Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
In the proposed problem, the Hertz problem is modeled for two hemispheres with contact. The test task is designed to check the correctness:
setting parameters of sliding contact without friction in the interface;
static solution with sliding contact without friction for 3D models;
the correctness of the output of the Stress field, taking into account the contact interaction.
1. Set the mesh settings.
In the top panel, select (Tools - Options - Mesh Defaults). Check the box: Project Midnodes to Geometry: Always.
1. Create a sphere.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
From the list of geometric primitives, select Sphere.
Set the following parameters:
Radius: 50.
Click Apply.
2. Move the sphere.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Transform).
From the list, select Move.
Set the following parameters:
Volume ID(s): 1;
Include Merged;
Select Method: Distance;
Y Distance: 50.
Click Apply.
3. Create a second sphere.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
From the list of geometric primitives, select Sphere.
Set the following parameters:
Radius: 50.
Click Apply.
4. Move the second sphere.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Transform).
From the list, select Move.
Set the following parameters:
Volume ID(s): 2;
Include Merged;
Select Method: Distance;
Y Distance: -50.
Click Apply.
5. Cut the first sphere in two.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Webcut).
Select from the list Coordinate Plane.
Set the following parameters:
Volume ID(s): 1;
Coordinate plane: ZX;
Offset Value: 50.
Click Apply.
6. Cut the second sphere in two.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Webcut).
Select from the list Coordinate Plane.
Set the following parameters:
Volume ID(s): 2;
Coordinate plane: ZX;
Offset Value: -50.
Click Apply.
7. Delete the cut off parts of the spheres.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Delete).
Set the following parameters:
Volume ID(s): 2 3.
Click Apply.
8. Cut the geometry in two.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Webcut).
Select from the list Coordinate Plane.
Set the following parameters:
Volume ID(s): all;
Coordinate plane: YZ;
Offset Value: 0.
Click Apply.
9. Cut the geometry in two.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Webcut).
Select from the list Coordinate Plane.
Set the following parameters:
Volume ID(s): all;
Coordinate plane: XY;
Offset Value: 0.
Click Apply.
10. Remove parts of the spheres.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Delete).
Set the following parameters:
Volume ID(s): 5 6 7 8 9 10.
Click Apply.
1. Create a polyhedral mesh for the entire model.
On the command bar, select the volume mesh module (Mode — Mesh, Entity – Volume, Action – Mesh).
Select from the list Polyhedron.
Select Volumes: all.
Click Mesh.
2. Create a mesh.
On the command bar, select the volume mesh module (Mode — Mesh, Entity – Volume, Action – Intervals).
Select from the list Automatic Sizing.
Select Volumes: all;
Auto Factor: 4.
Click Apply Size.
Click Mesh.
1. Set the first material.
In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
In the column "Material" enter the name of the material Material 1.
Click Apply.
In the column "Material properties" select the created material, then drag the desired properties to it from the left column.
Drag properties and specify their value:
Young's Modulus: 20000;
Poisson ratio: 0.3.
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:
Block ID: 1;
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: Material 1;
Coordinate System: Global Cartesian;
Order: 1.
Click Apply.
1. Fix the plate at X.
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): 25 33;
Degrees of Freedom: X.
Click Apply.
2. Fix the plate at Z.
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): 23 31;
Degrees of Freedom: Z.
Click Apply.
3. Set displacement
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): 24;
Degrees of Freedom: Y.
Click Apply.
4. Set displacement
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): 34;
Degrees of Freedom: Y.
Click Apply.
5. Set the contact condition.
On the command panel, select the boundary conditions module (Mode — Boundary Conditions, Entity — Contact, Action — Create).
Set the following parameters:
Master and Slave Selection;
Master Entity;
Entity List: Surface;
Entity ID(s): 32;
Slave Entity;
Entity List: Surface;
Entity ID(s): 26;
Type: General;
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).
Please select:
Dimension: 3D;
Model: Elasticity.
Set Nonlinear Solver Options:
Min. Load Substeps: 10;
Max. Load Substeps: 30;
Max. Iterations: 50;
Tolerance: 1e-3;
Click Apply.
2. Set additional settings.
On the command bar, select the calculation settings module (Mode - Calculation Settings, Calculation Settings - Static, Static - Output Fields).
Check the box next to the parameters:
Click Apply.
Click Start Calculation.
3. In a pop-up window select a folder to save the result 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.
2. On the top panel, select the data of the calculation result to display. From the first dropdown list select Stress, from the second – YY.
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.