calculation. Click Open Results.
Select Results on Command Panel (Mode - Results). Click Open results.
3. You can see the way the body is deformed.
Select a filter Warp By Vector to do this.
Set the following parameters in the tab Properties:
Vectors: Mode # (frequency Hz): displacement (# means the number of the eigenvalue);
Scale Factor: 700.
As a result, the deformed body is displayed at the picture. To see the
original model, click 
near it in the Model
Tree. The picture below shows the deformed model at different eigenvalues.
4 eigenmode
5 eigenmode
6 eigenmode
7 eigenmode
8 eigenmode
9 eigenmode
10 eigenmode
Geometry creating, meshing, setting boundary conditions and materials can be performed using the console interface. Below is a link to the program code that allows you to perform the steps described above manual, you only need to specify the full path and name.