Search the documentation
Enter at least 2 characters
 |
CAE Fidesys 9.0 Documentation |
Enter at least 2 characters
|
CAE Fidesys 9.0 Documentation |
R.J. Roark, Formulas for Stress and Strain, 4th Edition? McGraw-Hill Book Co., Inc., New York, NY, 1965, pg 112, no. 33
The problem of the tube bending of under gravity force is to be solved. The pictures below represent a geometric model of the problem:
The side edges are rigidly fixed on all displacements and rotations. Material parameters are E = 30e6 psi, ν = 0.0, ρ = 0.00073 lb-sec2/in4. The gravity force is defined via the acceleration g = 386 in/sec2. The geometrical dimensions of the model: L = 200 in, d0 = 2 in, di=1 in.
Due to the symmetry of the problem, half tube will now be considered (L/2).
Test pass criterion is the following: displacement in the center of the tube uyy at the point D (0, d0/2, 0) is -0.12529 within 3%.
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 in the list of geometric elements.
Specify the cylinder dimensions:
Height: 100;
Cross section: Circular;
Radius: 1.
Click Apply.
2. Create the second cylinder.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Create).
Select Cylinder in the list of geometric elements.
Specify the cylinder dimensions:
Height: 100;
Cross section: Circular;
Radius: 0.5.
Click Apply.
As a result, two generated entities are displayed in the Model Tree (Volume 1 and Volume 2).
3. Subtract the first cylinder from the second one.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Boolean).
Select Subtract in the list of operations. Set the following parameters:
A Volume ID(s): 1 (the volumes to be subtracted);
B Volume ID(s): 2 (volumes from which other volumes will be subtracted).
Click Apply.
As a result, only one volume is displayed in the Model Tree (Volume 1).
4. Move the resulting volume.
On the command bar, select the module for constructing volume geometry (Mode - Geometry, Entity - Volume, Action - Transform).
From the list of actions, select Move.
Set the following parameters:
Volume ID(s): 1;
Include Merged;
Select Method: Distance;
Z Distance: 50.
Click Apply.
1. Set the approximate size of the elements.
On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action - Intervals).
Specify the Approximate Size of the elements:
Select Volumes: 1;
Approximate Size: 0.25.
Click Apply Size.
2. Select the way of mesh generation.
On the command bar, select the volume mesh module (Mode - Mesh, Entity - Volume, Action - Mesh).
Specify the following parameters:
Select meshing scheme: Sweep.
Select Volumes: 1;
Auto Select Source and Target;
Default.
Click Apply Scheme.
Click Mesh.
The resulting number of elements can be found on the property page by clicking on Volume 1 in the Model Tree on the left.
To view the mesh properties, you can follow these steps:
Select the entire model;
Right-click on the model;
In the pop-up menu, select List Information - List Mesh Info;
Information on the mesh will be displayed in Command Line.
1. Fix the right lateral edge at all directions.
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): 8;
Degrees of Freedom: Fix All.
Click Apply.
2. Fix the left lateral edge along X and Z axes by analogy.
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): 9;
Degrees of Freedom: X, Z.
Click Apply.
3. Set the gravity force.
On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity - Gravity, Action - Create).
Set the following parameters:
Entity List: Global;
Directions: Y;
Y: -386.
Click Apply.
1. Create the 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 Material 1.
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 3e+07.
Similarly, from the Isotropic Material section add the Poisson ratio 0 ; from the section General - Density: 0.00073.
Click Apply.
Close the Materials management window.
2. Create the block of one material type.
On the command bar, select the block management module (Mode - Blocks, Entity - Block, Action - Add).
Set the following parameters:
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: Material 1;
Coordinate System: Global Cartesian;
Order: 1.
Click Apply.
1. Set the type of the problem to be solved.
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. In a pop-up window select a folder to save the result 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.
To apply all of the filters changes automatically
in FidesysViewer, click Apply changes to parameters automatically
on Command Panel.
2. Display the Uyy component of the displacement field on the model.
In FidesysViewer window set the following parameters on Toolbar:
Representation Field: Displacement;
Representation Component: Y;
Representation Mode: Surface.
After applying the settings, you will see the following picture:
3. Check the maximum value Uyy at the selected point D.
In the picture, it is the maximum in modulus Displacement (blue). It corresponds to -0.127222 in the color legend.
The obtained value of -0.128 differs from the required value of -0.12529 by 2.12%.
4. Download numerical data.
Select File → Save Data in the Main Menu or click Ctrl+S. Enter the file name (*.csv format), leave it by default. Click OK. The saved file is an ordinary table of numerical data which can be opened in any text editor.
5. You can see the way the body is deformed under the applied pressure.
To do this, select Filters → Alphabetical → Warp By Vector.
Set the following parameters in the tab Properties:
Vectors: Displacement;
Scale Factor: 100.
As a result, the deformed body is displayed at the picture. To see the original model, click the button near the model in the Model Tree. The picture below shows the deformed (solid grey filling) and the original model (with the field of displacements distribution along Y axis).
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.