Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
The problem of loading a rectilinear pipe element with internal pressure is considered.
1. Create a straight line.
On the command bar, select the module for constructing geometry (Mode - Geometry, Entity - Curve, Action - Create).
From the list of geometric entities, select Line.
Set the following parameters:
Build Using: Locations;
Location: 0 0 0 (beginning of line);
Location: 2 0 0 (end of line).
Click Apply.
1. On the command bar, select the mesh module (Mode - Mesh, Entity - Curve, Action - Intervals).
Specify the degree of mesh refinement:
Select Curves: 1;
Select the mesh construction method: Equal;
Select construction parameters: Interval;
Interval: 10.
Click Apply Size.
Click Mesh.
1. In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).
Drag "Steel" from the "Imported Material" column to the "Material" window.
Click Apply.
Close the Material 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: Curve;
Entity ID(s): 1 (or 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: Beam;
Material: Steel;
Coordinate System: Global Cartesian;
Order: 1.
Set the properties of the beam, to do this, click on the button 
. From the Section profile drop-down list, select Pipe.
Set the following parameters:
Profile Mesh Quality: Coarse;
Outer Diameter (D1): 0.1;
Inner Diameter (D2): 0.098;
Internal Pressure (p2): 1e6.
Click Apply.
Close the Set Beam Properties 1 window.
Click Apply.
1. Secure the ends of the curve in & all directions.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity - Displacement, Action - Create).
Set the following parameters:
Entity List: Vertex;
Entity ID(s): 2 1;
Degrees Of Freedom: All;
DOF Value: 0.
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.
2. Set the output of intermediate results.
On the command bar, select the calculation settings module Static - Output Fields.
Set the flag Output results in 3D view (for beams and shells).
Set the flag Output Static or Preload intermediate results:
Output intermediate results: Every (substeps) - 1.
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.
2. Open a 3D image of the beam.
To do this, click on the name of the *.pvd file in the Entity Tree and
click button 
3D view in standard FidesysViewer.
3. Display the strain component.
In the FidesysViewer window, select the data result in the top panel. calculation for display. From the first drop-down list, select Strain, from the second - Mises, from the third - Surface.
4. Select the point where you want to check the strain.
In the main menu, select the Probe Location filter. In the tab Properties set the coordinates of the point at which you want to check strain:
Point (coordinates): 1 0.05 0;
Number of Points: 1;
Radius: 0.
Click Apply.
The results at the selected point will be displayed on the right side of the screen:
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.