Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
In this example, a plate under the action of creep is considered.
1. Create a rectangle.
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Create).
Select Rectangle in the list of geometric elements.
Set the brick dimensions:
Width: 1;
Height 100;
ZPlane.
Click Apply.
2. Move the created rectangle.
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Transform).
From the list of geometric entities, select Move.
Set the parameters:
Surface ID(s): 1;
Select Method: Distance;
X Distance: 0.5;
Y Distance: 50.
Click Apply.
1. Create a mesh for the rectangle.
On the command bar, select the surface mesh module (Mode — Mesh, Entity — Surface, Action — Mesh).
Set the following parameters:
Automatically Calculate;
Select Surfaces: 1.
Click Apply.
Click Mesh.
1. In the command bar, select the module for specifying material properties (Mode - Material, Entity - Material Management).
Specify the material name Salt. Drag the Isotropic Material label from the left column to the column material properties. Set the following options:
Young's modulus: 941;
Poisson ratio: 0.3.
In the window on the left, go to the General section and drag Density to the Material Properties window. Enter value:
Density: 0.00217.
Next, go to the Plasticity section. Drag Drucker-Prager-Creep Criterion in the Material Properties window. Enter values:
Cohesion: 1000;
Internal friction angle: 0;
Dilatacy angle: 0;
A coefficient: 2.28e-08;
N coefficient: 3.34;
M coefficient: -0.82.
Click Apply.
Close the Materials management window.
2. Set up a block of one type of 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: Surface;
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: Plane;
Material: Salt;
Coordinate System: Global Cartesian;
Order: 2.
Click Apply.
1. Fix curve 3 in the Y direction.
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): 3;
Degrees of Freedom: Y.
Click Apply.
2. Fasten curve 2 in the X direction.
Set the following parameters:
Entity List: Curve;
Entity ID(s): 2;
Degrees of Freedom: X-Translation Disp.
Click Apply.
3. Apply pressure.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity - Pressure, Action - Create).
Set the following parameters:
Entity List: Curve;
Entity ID(s): 1;
Value: 20.
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 - Static, Static - General).
Set the following parameters:
Dimensions: 2D;
Plain State: Plane Strain;
Model: Elasticity, Plasticity;
Set Static Load Steps Count;
Load Steps Count: 50;
Set Nonlinear Solver Options:
- Min Load Substeps: 10;
- Max Load Substeps: 1000000;
- Max Iterations: 1000;
- Tolerance: 1е-3;
- Target Iterations: 5;
- Uncheck Line Search.
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 results of the calculation.
2. Select any point on the surface with the Select Points On tool.
3. Plot a timeline for this point. Select Menu - Filters- Alphabetical - Plot Selection Over Time. Click Apply. Select Stress YY as the field to display on the graph.
Also, using the same filter on one graph, you can build Creep Strain XX, Creep Strain YY, Creep Strain ZZ.
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.