Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
The problem of beam oscillation under the influence of acceleration is solved. The considered period of time is 5 s. The beam model is fixed (embedment), acceleration (0.01 m / s 2 ) is applied at the ends.
1. Create a straight line with a length of 100.
On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Curve, Action — Create).
From the list of geometric primitives, select Line.
Creatе, build using Location and Direction.
Set the following parameters:
Location: 0 0 0 (top of the line);
Direction: 1 0 0 (along the Х axis);
Length: 100.
Click Apply.
1. On the command bar, select the mesh module (Mode — Mesh, Entity — Curve, Action — Mesh).
Specify the mesh refinement degree:
Select Curves: all;
Select a method for constructing the mesh: Equal;
Select the construction parameters: Auto Size;
Auto Factor: 3.
Click Apply Size.
Click Mesh.
1. In the command bar, select the module for specifying material properties (Mode - Material, Entity - Materials Management).
Drag "Carbon steel" from the "Imported Material" column to the "Material" window.
Click Apply.
Close the Material management window.
2. Create a block of one material type.
On the command bar, select the block management module (Mode — Blocks, Entity — Block, Action — Add).
Set the following parameters:
Block ID: 1;
Entity List: Curve;
Entity ID(s): 1 (or 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: Beam;
Material: Steel;
Coordinate System: Global Cartesian;
Order: 1.
Set the properties of the beam, to do this, click on the button 
. From the Section profile drop-down list, select I-Beam.
Set the following parameters:
Height (H): 0.1;
Bottom Width (B1): 0.055;
Top Width (B2): 0.055;
Top Thickness (c1): 0.0072;
Top Thickness (c2): 0.0072;
Thickness (d): 0.0045.
Click Apply.
Close the Set Beam Properties window.
Click Apply.
1. Pin top 2 in all directions.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Displacement, Action — Create).
Set the following parameters:
Entity List: Vertex;
Entity ID(s): 2;
Degrees of Freedom: Fix All.
Click Apply.
2. Set the acceleration.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Acceleration, Action — Create).
Set the following parameters:
Entity List: Vertex;
Entity ID(s): 1;
Degrees of Freedom: Z.
Click Apply.
1. Set the type of problem you want to solve.
On the command bar, select the calculation settings module (Mode — Calculation Settings, Calculation Settings - Transient Analysis, Transient - General).
Set the following calculation parameters:
Dimension: 3D;
Method: Full Solution;
Scheme: Implicit;
Max Time: 1;
Steps Count: 5.
Click Apply.
Click Start Calculation.
2. In the window that appears, select the directory in which the result will be saved, and enter the file name.
3. In the case of a successful calculation, the console displays the message: Calculation finished successfully at "date" "time".
1. 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.
The FidesysViewer window will appear, in which you can view the calculation results.
When switching to FidesysViewer, the result may not be visible, in order to see it you need to rotate the coordinate axes.
Connect the filter Deform by Vector (Menu - Filters - Index - Strain by Vector). Or use the corresponding command panel button:
In the Properties tab, set the following parameters:
Vectors: Displacement;
Scale Factor: 100.
In the Step window, set 0 - the initial view of the model.
t=0
By switching steps from 1 to 5, you can view the deformed view of the model at all steps.
t=1
t=2
t=3
t=4
t=5
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.