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, we consider the loading of a disk segment subjected to a force effect on the outer parallelepiped elements that simulate blades. The disc is fixed to the inner diameter.
We consider a part of the disc. The problem is solved using periodic boundary conditions.
1. Create the first circular cylinder.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
Select Cylinder from the list of geometric primitives.
Set the following parameters:
Height: 1;
Section type: Circular;
Radius: 10.
Click Apply.
2. Create the second circular cylinder.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
Select Cylinder from the list of geometric primitives.
Set the following parameters:
Height: 1;
Section type: Circular;
Radius: 1.
Click Apply.
3. Subtract the second cylinder from the first.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Boolean).
From the list of operations, select Subtract.
Set the following parameters:
A Volume ID(s): 1 (volumes from which other volumes will be subtracted);
B Volume ID(s): 2 (volumes to be subtracted).
Click Apply.
4. Leave the segment.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Webcut).
Select Coordinate Plane from the list of available section views.
Set the following parameters:
Volume ID(s): 1;
Cut Plane: ZX;
Offset Value: 0;
Rotate Plane;
Angle: 15;
Direction: Z Axis;
Center X, Y, Z: 0 0 0.
Click Apply.
Do the same for the other angle.
Volume ID(s): 1;
Cut Plane: ZX;
Offset Value: 0;
Rotate Plane;
Angle: -15;
Direction: Z Axis;
Center X, Y, Z: 0 0 0.
Click Apply.
5. Remove volumes 1 and 3. To do this, while holding down the Ctrl key, select these volumes in the model tree and click Delete in the context menu.
6. Create a brick.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
Select Brick from the list of geometric primitives.
Set the following parameters:
X (width): 4;
Y (height): 3;
Z (depth): 1.
Click Apply.
7. Rotate the brick.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Transform).
From the list of operations, select Rotate.
Set the following parameters:
Volume ID(s): 5;
Include Merged;
Angle: 90;
Rotate About: X-Axis.
Click Apply.
8. Move the brick.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Transform).
From the list of operations, select Move.
Set the following parameters:
Volume ID(s): 5;
Include Merged;
Select Method: Distance;
X Distance: 11.
Click Apply.
9. Cut the brick.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Webcut).
From the list of available section views, select Plane From Surface.
Set the following parameters:
Volume ID(s): 5;
Plane From Surface ID: 31.
Click Apply.
Do the same for the other surface.
Volume ID(s): 6;
Plane From Surface ID: 29.
Click Apply.
10. Delete volumes 6 and 5. To do this, hold down the Ctrl key, select these volumes in the model tree and click Delete in the context menu.
11. Merge the remaining volumes.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Boolean).
From the list of operations, select Intersect.
Set the following parameters:
Volume ID(s): 4 7.
Click Apply.
1. On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action - Intervals).
Set the following parameters:
Automatic Sizing;
Select Volumes: 4;
Auto Factor: 4.
Click Apply Size.
2. On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action — Mesh).
Set the following parameters:
Automatically Calculate;
Select Volumes: 4.
Click Mesh.
1. Attach one side edge.
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): 30;
Degrees Of Freedom: X, Y, Z.
Click Apply.
2. Apply pressure.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity — Pressure, Action - Create).
Set the following parameters:
Entity List: Surface;
Entity ID(s): 58;
Value: 1e5.
Click Apply.
3. Set the periodic condition.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity — Periodic Condition, Action - Create).
Set the following parameters:
Entity List (Master Entity): Surface;
Entity ID(s) (Master Entity): 27;
Entity List (Slave Entity): Surface;
Entity ID(s) (Slave Entity): 11;
General;
Coordinate System: Global Cartesian*;
Number of Sectors: 12.
Click Apply.
* For calculations taking cyclic symmetry into account, it is sufficient to specify a Cartesian coordinate system. In fact, for correct calculations, the direction of the Z-axis and the origin of the coordinates are required.
1. Create a material.
In the command bar, select the module for specifying material properties (Mode - Material, Entity - Material Management).
In the Manage Materials window that opens, drag the Material Carbon Steel from the third column. Specify the name of the material and write «Steel». Click the ENTER key.
Click Apply.
Close the Materials 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: Volume;
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;
Category: Solid;
Material: Steel;
Coordinate System: Global Cartesian;
Order: 1.
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: 3D;
Model: Elasticity.
Click Apply.
2. On the command bar, select the calculation settings module (Mode - Calculation Settings, Calculation Settings - Static, Static - Output Fields).
Put a tick Full Model for Periodic BCs.
Click Apply.
Click Start Calculation.
3. In the window that appears, select the directory where the result will be saved 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.
Show the Displacement component.
In the FidesysViewer window on the toolbar, set the following parameters:
Display field: Displacement (Magnitude);
Display type: Surface.
Display Equivalent Stress.
Display field: Stress (Mises);
Display type: Surface.
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.