Twisting and Bending of a Metal Frame

A thin-walled frame member with a central cutout is subjected to bending and twisting. The stresses around the cutout are expected to be above the yield stress of the material.

This example demonstrates how to model plastic deformation in thin structures. The Layered Linear Elastic Material in the Shell interface is used to define the load scenario, and the Plasticity subnode to quantify the plastic deformation around the cutout. The residual stress and plastic strains after removal of the load are investigated.

Model Definition

The load carrying beam is shown in Figure 1. It has a length of 1.1 m, a thin-walled square cross section with dimensions 160 x 160 mm2 and a wall thickness of 6 mm. The cutout is centrally placed on one of the faces and is 100 mm long, 80 mm wide, and has a fillet with a radius of 10 mm in each corner.

Figure 1: Geometry of the frame member.

The loading consists of a bending moments in the y direction, and a twisting moment around the x-axis. Both loads can vary independently and are applied at the right end of the frame at x = 1.1 m. The left end, x = 0, is clamped.

The frame is made out of steel with Young’s modulus, Poisson’s ratio, and density given as E = 200 GPa, ν = 0.33, and ρ = 7800 kg/m3, respectively. Yielding of the steel is governed by a von Mises plasticity model with an initial yield stress σys0 = 355 MPa. A tangent modulus Et = 100 MPa defines the isotropic hardening behavior.

Results and Discussion

Figure 2 shows the distribution of the von Mises stress at the peak of the applied loads. The effect of the cutout on the stress field is clearly visible. Due to the applied loads, stresses on the inner side of the frame are higher than on the outside.

Figure 2: Distribution of von Mises stress in the frame at the maximum load.

Figure 3 shows the residual stress on the outer surface of the frame after removal of the applied loads. Large stresses are visible in the vicinity of the cutout.

It is possible to observe the development of plastic strains in the structure during loading. Figure 4 shows the parts of the frame where plastic deformations have occurred at the end of the loading cycle. Note that plastic strains are not uniform through the shell thickness

Figure 3: Residual stress on the outside of the frame after removal of the applied loads

Figure 4: Equivalent plastic strain in the frame at end of the loading cycle.

Notes About the COMSOL Implementation

The structure is modeled with the interface and the model. This feature enables to model phenomena that are thickness dependent, such as . The user interface is similar to what is available in the Solid Mechanics interface.

In COMSOL Multiphysics, several load types can be applied to a node. In this example, the node is used twice to apply a twisting moment around the x-axis, and a bending moment in the y direction. A piecewise function is used to ramp up the magnitude of these moments, and to remove the loads to observe the residual stress and plastic strains.

Nonlinear_Structural_Materials_Module/Plasticity/frame_with_cutout_plasticity

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

Click

In the tree, select .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
para	0	0	Parameter

Piecewise 1 (pw1)

In the toolbar, click

and choose .

In the window for , locate the section.

Find the subsection. In the table, enter the following settings:


Start	End	Function
0	1	x
1	2	2-x

Locate the section. In the text field, type 1.

In the text field, type N*m.

Geometry 1

Block 1 (blk1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 1.1.

In the text field, type 0.154.

Locate the section. From the list, choose .

Work Plane 1 (wp1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

On the object , select Boundary 3 only.

Click

Work Plane 1 (wp1)>Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 80 [mm].

In the text field, type 100 [mm].

Work Plane 1 (wp1)>Fillet 1 (fil1)

In the toolbar, click

On the object , select Points 1–4 only.

In the window for , locate the section.

In the text field, type 10 [mm].

Difference 1 (dif1)

In the window, right-click and choose .

Select the object only.

In the window for , locate the section.

Find the subsection. Select the

toggle button.

Select the object only.

Delete Entities 1 (del1)

Right-click and choose .

On the object , select Boundaries 1 and 6 only.

In the window for , click

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click

In the toolbar, click

to close the window.

Shell (shell)

Layered Linear Elastic Material 1

In the window, under right-click and choose .

In the window for , locate the section.

From the list, choose .

Plasticity 1

In the toolbar, click

and choose .

Materials

Structural steel (mat1)

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Thickness	lth	6[mm]	m	Shell
Initial yield stress	sigmags	355[MPa]	Pa	Elastoplastic material model
Isotropic tangent modulus	Et	100[MPa]	Pa	Elastoplastic material model