CAE Fidesys 9.0 Documentation

Concrete Mobility Test (Cone Slump)

The problem of elastic-plastic calculation for the Drucker-Prager model with tabular (multilinear isotropic) asymmetric hardening in small strains.

Geometry creation

1. Create a vertex.

 On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Vertex, Action — Create).

Select Location in the list of geometric elements.

Set the following parameters:

• Location...: 0 0 0 (through a space).

Click Apply.

2. Create a vertex.

 On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Vertex, Action — Create).

Select Location in the list of geometric elements.

Set the following parameters:

• Location...: 0.1 0 0 (through a space).

Click Apply.

3. Create a vertex.

 On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Vertex, Action — Create).

Select Location in the list of geometric elements.

Set the following parameters:

• Location...: 0.0  0.3  0 (through a space).

Click Apply.

4. Create a vertex.

 On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Vertex, Action — Create).

Select Location in the list of geometric elements.

Set the following parameters:

• Location...: 0.05  0.3  0 (through a space).

Click Apply.

5. Connect the vertices with curves.

On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Curve, Action — Create).

Select Line in the list of geometric elements.

Set the following parameters:

• Build Using: Vertex IDs;

• Vertex IDs: 1 2.

Click Apply.

6. Connect the vertices with curves.

On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Curve, Action — Create).

Select Line in the list of geometric elements.

Set the following parameters:

• Build Using: Vertex IDs;

• Vertex IDs: 2 4.

Click Apply.

7. Connect the vertices with curves.

On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Curve, Action — Create).

Select Line in the list of geometric elements.

Set the following parameters:

• Build Using: Vertex IDs;

• Vertex IDs: 4 3.

Click Apply.

8. Connect the vertices with curves.

On the command bar, select the module for constructing geometry (Mode — Geometry, Entity — Curve, Action — Create).

Select Line in the list of geometric elements.

Set the following parameters:

• Build Using: Vertex IDs;

• Vertex IDs: 3 1.

Click Apply.

9. Create a curved surface.

On the command bar, select the module for constructing surface geometry (Mode — Geometry, Entity — Surface, Action — Create).

Select Bounding Curves in the list of geometric elements.

Set the following parameters:

• Curve ID(s): all.

Click Apply.

10. Create a volume on the surface.

On the command bar, select the module for constructing volume geometry (Mode — Geometry, Entity — Volume, Action — Create).

Select Sweep in the list of geometric elements.

Set the following parameters:

• Surface ID(s): 1;

• Sweep method: About Axis;

• Angle: -90;

• Axis of Rotation: Y-Axis.

• Delete Source Surfaces.

Click Apply.

Meshing

1. On the command bar, select the mesh module (Mode — Mesh, Entity — Curve, Action — Mesh).

From the drop-down list, select Equal.

Set the following parameters:

• Select Curves: 1 3 5 9;

• Interval;

• Interval: 3.

Click Apply Size.

2. Create a mesh.

On the command bar, select the mesh module (Mode — Mesh, Entity — Curve, Action — Mesh).

From the drop-down list, select Equal.

Set the following parameters:

• Select Curves: 2 4 7;

• Interval;

• Interval: 9.

Click Apply Size.

3. Create a mesh on the volume.

On the command bar, select the volume mesh module (Mode — Mesh, Entity — volume, Action — Intervals).

From the drop-down list, select Automatic Sizing.

Set the following parameters:

• Select Volumes: 1.

Click Apply Size.

Click Mesh.

Setting the material and properties of blocks

1. Specify the material.

In the command bar, select the module for specifying material properties (Mode — Material, Entity — Materials Management).

In the Material Management widget, in the middle column, specify the name of the material material.

In the Material Properties column, select the created material, then drag to him the desired properties from the left column.

Drag the following properties:

• Young's modulus;

• Poisson ratio;

• Density;

• Yield strength;

• Yield compressive strength;

• Stress(Strain) curve.

Set the values ​​required for the material properties:

• Young's modulus: 2.25;

• Poisson ratio: 0.125;

• Density: 0.1;

• Yield strength: 0.00148461;

• Compressive yield strength: 0.0034641.

Specify tabular values ​​for "Stress(Strain) curve":

Double click to enter the value and go to the table task

Specify that the tabular dependence will be on plastic deformation and press to get 6 lines. Enter values:

• Strain: 0.      Value: 0.00148461;

• Strain: 0.3.   Value: 0.00185;

• Strain: 0.6.   Value: 0.00205;

• Strain: 0.9.   Value: 0.00215.

• Strain: 1.2.   Value: 0.0022;

• Strain: 1.5.   Value: 0.00222.

Click Ok.

Click Apply.

Close the Materials management window.

2. Create a block for the model.

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): 1.

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;

• Coordinate System: Global Cartesian;

• Order: 3.

Click Apply.

Setting boundary conditions

1. Fix the model in displacements in x-axis.

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): 1;

• Degrees of Freedom: X-Translation Disp;

• DOF Value: 0.

Click Apply.

2. Fix the model in displacements in y-axis.

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): 4;

• Degrees of Freedom: Y-Translation Disp;

• DOF Value: 0.

Click Apply.

3. Fix the model in displacements in z-axis.

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;

• Degrees of Freedom: Z-Translation Disp;

• DOF Value: 0.

Click Apply.

4. Set gravity.

On the command panel, select the boundary conditions module (Mode - Boundary Conditions, Entity — Gravity, Action - Create).

Set the following parameters:

• Entity List: Volume;

• Entity ID(s): 1.

Click Apply.

5. Set the formula for the distribution of gravity.

On the command panel, select the module for specifying Dependency BC (Mode - BC Dependency).

Click on gravity and select the Y component. Then in the "Formula" column, enter the formula by which the distribution will go. Enter '-0.3 * t'.

Click Apply.

Starting calculation

1. Set the type of problem you want to solve.

On the command bar, select the calculation settings module (Mode — Calculation Settings, Calculation Settings — Transient Analysis, Transient Analysis — General).

Set the following calculation parameters:

• Dimensions: 3D;

• Method: Full solution;

• Scheme: Implict;

• Max time: 2.0;

• Time step: 0.01;

• Model: Elasticity;

• Model: Plasticity;

• Set nonlinear solver options;

• Start load substeps: 11;

• Min load substeps: 10;

• Max load substeps: 30;

• Max iterations: 50;

• Tolerance: 1e-6;

• Target iterations: 5.

Click Apply.

Click Start Calculation.

2. In the window that appears, select the directory where 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".

Results analysis

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 drop-down list, select Displacement, from the second - Magnitude.

Select a point on the surface with the Select Points  .

3. Display a displacement plot.

On the command bar, choose Filters - Alphabetical - Plot Selection Over Time.

In properties, click Apply.

4. From the first drop-down list, select Plastic Strain deformations, from the second - Mises.

Select a point on the surface with the Select Points  .

5. Display a plot of plastic strain.

On the command bar, choose Filters - Alphabetical - Plot Selection Over Time.

In properties, click Apply.

6. From the first drop-down list, select Stress, from the second, Mises.

Select a point on the surface with the Select Points  

7. Display the stress graph.

On the command bar, choose Filters - Alphabetical - Plot Selection Over Time.

In properties, click Apply.

Using Console Interface

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.

cone_slump