PDF
Connecting Shells and Beams
Introduction
Many engineering structures consist of thin and slender components, where a full solid model results in many extremely small elements. For such structures, the number of degrees of freedom can be reduced by orders of magnitude if shell or beam elements are used instead.
In this tutorial and verification problem, you learn how to connect beam and shell elements in different situations. The results are also compared to a solid model of the same geometry.
Model Definition
The solid geometry is shown in Figure 1. The plate is shown in green, the longitudinal stiffeners in red, the H-section beam in yellow, and the central beam in blue.
Figure 1: The solid geometry
The corresponding shell and beam representation is shown in Figure 2. Note that the two longitudinal beams are modeled using different methods. On one side, the actual centerline of the beam is created below the plate, whereas on the other side the beam is sharing the edge of the shell boundary. In the latter case, the true position of the beam is entered as an offset property. There are also two connections from points on the beams: One to the boundary and one to the edge of the shell.
Figure 2: The shell and beam geometry
GEOMETRY
•
Plate dimensions: 2.0 m x 0.4 m
•
Plate thickness: 10 mm
•
Cross section of longitudinal stiffeners: 40 x 30 mm
•
Cross section of vertical H-section beam: 70 x 60 mm with 8 mm thickness in web and flanges.
•
Cross section of central beam: 50 x 10 mm
Material
The material is Structural Steel from the material library, having the following data
•
Young’s modulus, E = 200 GPa
•
Poisson’s ratio, ν = 0.33
Constraints
The end section of the plate is fixed.
Load
•
A uniform pressure of 5 kPa is applied to the top of the plate.
•
At the top of the H-section beam, 500 N is applied as force in the positive X direction
•
At the end of the central beam, 50 N is applied as force in the negative Z direction.
Results and Discussion
The number of degrees of freedom in the solid model is 270000, whereas the number of degrees of freedom in the shell and beam model is 18000. Still, the solid model can be considered to be somewhat coarse, since there is only one element in the thickness direction of the thin parts. Creating a better mesh on the solid would require quite some effort, if the number of degrees of freedom should not increase by another order of magnitude. The potential gains in model size are thus large for the types of structures where shell or beam modeling can be used.
The von Mises stress in the solid model is compared to the results from the shell and beam model in Figure 3. The correspondence between the results is very good.
Figure 3: Stress distribution in the solid model and the shell-beam model
In Figure 4, the stress along the longitudinal stiffeners is compared between the solid model and the beam. In the solid, the outermost edge has been selected, since that is where the highest stresses occur. The equivalent stress in the beam is always computed at the worst position in the cross section.
Again, the correspondence is very good. The comparison between the results in the beams on the two sides of the plate is especially interesting. On the side where the beam shares the edge with the shell, the mesh on the beam automatically matches that on the shell. This is not the case on the other side. There is no difference in quality between the results.
Figure 4: Comparison of the stress along the stiffeners
Notes About the COMSOL Implementation
The built-in Shell-Beam Connection multiphysics coupling is used to connect the Shell and Beam interfaces.
All possible types of connections between shells and beams are displayed in this model:
•
The longitudinal stiffening beams are connected to the long edges of the plate. Two different modeling possibilities are used. On one side, there is a separate edge at the center of the beam (Figure 6), whereas on the other side, the edge of the shell is also used for the beam (Figure 5), and the actual location of the beam is specified using the offset property in the settings for Shell-Beam Connection.
•
The H-section beam is perpendicular to the plate (Figure 7). The endpoint of it is connected to a representative region on the shell surface, using a Boolean expression that is a function of the coordinates. This expression makes the connection act on a 70 x 60 mm rectangular area centered around the end of the beam. You could easily modify that expression so that only the actual H-shape is connected, possibly allowing for a weld thickness. Another option could be use a pure distance criterion, where a circle with a given diameter is connected.
•
The central beam is modeled as a beam only for instructional purposes. In practice it would be simpler to treat it as an extension of the plate. This beam has its endpoint connected to the edge of the shell (Figure 8). The part of the edge which is connected is selected as the width of the beam.
