Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
We consider stepwise plate stretching. A round inclusion is made in the plate from the main material (i.e. the material is the same throughout the plate). The problem is solved in 2 steps of loading. At the first step, the plate undergoes uniaxial tension along the x axis,in the second step, the load is removed and the material is replaced for inclusion in such a way that Young's modulus and Poisson's ratio remain the same, but zero initial stresses are set. Stresses around the inclusion at the last loading step are analyzed.
1. Create a plate with a side of 100.
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Create).
From the list of geometric primitives, select Rectangle.
Set the following parameters:
Width: 100.
Click Apply.
2. Create a circle with a radius 10.
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Create).
From the list of geometric primitives, select Circle.
Set the following parameters:
Radius: 10;
Select ZPlane.
Click Apply.
3. Cut the circle out of the plate while keeping the originals (Save In).
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Boolean).
From the list of operations, select Subtract.
Set the following parameters:
А Surface ID(s): 1;
В Surface ID(s): 2;
Keep Originals.
Keep В.
Click Apply.
4. Merge geometry.
On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Merge).
From the list of actions, select Merge.
Set the following parameters:
Surface ID(s): all.
Click Apply.
On the command bar, select the surface mesh module (Mode - Mesh, Entity - Surface, Action - Intervals).
Set the following parameters:
Automatic Sizing;
Select Surfaces: all.
Click Mesh.
In the command bar, select the module for specifying material properties (Mode - Material, Entity - Materials Management).
Create two materials.
material 1:
Young's modulus Е = 210000;
Poisson ratio ν = 0.3.
material 2:
Young's modulus Е = 210000;
Poisson ratio ν = 0.3.
Click Apply.
Close the Materials management window.
1. 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: Surface;
Entity ID(s): 3.
Click Apply.
2. Create the second 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: Surface;
Entity ID(s): 2.
Click Apply.
3. Set parameters for blocks 1 and 2.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Block properties/parameters).
Set the following parameters:
Block ID(s): all;
Category: Plane;
Material: material 1;
Coordinate System: Global Cartesian;
Order: 2.
Click Apply.
1. Fix the right and left sides according to the symmetry condition 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: Curve;
Entity ID(s): 2 4;
Degrees of Freedom: Х-Translation Disp;
DOF Value: 0.
Click Apply.
2. Fix some knot in the center of the plate along all degrees of freedom.
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 5;
Degrees of Freedom: All;
DOF Value: 0.
Click Apply.
3. Set the pressure to 100 MPa (tensile) on the top and bottom faces.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Pressure, Action — Create).
Set the following parameters:
Pressure Entity List: Surface;
Entity ID(s): 1 3;
Magnitude Value: -100.
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).
Select:
Dimension: 2D;
Plain state: Plane strain;
Model: Elasticity;
Set static load steps count;
Load steps count: 2.
2. Set active steps for pressure: 1.
3. Change the material in the second step to material 2.
Click Apply.
Click Start Calculation.
4. In the window that appears, select the directory in which the result will be saved and enter the file name.
5. 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.
2. Display the Stress field on a surface with ribs.
In the resulting FidesysViewer window toolbar, set the following parameters:
Display type: Surface with ribs;
Display field: Displacement;
Display Component: Voltages.
The model displays a voltage distribution box.
Step 1
Step 2
At the last step of the solution for the deformed view, the plate returned to its original
condition, and the cutout remained elliptical.
For comparison, a solution without zero initial stresses for the second material is shown.:
Step 1
Step 2
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.