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 an example of the calculation of a structure consisting of several volumes that are not merged with each other. There is a geometric gap between the two volumes, so instead of “gluing” the volumes, the bounded contact will be used. The model represents a quarter of the original part.
The model is fixed on the lateral faces of the symmetry conditions. The inner surface of the hole is fixed in all degrees of freedom. A pressure of 1 MPa is applied to the upper face of the part. Material parameters: Young's modulus E = 2e11 Pa, Poisson’s ratio ν = 0.3.
1. Import geometry.
In the standard line select Menu - File - Import. Specify the path to the file geom_example_contact.stp. If you cannot download the model, right-click on its name and select Save target as.... Then specify the folder where you want to go. place it.
The file can also be found in the folder C:\Program Files\Fidesys\CAE-Fidesys-9.0\preprocessor\bin\help\fidesys_example_tutorials\TestsFromHelp\models and select the specified model.
In the window that appears, click Finish with all the default values of settings.
In the Tree on the left you can see three volumes into which the model is separated. All three volumes have no common surfaces.
1. On the command bar, select the volume mesh module (Mode — Mesh, Entity — Volume, Action — Intervals).
Specify the following parameters:
In the drop-down list, select: Approximate Size;
Select Volumes: 1;
Approximate Size: 0.1.
Click Apply Size.
Click Mesh.
2. On the command bar, select the volume mesh module (Mode — Mesh, Entity — Volume, Action — Intervals).
Specify the following parameters:
In the drop-down list, select: Approximate Size;
Select Volumes: 2;
Approximate Size: 0.3.
Click Apply Size.
Click Mesh.
3. On the command bar, select the volume mesh module (Mode — Mesh, Entity — Volume, Action — Intervals).
Specify the following parameters:
In the drop-down list, select: Approximate Size;
Select Volumes: 2;
Approximate Size: 0.3.
Click Apply Size.
Click Mesh.
Thus, a non-conformal finite element mesh was created on the model.
1. Create a material.
In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
In the Materials Management window that opens, in the second column, click on the caption Enter the name of the material and write “material1”. Click the ENTER key.
In the left column, select Elasticity - Isotropic Material. Select with the mouse the characteristic Young's modulus. Hold down the left mouse button and drag the label to Material Properties. Double-click in the Value field next to Young’s modulus and enter the number 2e+11.Similarly, from the Isotropic Material section add the Poisson ratio 0.3
Click Apply.
Close the Materials management window.
2. Create a block of the 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: 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: material1;
Coordinate System: Global Cartesian;
Order: 1.
Click Apply.
1. Fix the sides of the part with the condition of symmetry.
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): 2 27 38 (or select the vertices with the mouse while holding down the Ctrl key);
Degrees of Freedom: X.
Click Apply.
2. 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): 5 22 23 36 (or select the vertices with the mouse by pressing the Ctrl key);
Degrees of Freedom: Z.
Click Apply.
3. Fix the hole.
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 (or select the vertices with the mouse by pressing the Ctrl key);
Degrees of Freedom: Fix All.
Click Apply.
4. Apply pressure to the top face.
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): 17 37;
Value: 1e6 (the exponential type of the number is supported using the Latin letter “e”).
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:
Auto Selection;
Entity List: Global;
Type: Tied;
Tolerance: 0.055;
Method: Auto.
Click Apply.
In the Tree on the left, find the Boundary Conditions - Constraints - Contacts.
Two contact pairs are automatically identified.
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 calculation parameters:
Dimension: 3D;
Model: Elasticity.
Click Apply.
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 calculation results.
2. Display the Contact Status Node for the model.
3. Display displacements for the deformed view of the model.
On the Properties page, set the Scale Factor to 2000.
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.