PDF
Tapered Cantilever with Two Load Cases
Introduction
This example, taken from a NAFEMS benchmark collection (Ref. 1), demonstrates how to apply and evaluate different boundary conditions acting on a cantilever beam.
Model Definition
The cantilever beam has a thickness of 0.1 m, width of 4 m and is 4 m on its long edge and 2 m on its short edge. Two cases are considered. In the first one a gravity load, mg, acts in the negative y direction with an acceleration of 9.81 m/s2. The left end boundary is fully fixed (no displacements). In the second case gravity load is not present and instead a uniformly distributed horizontal load, F, of 10 MN/m acts along the right end. At the left end there is no displacement in the x direction. Also at a midpoint location the left end is fixed in the y direction; see Figure 1.
Figure 1: Schematic description of two load cases.
Material Model
The model uses the following material properties:
•
The material is isotropic.
•
The Young’s modulus (elasticity modulus) is 210 GPa.
•
The Poisson ratio is 0.3.
•
The density is 7000 kg/m3.
Results and Discussion
For the gravity case shear stress is evaluated. The benchmark target value of −0.200 MPa at the point (0,  2) is in good agreement with the model results. Using the default Normal mesh size, the COMSOL Multiphysics solution gives a value of −0.199 MPa; see Figure 2.
Figure 2: In plane shear stress due to gravity load.
For the load case, the horizontal (x direction) normal stress is evaluated. The benchmark target value of 61.3 MPa at the point (0,  2) is in good agreement with the results. Using the default mesh size, the COMSOL Multiphysics solution gives a value of 61.4 MPa; see Figure 3.
Figure 3: Counteracting stress due to applied edge load.
Notes About the COMSOL Implementation
Use predefined variables for the acceleration of gravity and density to enter the gravity load as a force/volume. COMSOL then computes the load using the thickness of the geometry.
Use the Solid Mechanics interface to perform a stress analysis. The finite element model uses the default second-order triangular Lagrange elements. To show convergence toward the benchmark value, create a finer mesh.
Use the Load Group and Constraint Group features to collect conditions that are enabled in different studies. Define a group in Global Definitions and assign its content directly from the load or constraint itself. You define load cases in the Study Extensions of a Study Type and enable active load and constraint groups; see Figure 4, where lg denotes a load group and cg denotes a constraint group. Weight is used as a multiplication factor for the corresponding load group.
Figure 4: Definition of load cases.
Reference
1. D. Hitchings, A. Kamoulakos, and G.A.O. Davies, Linear Statics Benchmarks Vol. 1, NAFEMS, Glasgow, 1987.
Application Library path: COMSOL_Multiphysics/Structural_Mechanics/tapered_cantilever
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Geometry 1
Polygon 1 (pol1)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
From the Data source list, choose Vectors.
4
In the x text field, type 0 4 4 0 0.
5
In the y text field, type 0 1 3 4 0.
6
Click  Build Selected.
Point 1 (pt1)
1
In the Geometry toolbar, click  Point.
2
In the Settings window for Point, locate the Point section.
3
In the y text field, type 2.
4
Click  Build Selected.
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
210[GPa]
Pa
Basic
Poisson’s ratio
nu
0.3
1
Basic
Density
rho
7000[kg/m^3]
kg/m³
Basic
Global Definitions
Load Group Gravity
1
In the Model Builder window, right-click Global Definitions and choose Load and Constraint Groups>Load Group.
2
In the Settings window for Load Group, type Load Group Gravity in the Label text field.
3
In the Parameter name text field, type lgGravity.
Load Group Force
1
In the Model Builder window, right-click Load and Constraint Groups and choose Load Group.
2
In the Settings window for Load Group, type Load Group Force in the Label text field.
3
In the Parameter name text field, type lgForce.
Constraint Group Gravity
1
In the Model Builder window, right-click Global Definitions and choose Load and Constraint Groups>Constraint Group.
2
In the Settings window for Constraint Group, type Constraint Group Gravity in the Label text field.
3
In the Parameter name text field, type cgGravity.
Constraint Group Force
1
Right-click Global Definitions and choose Load and Constraint Groups>Constraint Group.
2
In the Settings window for Constraint Group, type Constraint Group Force in the Label text field.
3
In the Parameter name text field, type cgForce.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the 2D Approximation section.
3
From the list, choose Plane stress.
4
Locate the Thickness section. In the d text field, type 0.1.
First, define all constraints for both load cases and then assign them to different load and constraint groups.
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundaries 1 and 3 only.
3
In the Physics toolbar, click  Constraint Group and choose Constraint Group Gravity.
Body Load 1
1
In the Physics toolbar, click  Domains and choose Body Load.
2
Select Domain 1 only.
3
In the Settings window for Body Load, locate the Force section.
4
Specify the FV vector as
0
x
-g_const*solid.rho
y
5
In the Physics toolbar, click  Load Group and choose Load Group Gravity.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 1 and 3 only.
3
In the Physics toolbar, click  Constraint Group and choose Constraint Group Force.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 5 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Force per unit length.
5
Specify the FL vector as
10[MN/m]
x
0
y
6
In the Physics toolbar, click  Load Group and choose Load Group Force.
Fixed Constraint 2
1
In the Physics toolbar, click  Points and choose Fixed Constraint.
2
Select Point 2 only.
Mesh 1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Build All.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Define load cases check box.
4
Click  Add.
5
In the table, enter the following settings:
Load case
lgGravity
Weight
lgForce
Weight
cgGravity
cgForce
Gravity
√
1.0
 
1.0
√
 
6
Click  Add.
7
In the table, enter the following settings:
Load case
lgGravity
Weight
lgForce
Weight
cgGravity
cgForce
Force
 
1.0
√
1.0
 
√
The study extension for the load cases should look like Figure 4.
8
In the Home toolbar, click  Compute.
Results
Normal stress
In the Settings window for 2D Plot Group, type Normal stress in the Label text field.
Surface 1
1
In the Model Builder window, expand the Normal stress node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Stress (Gauss points)>Stress tensor, Gauss point evaluation (spatial frame) - N/m²>solid.sGpx - Stress tensor, Gauss point evaluation, x component.
3
In the Normal stress toolbar, click  Plot.
Shear stress
1
In the Model Builder window, right-click Normal stress and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Shear stress in the Label text field.
3
Locate the Data section. From the Load case list, choose Gravity.
Surface 1
1
In the Model Builder window, expand the Shear stress node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type solid.sGpxy.
4
In the Shear stress toolbar, click  Plot.
Point Evaluation - normal stress
1
In the Results toolbar, click  Point Evaluation.
2
In the Settings window for Point Evaluation, type Point Evaluation - normal stress in the Label text field.
3
Select Point 2 only.
4
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Stress (Gauss points)>Stress tensor, Gauss point evaluation (spatial frame) - N/m²>solid.sGpx - Stress tensor, Gauss point evaluation, x component.
5
Click  Evaluate.
Point Evaluation - shear stress
1
In the Results toolbar, click  Point Evaluation.
2
In the Settings window for Point Evaluation, type Point Evaluation - shear stress in the Label text field.
3
Select Point 2 only.
4
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Stress (Gauss points)>Stress tensor, Gauss point evaluation (spatial frame) - N/m²>solid.sGpxy - Stress tensor, Gauss point evaluation, xy component.
5
Click  Evaluate.