Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
1. Create a first brick.
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): 0.006;
Y (height): 0.012;
Z (depth): 0.25.
Click Apply.
2. Create a second brick.
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): 0.006;
Y (height): 0.012;
Z (depth): 0.25.
Click Apply.
3. Move the second brick.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Transform).
From the pop-up list, select Move.
Specify the required parameters:
Volume ID(s): 2;
Include Merged;
Select Method: Distance;
Х Distance: 0.1.
Click Apply.
4. Create a vertex.
On the command bar, select the module for constructing geometry (Mode - Geometry, Entity - Vertex, Action - Create).
From the pop-up list, select Coordinates.
Set the following parameters:
X Coordinate: 0.05;
Y Coordinate: 0;
Z Coordinate: 0.125;
Create On: Surface.
Click Apply.
1. Set mesh parameters.
On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action - Intervals).
From the list of actions, select Automatic Sizing.
Set the following parameters:
Select Volumes: all;
Auto Factor: 4 (move the slider to 4).
Click Apply Size.
Click Mesh.
2. Set the mesh parameters.
On the command bar, select the mesh module (Mode - Mesh, Entity - Vertex, Action - Mesh).
Specify the required parameters:
Vertex ID(s): 17.
Click Mesh.
1. In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
Specify the name of the first material, stal.
Drag the text from the left column Isotropic Material in the Material Properties column.
Set the following parameters:
Young's modulus: 2.07e+11;
Poisson ratio: 0.3.
Click Apply.
Specify the name of the second material alum. Drag the text from the left column Isotropic Material in the Material Properties column.
Set the following parameters:
Young's modulus: 7.31e+10;
Poisson ratio: 0.3.
Click Apply.
Close the Materials management window.
2. Create the first block.
Create a block.
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.
Click Apply.
3. Create a second block.
Create a block.
On the command bar, select the block management module (Mode — Blocks, Entity — Block, Action — Add).
Set the following parameters:
Block ID: 2;
Entity List: Volume;
Entity ID(s): 2.
Click Apply.
4. Create a third block.
Create a block.
On the command bar, select the block management module (Mode — Blocks, Entity — Block, Action — Add).
Set the following parameters:
Block ID: 3;
Entity List: Vertex;
Entity ID(s): 17.
Click Apply.
5. Set parameters for the first block.
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: stal;
Coordinate System: Global Cartesian;
Order: 2.
Click Apply.
6. Set parameters for the second block.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Block properties/parameters).
Set the following parameters:
Block ID(s): 2;
Category: Solid;
Material: alum;
Coordinate System: Global Cartesian;
Order: 2.
Click Apply.
6. Set parameters for the second block.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Block properties/parameters).
Set the following parameters:
Block ID(s): 3;
Category: Lumped Mass;
Coordinate System: Global Cartesian;
Block Properties ID: 1.
Set the properties of the lump mass, to do this, click on the button
.
Set the following parameters:
Set Masses: Mass;
Mass: 1e-07.
Click Apply.
Close the Set Lumped Mass Properties window.
Click Apply.
1. Secure entity 2, 8 along all axes.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Displacement, Action — Create).
Set the following parameters:
Entity List: Surface;
Entity ID(s): 2 8;
Degrees Of Freedom: Fix All.
Click Apply.
2. Fix entity10, 6 along the X axis.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Displacement, Action — Create).
Set the following parameters:
Entity List: Surface;
Entity ID(s): 10 6;
Degrees Of Freedom: Х.
Click Apply.
3. Apply a point force to vertex 17.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Force, Action — Create).
Set the following parameters:
Force Entity List: Vertex;
Entity ID(s): 17;
Force Х Component: 0;
Force Y Component: -1000;
Force Z Component: 0;
Moment Х Component: 0;
Moment Y Component: 0;
Moment Z Component: 0.
Click Apply.
4. Make connections.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Coupling Constraint, Action — Create).
Set the following parameters:
From the pop-up list, select Master and Slave Selection.
Master Entity: Entity List: Vertex;
Entity ID(s): 17;
Slave Entity: Entity List: Surface;
Entity ID(s): 7 1;
Interpolation;
Master: All;
Slave: All;
Factor: 1.
Click Apply.
1. Specify the type of task you want to solve.
On the command bar, select the calculation settings module (Mode — Calculation Settings, Settings Calculation — Static, Static — General).
Set the following parameters:
Dimensions: 3D;
Model: Elasticity.
Click Apply.
2. Set the output fields.
On the command bar, select the calculation settings module (Mode — Calculation Settings, Settings Calculation — Static, Static — Output Fields).
Check the box next to Nodal and Reaction Forces.
Click Apply.
Click Start Calculation.
3. In a pop-up window select a folder to save the result and enter the file name.
4. 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.
Display Displacements (Magnitude) on the model.
Display Stress (Mises) on the model.
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.