A Step-by-step Example to Demonstrate the Zeroing of Stresses When Changing Material at a Certain Step

Problem Description

We consider stepwise plate stretching. A round inclusion is made in the plate from the main material (i.e. the material is the same throughout the plate). The problem is solved in 2 steps of loading. At the first step, the plate undergoes uniaxial tension along the x axis,in the second step, the load is removed and the material is replaced for inclusion in such a way that Young's modulus and Poisson's ratio remain the same, but zero initial stresses are set. Stresses around the inclusion at the last loading step are analyzed.

Geometry creation

1. Create a plate with a side of 100.

On the command panel, select the mode for creating volume geometry (Mode — Geometry, Entity — Surface, Action — Create).

From the list of geometric primitives, select Rectangle.

Set the following parameters:

Width: 100.

Click Apply.

2. Create a circle with a radius 10.

On the command panel, select the mode for creating volume geometry (Mode — Geometry, Entity — Surface, Action — Create).

From the list of geometric primitives, select Circle.

Set the following parameters:

Radius: 10;
Select Z-plane.

Click Apply.

3. Cut the circle out of the plate while keeping the originals (Save In).

On the command panel, select the mode for creating volume geometry (Mode — Geometry, Entity — Surface, Action — Logical operations).

From the list of logical operations, select Subtract.

Set the following parameters:

А - Surface ID: 1;
В - Surface ID: 2;
Save В.

Click Apply.

4. Merge geometry.

On the command panel, select the mode for creating volume geometry (Mode — Geometry, Entity — Surface, Action — Print/Splice).

From the list of actions, select Print and Splice.

Set the following parameters:

Surface ID: all

Click Apply.

Meshing

On the command panel, select the curve meshing mode (Mode - Mesh, Entity - Surface, Action - Intervals).

Set the following parameters:

Automatic size;
Select Surfaces: all.

Click Build Mesh.

Specifying the material

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

Create two materials.

material 1:

Young's modulus Е = 210000;
Poisson's ratio ν = 0.3.

material 2:

Young's modulus Е = 210000;
Poisson's ratio ν = 0.3.

Click Apply.

Specifying the block properties

1. Create a block of one material type.

On the command panel, select the mode for setting material properties (Mode — Blocks, Object — Block,Action — Add entity to the block .

Set the following parameters:

Block ID:: 1;
Entity List: Surface;
Object(s)ID: 3.

Click Apply.

2. Create the second block.

On the command panel, select the mode for setting material properties (Mode — Blocks, Object — Block,Action — Add entity to the block.

Set the following parameters:

Block ID: 2;
Entity List: Surface;
Object(s)ID: 2.

Click Apply.

3. Set parameters for blocks 1 and 2.

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

Set the following parameters:

Block (s) ID: all;
Material: material 1;
Coordinate system: Global Cartesian;
Category: Plane;
Order: 2.

Click Apply.

Setting boundary conditions

1. Fix the right and left sides according to the symmetry condition along the X axis. On the command panel, select Mode — Boundary Conditions, Entity — Displacement, Action — Create.

Set the following parameters:

System Assigned ID;;
Entity List: Curve;
Entity ID(s): 2 4;
Degrees of freedom: Х;
Value: 0.

Click Apply.

2. Fix some knot in the center of the plate along all degrees of freedom. On the command panel, select Mode — Boundary Conditions, Entity — Displacement, Action — Create.

Set the following parameters:

System Assigned ID;;
Entity List: Curve;
Entity ID(s): 3 5;

Degrees of freedom: All;
Value: 0.

Click Apply.

3. Set the pressure to 100 MPa (tensile) on the top and bottom faces.

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

Set the following parameters:

System Assigned ID;;
Entity List: Surface;

Entity ID(s): 1 3;
Value: 100.

Click Apply.

Starting calculation

1. Set the type of problem you want to solve. On the command panel, select the calculation settings mode (Mode - Calculation Settings, Calculation Settings — Static, Static — General).

Select:

Dimension: 2D;
Type of plane problem: plane strain;
Model: Elasticity;
Number of loading steps: 2.

2. Specify the number of loading steps for pressure 1.

3.Change the material in the second step to material 2.

Click Apply.

Click Start calculation.

4. In the window that appears, select the directory in which the result will be saved and enter the file name.

5.In case of a successful calculation, the console will display a 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 → Results. Click Open the last result.
Select Results on Command Panel (Mode - Results). Click Open last result)

2. Display the Stress field on a surface with ribs.

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

Display type: Surface with ribs;
Display field: Displacement;
Display Component: Voltages.

The model displays a voltage distribution box.

Step 1

Step 2

At the last step of the solution for the deformed view, the plate returned to its original

condition, and the cutout remained elliptical.

For comparison, a solution without zero initial stresses for the second material is shown.:

Step 1

Step 2

Using the console interface

Geometry creating, meshing, setting boundary conditions and materials can be performed using the console interface. Below is the program code that allows you to perform the steps of the above manual, you only need to specify the full path and name of the saved file.

reset
create surface rectangle width 100 zplane
create surface circle radius 10 zplane
subtract surface 2 from surface 1  keep_tool
merge all
surface all size auto factor 1
undo group begin
surface all size auto factor 1
mesh surface all
undo group end
create material 1
modify material 1 name 'material 1'
create material 2
modify material 2 name 'material 2'
modify material 1 set property 'MODULUS' value 210000
modify material 1 set property 'POISSON' value 0.3
modify material 2 set property 'MODULUS' value 210000
modify material 2 set property 'POISSON' value 0.3
modify material 2 set property 'INIT_STRESS_XZ' value 0
modify material 2 set property 'INIT_STRESS_YZ' value 0
modify material 2 set property 'INIT_STRESS_XY' value 0
modify material 2 set property 'INIT_STRESS_ZZ' value 0
modify material 2 set property 'INIT_STRESS_YY' value 0
modify material 2 set property 'INIT_STRESS_XX' value 0
set duplicate block elements off
block 1 add surface 3 
set duplicate block elements off
block 2 add surface 2 
block all material 1 cs 1 element plane order 2
create displacement  on curve 4 2  dof 1 fix  
create displacement  on node 53  dof all fix  
static steps 2
block 2 step 2 material 2
create pressure  on curve 1 3  magnitude -100 
bcdep pressure 1 step 1
analysis type static elasticity dim2 planestrain