Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
An analysis of the stress-strain state (SSS) of the rock with a working, under the pressure of the upper layers. The calculation is done in 2D, taking into account axisymmetry.
1. Create a rectangle.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action - Create).
From the list of geometric entities, select Rectangle.
Set the following parameters:
Width: 10;
Height: 10;
ZPlane.
Click Apply.
2. Create a circle with a radius of 2.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action - Create).
From the list of geometric entities, select Circle.
Set the following parameters:
Specify Circle Using: Radius;
Radius: 2;
ZPlane.
Click Apply.
3. Subtract the circle from the rectangle.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action - Boolean).
From the list of boolean operations, select Subtract.
Set the following parameters:
A Surface ID(s): 1;
B Surface ID(s): 2.
Click Apply.
4. Leave half of the model.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action - Webcut).
From the list of possible cut types, select Coordinate Plane.
Set the following parameters:
Body ID(s): 1;
Plane: YZ;
Offset Value: 0.
Click Apply.
5. Remove surface 5.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action - Delete).
Set the following parameters:
Surface ID(s): 5.
Click Apply.
1. Build the mesh.
On the command bar, select the surface mesh module (Mode - Mesh, Entity - Surface, Action - Intervals).
Specify the degree of mesh refinement:
Select the way to build the mesh: Approximate Size;
Select Surfaces: 4;
Approximate Size: 0.05.
Click Apply Size.
Click Mesh.
1. In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
Drag the Soil material from the Imported Material column.
Click Apply.
Close the Material management window.
2. 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: Surface;
Entity ID(s): 4.
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 or all;
Category: Plane;
Material: Soil;
Coordinate System: Global Cartesian;
Order: 1.
Click Apply.
1. Fasten the bottom end along the vertical movements.
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): 10;
Degrees Of Freedom: Y.
Click Apply.
2. Fasten the right end along the horizontal movements.
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): 4;
Degrees Of Freedom: X.
Click Apply.
3. Apply pressure to the top face.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity - Pressure, Action - Create).
Set the following parameters:
Enttity List: Curve;
Entity ID(s) 11;
Value: 1e7.
Click Apply.
1. Set the type of problem you want to solve.
On the command panel, select the calculation settings module (Mode - Calculation Settings, Calculation Settings - Static, Static - General).
Select:
Dimensions: 2D;
Plain state: Axisymmetric;
Model: Elasticity.
Click Apply.
Click Start Calculation.
2. In the window that appears, select the directory where 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, allowing you to view with calculation results.
2. In the top panel, select the calculation result data to display. From the first drop-down list select Displacement, from the second – Magnitude, from the third – Surface.
The picture below shows the total movements.
3. In the top panel, select the calculation result data to display. From the first drop-down list select Stress, from the second - Mises, from the third – Surface.
The picture below shows the von Mises stress distribution.
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.