Figure 5: Longitudinal shell-beam connection with common edge
Figure 6: Longitudinal shell-beam connection with separate edge
Figure 7: Shell-beam connection with beam normal to the shell
Figure 8: Shell-beam connection where the beam is an extension of the shell
Application Library path: Structural_Mechanics_Module/Beams_and_Shells/shell_beam_connection
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  3D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
In the Select Physics tree, select Structural Mechanics>Shell (shell).
5
Click Add.
6
In the Select Physics tree, select Structural Mechanics>Beam (beam).
7
Click Add.
8
Click  Study.
9
In the Select Study tree, select General Studies>Stationary.
10
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file shell_beam_connection_parameters.txt.
The following section provides the step-by-step instructions to create the geometry from scratch. If you do not want to build the geometry yourself you can load the geometry sequence from the stored model. In the Model Builder window, under Component 1 (comp1) right-click Geometry 1 and choose Insert Sequence. Browse to the model’s Application Libraries folder and double-click the file shell_beam_connection.mph. Note that if you load the geometry sequence, all parameters used for defining the geometry will be duplicated with slightly modified names to avoid ambiguities.
You can then move on to the instruction after the geometry plot below and start with specifying the materials for the various components.
Geometry 1
To build the geometry from scratch, continue here. Start by building the solid geometry.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type lp.
4
In the Depth text field, type wp.
5
In the Height text field, type tp.
Block 2 (blk2)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type lp.
4
In the Depth text field, type wbl.
5
In the Height text field, type hbl.
6
Locate the Position section. In the z text field, type -hbl.
7
Click  Build All Objects.
Block 3 (blk3)
1
Right-click Block 2 (blk2) and choose Duplicate.
2
In the Settings window for Block, locate the Position section.
3
In the y text field, type wp-wbl.
4
Click  Build All Objects.
Block 4 (blk4)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type lbc.
4
In the Depth text field, type wbc.
5
In the Height text field, type tp.
6
Locate the Position section. In the x text field, type lp.
7
In the y text field, type (wp-wbc)/2.
8
Click  Build All Objects.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
In the z-coordinate text field, type tp.
4
Click  Show Work Plane.
Work Plane 1 (wp1)>Plane Geometry
Click the  Zoom Extents button in the Graphics toolbar.
Work Plane 1 (wp1)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type hbh-2*tbh.
4
In the Height text field, type tbh.
5
Locate the Position section. From the Base list, choose Center.
6
In the xw text field, type lp/2.
7
In the yw text field, type wp/2.
8
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Rectangle 2 (r2)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type tbh.
4
In the Height text field, type wbh.
5
Locate the Position section. From the Base list, choose Center.
6
In the xw text field, type lp/2-hbh/2+tbh/2.
7
In the yw text field, type wp/2.
8
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Rectangle 3 (r3)
1
Right-click Component 1 (comp1)>Geometry 1>Work Plane 1 (wp1)>Plane Geometry>Rectangle 2 (r2) and choose Duplicate.
2
In the Settings window for Rectangle, locate the Position section.
3
In the xw text field, type lp/2+hbh/2-tbh/2.
4
In the Work Plane toolbar, click  Build All.
Extrude 1 (ext1)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 right-click Work Plane 1 (wp1) and choose Extrude.
2
In the Settings window for Extrude, locate the Distances section.
3
In the table, enter the following settings:
Distances (m)
lbh
4
Click  Build All Objects.
Move the solid, and then create the shell-beam structure.
Move 1 (mov1)
1
In the Geometry toolbar, click  Transforms and choose Move.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Move, locate the Displacement section.
4
In the y text field, type wp*1.5.
5
Click  Build Selected.
Work Plane 2 (wp2)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Show Work Plane.
Work Plane 2 (wp2)>Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 2 (wp2)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type lp.
4
In the Height text field, type wp.
5
Click the  Zoom Extents button in the Graphics toolbar.
