Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
To implement this type of loading, Fidesys uses this type of contact as "tangentially connected", which allows surfaces to interpenetrate contact with each other, but does not allow their relative transverse displacement than the integrity of the bolt body is maintained.
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: 0.02;
Section type: Circular;
Radius: 0.005.
Click Apply.
2. Create inner 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: 0.015;
Section type: Circular;
Radius: 0.01.
Click Apply.
3. Cut the volume of the inner cylinder into two horizontally.
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: XY;
Offset Value: 0.
Click Apply.
4. Cut the volume of the outer cylinder into two parts horizontally.
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): 2;
Cut Plane: XY;
Offset Value: 0.
Click Apply.
5. Move part of the outer cylinder up.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action — Transform).
Select Move from the dropdown list.
Set the following parameters:
Surface ID(s): 11;
Check the box: Include Merged.
Select Method: To Entity;
Surface;
Surface ID: 3.
Click Apply.
6. Move part of the outer cylinder up.
On the command bar, select the module for constructing surface geometry (Mode - Geometry, Entity - Surface, Action — Transform).
Select Move from the dropdown list.
Set the following parameters:
Surface ID(s): 13;
Check the box: Include Merged.
Select Method: To Entity;
Surface;
Surface ID: 2.
Click Apply.
7. Imprint the top cylinders.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Imprint and Merge).
From the list select Imprint/Merge Volumes.
Set the following parameters:
Volume ID(s): 1 2.
Click Apply.
8. Imprint the lower cylinders.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action — Imprint and Merge).
From the list select Imprint/Merge Volumes.
Set the following parameters:
Volume ID(s): 3 4.
Click Apply.
1. Create a mesh on volumes.
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: 5.
Click Apply Size.
Click Mesh.
1. Specify the material.
In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
In the column "Imported material", double-click on Steel.
Click Apply.
Close the Materials 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:
Entity List: Volume;
Entity ID(s): 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: Solid;
Materials: Steel;
Coordinate System: Global Cartesian;
Order: 1.
Click Apply.
1. Set the boundary conditions for displacements.
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): 18;
Degrees of Freedom: Fix All.
Click Apply.
2. Set the boundary conditions for displacements.
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): 16;
Degrees of Freedom: Fix All.
Click Apply.
3. Define a tangent contact between preloaded surfaces.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Contact, Action — Create).
From the drop-down list, select: Master and Slave Selection.
Set the following parameters:
Master Entity: Entity List: Surface;
Entity ID(s): 7;
Slave Entity: Entity List: Surface;
Entity ID(s): 9;
Type: Tied Tangent;
Preload: 1000;
Tolerance: 0.0005;
Method: Auto.
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:
Dimensions: 3D;
Model: Elasticity.
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. From the first dropdown select Displacement, from the second select Magnitude.
3. Apply the "Warp By Vector" filter to display the results in deformed form.
On the top line, select (Menu - Filters — Alphabetical - Warp By Vector).
In Properties select:
Vectors: Displacement;
Scale Factor: 400;
Performance: Surface With Edges.
Click Apply.
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.