Home / Examples / Stress Analysis [Galileo] / Example 58: Spring Back Analysis with ON/OFF Setting

Example 58: Spring Back Analysis with ON/OFF Setting

General

Analysis is performed on a plate which is bent in 90° angle and then released.
Procedure for the release after the 90° bent is set by applying [ON/OFF] setting of the boundary condition.
Alternatively, the same results will be given by selecting [Add unloading step] with the step setting of [Single-step].
(The analysis model with the unloading setup is also included in the project file)
The elasto-plastic material is used. The plastic deformation will take place at the bending and the material will go backward to the original position in a small degree after the release.
(This nature is called spring back)
Unless specified in the list below, the default conditions will be applied.
Obtain this session's project file. (Right-click and choose 'Save link as')
Results will vary depending on Femtet version and the PC environment.
Elasto-plastic analysis is available in an optional package.

Analysis Space

Item	Settings
Analysis Space	2D
Model Unit	mm

Analysis Conditions

Select [Large displacement] in the Large Deformation as deformation of 90° is large.

Item	Settings
Solver	Stress Analysis [Galileo]
Analysis Type	Static Analysis
Large Deformation	Select [Large Displacement]

Set up as follows on the Step/Thermal Load tab.

Step 1 corresponds to Bend 90°, and Step 2 corresponds to Release (set off the constrain of rotational displacement).

Tab

Setting Item

Settings

Step/Thermal Load

Step Setting

Multiple Steps

Step/Reached Temperature Setting

Step	Substeps
1	20
2	5

Options for the Multi-Step Analysis

Select [Save the results of substeps]

The setting below is done on the High-level setting tab.

[Adjust acceleration/deceleration coefficient automatically] is not selected for this model to have faster calculation.

Tab

Item

High-Level Setting

Nonlinear Analysis

Deselect [Adjust acceleration/deceleration factor automatically]

Graphical Objects

The model is a box solid body with an edge length of 200 mm. The material is elasto-plastic.

Fix the left end in the X direction. Fix the 90mm area of the left end at its bottom in the Z direction.
The plate is bent at its center in 90-degree angle. Set the rotational displacement on the 90mm area of the right end at its top side.

Set the general mesh size at 1.

Body Attributes and Materials

Body Number/Type	Body Attribute Name	Material Name
0/Solid	PLATE	PlasticMat
1,2/Face	No Setup *1	No Setup *1

*1 Imprinting body for the boundary condition.

Material Name

Tab

Properties

PlasticMat

Elasticity

Material Type: Elasto-plastic Bilinear

Material Property:

Young's Modulus: 200x109 [Pa]

Poisson's Ratio: 0.3

Strain Hardening Rate: 20x109 [Pa]

Initial Yield Stress: 200x106 [Pa]

Boundary Conditions

Rotational displacement and ON/OFF are set.

Boundary Condition Name/Topology

Tab

Boundary Condition Type

Settings

xFix/Face

Mechanical

Displacement

Select the X component.
UX=0

zFix/Face

Mechanical

Displacement

Select the Z Component.
UZ=0

Rot/Face

Mechanical

Rotational Displacement

Coordinates on Axis:
(100, 0.0, 2)

Vectors of Axis
(0.0, 1, 0.0)

Rotation Angles
90 [deg]

Set ON/OFF

Select

ON/OFF List

Boundary Condition ON/OFF Tab

Number of Calculation Steps	Rot
1	Yes
2	No

*1) If [Weight function] tab is selected in the Time/Step Table of ON/OFF List, the loads at the substeps can be viewed.

The figure below is the view when [Show with actual loads] is selected.

The set rotational displacement will gradually reach to 90[deg] in one step.

It goes up by 4.5[deg] per substep as the number of substeps is 10.

Since OFF (No) is set on the step 2, the constrain of rotational displacement is removed from the first substep in the step 2 onward.

See [Weight Function Setting] for the details of viewing the weight function.

Results

The results of all torques are shown in the table.

The data in the table are shown in the chart below.

Torque on the boundary Rot is increasing through step 1.
It goes down to zero at the first substep of step 2 (1.2[Step]).

Right after removing the constrain, minute value is observed because the convergence judgment is a bit inaccurate.

But from the following substep onward, the torque is almost zero.

The displacement at the 1st step is shown below. The contour diagram shows the magnitude of displacement.

The 90-degree bending is observed.

The displacement at the 2nd step is shown below.

The bending angle is smaller than the step 1 because the constrain of rotational displacement is removed.
Spring back can be observed.