Home / Examples / Stress Analysis [Galileo] / Example 28: Contact Analysis with Large Deformation

Example 28: Contact Analysis with Large Deformation

General

• A round-head stick in contact with a concave face. The stick is subjected to the large deformation. The deformation is analyzed.
   

• 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.

 

Analysis Space

Item	Settings
Analysis Space	2D
Model Unit	mm

 

Analysis Conditions

[Large Displacement] is selected for the [Large Deformation].
[Large Displacement] is more suitable than [Large Strain] for this model.

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

 

The nonlinear analysis is set up on the Step/Thermal Load tab as follows.

Number of Substeps is set to 40, which is larger than the default setting of 20 because the stick exhibits a large deformation and the contact point changes drastically.

As Save results of substeps is selected, states at intermediate substeps through the final step will be saved.

Tab	Setting Item	Settings
Step/Thermal Load	Step/Reached Temperature Setting	Substeps of Step 1 : 40
	Options for the Nonlinear Analysis	Save the results of substeps : Select

Model

This model consists of two bodies: BA1 and BA2. They have the same body attributes and material properties.

The mesh size of contact surfaces is set to 0.3 [mm], which is smaller than general mesh size of 0.9 [mm].

Body Attributes and Materials

Body Number/Type	Body Attribute Name	Material Name
2/Sheet	BA1	M1
7/Sheet	BA1	M1

 

The material properties are set up as follows:

Material Name	Tab	Properties
M1	Elasticity	Young's Modulus: 1×109 [Pa] Poisson's Ratio: 0.3

Boundary Conditions

On the left end of the stick, the forced displacement of 4.5 [mm] is applied in the right direction (positive x direction).

The bottom of the target with a concave face is fixed completely.

Boundary Condition Name/Topology	Tab	Boundary Condition Type	Settings
Fix_x/Edge	Mechanical	Displacement	Select the XZ component. UX=0, UZ=0
MOVE/Edge	Mechanical	Displacement	Select the XZ component. UX = 4.5 x 10-3 [m] UZ = 0.0 x 10-3 [m]
Contactor/Edge	Mechanical	Contact Surface	Select [Contactor surface].
Target/Edge	Mechanical	Contact Surface	Select [Contactee surface].

The contactor and contactee surfaces are designated as a contact pair in the [Boundary Pair] dialog. In contact analyses, the contact surfaces must be designated as a boundary pair.

Results

The displacement and the stress distribution at the step 0.2 (corresponding to the displacement of 0.9 [mm] in X direction of MOVE) are shown below.

The round head of the stick slides on the concave surface of the target.

 

The displacement and the stress distribution at the step 0.4 (corresponding to the displacement of 1.8 [mm] in X direction of MOVE) are shown below.

The head reaches the upper end of the concave surface.

 

The displacement and the stress distribution at the step 0.7 (corresponding to the displacement of 3.15 [mm] in X direction of MOVE) are shown below.

The head starts to rotate. The stick exhibits the large deformation and the target deforms as well.

 

The displacement and the stress distribution at the step 1 (corresponding to the displacement of 4.5 [mm] in X direction of MOVE) are shown below.

The stick and target body deformed further. Compared with the state at step 0.4, the contact point moved further upward.

 

On the [Show Results] tab, go to



and click [Create Animation]. The animation file (.avi) will be created using the displayed results.

The animation gives you an intuitive visual understanding of the large deformation.