Non-axisymmetric disc loading with periodic boundary condition in Fidesys

In this example, we consider the loading of a disk segment subjected to a force effect on the outer parallelepiped elements that simulate blades. The disc is fixed to the inner diameter.

We consider a part of the disc. The problem is solved using periodic boundary conditions.

Geometry creating

1. Create the first circular cylinder.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action - Create).

Select Cylinder from the list of geometric primitives. Set the following parameters:

  • Height: 1;

  • Section type: Circular;

  • Radius: 10.

Click Apply.

2. Create the second circular cylinder.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action - Create).

Select Cylinder from the list of geometric primitives. Set the following parameters:

  • Height: 1;

  • Section type: Circular;

  • Radius: 1.

Click Apply.

3. Subtract the second cylinder from the first.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Boolean).

From the list of operations, select Subtract. Set the following parameters:

  • Body ID: 1 (volumes from which other volumes will be subtracted);

  • Subtract solids (ID): 2 (volumes to be subtracted).

Click Apply.

4. Leave the segment.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Webcut).

Select Coordinate Plane from the list of available section views.

Set the following parameters:

  • Volume ID(s): 1;

  • Cut: Plane ZX;

  • Offset Value: 0;

  • Rotate Plane;

  • Angle: 15;

  • Direction: Z Axis;

  • Center X, Y, Z: 0 0 0.

Click Apply.

Do the same for the other angle.

  • Volume ID(s): 1;

  • Cut: Plane ZX;

  • Offset Value: 0;

  • Rotate Plane;

  • Angle: -15;

  • Direction: Z Axis;

  • Center X, Y, Z: 0 0 0.

Click Apply.

5. Remove volumes 1 and 3. To do this, while holding down the Ctrl key, select these volumes in the object tree and click Delete in the context menu.

6.Create a parallelepiped.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action - Create).

Select Brick from the list of geometric primitives. Set the following parameters:

  • X (width): 4;

  • Y (height): 3;

  • Z (depth): 1.

Click Apply.

7. Rotate the parallelepiped.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Transform).

From the list of operations, select Rotate. Set the following parameters:

  • Volume ID(s): 5;

  • Include Merged;

  • Angle: 90;

  • Rotate About: X-axis.

Click Apply.

8. Move the parallelepiped.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Transform).

From the list of operations, select Move. Set the following parameters:

  • Volume ID(s): 5;

  • Include Merged;

  • Select Method: Distance;

  • X Distance: 11.

Click Apply.

9. Cut the parallelepiped.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Webcut).

From the list of available section views, select Plane From Surface.

Set the following parameters:

  • Volume ID(s): 5;

  • Plane From Surface ID: 31.

Click Apply.

Do the same for the other surface.

  • Volume ID(s): 6;

  • Plane From Surface ID: 29.

Click Apply.

10. Delete volumes 6 and 5. To do this, hold down the Ctrl key, select these volumes in the object tree and click Delete in the context menu.

11. Merge the remaining volumes.

On the command panel select a module for constructing solid geometry (Mode - Geometry, Entity - Volume, Action — Boolean).

From the list of operations, select Intersect. Set the following parameters:

  • Volume ID(s): 4 7.

Click Apply.

Meshing

1. On the command panel, select a module for generating a volumetric mesh (Mode - Mesh, Entity - Volume, Action - Intervals).

Set the following parameters:

  • Select Volumes: 4;

  • Automatic Sizing;

  • Auto Factor: 4.

Click Apply Size.

2. On the command panel, select a module for generating a volumetric mesh (Mode - Mesh, Entity - Volume, Action — Mesh).

Set the following parameters:

  • Automatically Calculate;

  • Select Volumes: 4.

Click Apply Scheme.

Click Mesh.

Setting boundary conditions

1. Attach one side edge.

On the command panel, select Mode - Boundary Conditions, Entity — Displacement, Action - Create.

Set the following parameters:

  • System Assigned ID;

  • Entity List: Surface;

  • Entity ID(s): 30;

  • Degrees Of Freedom: X-Translation Disp, Y-Translation Disp, Z-Translation Disp;

  • DOF Value: 0.

Click Apply.

2. Apply pressure.

On the command panel, select Mode - Boundary Conditions, Entity — Pressure, Action - Create.

Set the following parameters:

  • System Assigned ID;

  • Pressure Entity List: Surface;

  • Entity ID(s): 58;

  • Magnitude Value: 1e5.

Click Apply.

3. Set the periodic condition.

On the command panel, select Mode - Boundary Conditions, Entity — Periodic Condition, Action - Create.

Set the following parameters:

  • System Assigned ID;

  • Entity List (master entity): Surface;

  • Entity ID(s) (main entity): 27;

  • Entity List (slave entity): Surface;

  • Entity ID(s) (slave entity): 11;

  • General;

  • Coordinate System: Global Cartesian;

  • Number of sectors: 12.

Click Apply.

Setting the material and block properties

1. Create a material.

On the command panel, select the module for setting material properties (Mode - Material, Entity - Material Management).

In the Manage Materials window that opens, drag the Material Carbon Steel from the third column. Specify the name of the material and write «Steel». Press the ENTER key.

Click Apply.

2. Create a block of one material type.

On the command panel, select Mode - Blocks, Entity - Block, Action - Add.

Set the following parameters:

  • Block ID: 1;

  • Entity List: Volume;

  • Entity ID(s): 4.

Click Apply.

3. Set the block parameters.

On the command panel, select the mode for setting material properties (Mode - Blocks, Entity - Block, Action - Block properties/parameters).

Set the following parameters:

  • Block ID(s): 1;

  • Available materials: Steel;

  • Coordinate System: Global Cartesian;

  • Category: Solid;

  • Order: 1.

Click Apply.

Starting calculation

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

On the command panel, select the calculation settings module (Mode - Calculation Settings, Calculation Settings - Static, Static - General).

Select:

  • Dimension: 3D;

  • Model: Elasticity.

Click Apply.

2. Go to the settings section for Output Fields.

Put a tick Output full model (for periodic BCs).

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 case of a successful calculation, the console displays a message: “Calculation finished successfully at "date time ".

Results analysis

1. Open the file with the results. There are three ways to do it.

  • Click Ctrl+E.

  • Select Calculation - Open Results in the Main Menu. Click Open last result.

  • Select Results on Command Panel (Mode — Results). Click Open Results.

The Fidesys Viewer window will appear, in which you can view the calculation results.

Show the Displacement component.

In the Fidesys Viewer window on the toolbar, set the following parameters:

  • Display type: Surface;

  • Display field: Displacement (amount).

Display Equivalent Voltages.

  • Display type: Surface;

  • Display field: Stress (von Mises).

Using Console Interface

For geometry generation, meshing, setting boundary conditions and materials you can use Console Interface. The following program code allows performing the steps of the above-described guide, you only need to manually specify the full path and name of the file to be saved.

reset
create Cylinder height 1 radius 10
create Cylinder height 1 radius 1
subtract volume 2 from volume 1
webcut volume 1 with plane yplane offset 0 rotate 15 about z center 0 0 0
webcut volume 1 with plane yplane offset 0 rotate -15 about z center 0 0 0
delete volume 1 3
brick x 4 y 3 z 1
rotate Volume 5 angle 90 about X include_merged
move Volume 5 x 11
webcut volume 5 with plane from surface 31
webcut volume 6 with plane from surface 29
delete volume 6 5
unite volume 4 7
volume 4 size auto factor 4
mesh volume 4
create displacement on surface 30 dof 1 dof 2 dof 3 fix 0
create pressure on surface 58 magnitude 1e5
create periodic master surface 27 slave surface 11 general cs 1 sectors 12
create material 1 from 'Steel'
set duplicate block elements off
block 1 add volume 4
block 1 material 1
block 1 element solid
analysis type static elasticity dim3
output nodalforce off energy off midresults on record3d on material off fullperiodic on
calculation start path "D:\result.pvd"
И еще статьи из раздела