Polygon 1 (pol1)
1
In the Model Builder window, right-click Geometry 1 and choose More Primitives>Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
In the table, enter the following settings:
x (m)
y (m)
z (m)
lp
wp/2
0
lp+lbc
wp/2
0
4
Click  Build Selected.
Polygon 2 (pol2)
1
In the Geometry toolbar, click  More Primitives and choose Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
In the table, enter the following settings:
x (m)
y (m)
z (m)
0
wp-wbl/2
-(tp+hbl)/2
lp
wp-wbl/2
-(tp+hbl)/2
4
Click  Build Selected.
Polygon 3 (pol3)
1
In the Geometry toolbar, click  More Primitives and choose Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
In the table, enter the following settings:
x (m)
y (m)
z (m)
lp/2
wp/2
0
lp/2
wp/2
lbh+tp/2
4
Click  Build Selected.
Shell
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Shell in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
On the object wp2, select Boundary 1 only.
H-Beam
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type H-Beam in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Edge.
4
On the object pol3, select Edge 1 only.
It might be easier to select the correct edge by using the Selection List window. To open this window, in the Home toolbar click Windows and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
5
Locate the Resulting Selection section. Find the Cumulative selection subsection. Click New.
6
In the New Cumulative Selection dialog box, type Beam in the Name text field.
7
Click OK.
Stiffeners
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Stiffeners in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Edge.
4
On the object pol2, select Edge 1 only.
5
On the object wp2, select Edge 1 only.
6
Locate the Resulting Selection section. Find the Cumulative selection subsection. From the Contribute to list, choose Beam.
ProtrudingBeam
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type ProtrudingBeam in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Edge.
4
On the object pol1, select Edge 1 only.
5
Locate the Resulting Selection section. Find the Cumulative selection subsection. From the Contribute to list, choose Beam.
6
Click the  Zoom Extents button in the Graphics toolbar.
This concludes the geometry modeling.
Continue after reading geometry sequence
If you loaded the geometry sequence from file, continue here.
Add material to domains, boundaries, and edges since there are physics interfaces active in each of these dimensions.
Since the same material is applicable to all the physics, you first add the Structural Steel as a global material and subsequently use material links at the domain, boundary and edge levels.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>Structural steel.
4
Click the right end of the Add to Component split button in the window toolbar.
5
From the menu, choose Add to Global Materials.
6
In the Home toolbar, click  Add Material to close the Add Material window.
Materials
Material Link 1 (matlnk1)
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose More Materials>Material Link.
Material Link 2 (matlnk2)
1
Right-click Materials and choose More Materials>Material Link.
2
In the Settings window for Material Link, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Shell.
Material Link 3 (matlnk3)
1
Right-click Materials and choose More Materials>Material Link.
2
In the Settings window for Material Link, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Edge.
4
From the Selection list, choose Beam.
Add physics settings for the Solid Mechanics interface.
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Fixed Constraint.
2
Select Boundaries 2, 5, and 11 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 20, 26, and 32 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Total force.
5
Specify the Ftot vector as
Fh
x
0
y
0
z
Boundary Load 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 46 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Total force.
5
Specify the Ftot vector as
0
x
0
y
-Fc
z
Boundary Load 3
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 8 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0
x
0
y
-p
z
Add physics settings for the Shell interface.
Shell (shell)
1
In the Model Builder window, under Component 1 (comp1) click Shell (shell).
2
In the Settings window for Shell, locate the Boundary Selection section.
3
Click  Clear Selection.
4
From the Selection list, choose Shell.
Thickness and Offset 1
1
In the Model Builder window, under Component 1 (comp1)>Shell (shell) click Thickness and Offset 1.
2
In the Settings window for Thickness and Offset, locate the Thickness and Offset section.
3
In the d text field, type tp.
Fixed Constraint 1
1
In the Physics toolbar, click  Edges and choose Fixed Constraint.
2
Select Edge 1 only.
Face Load 1
1
In the Physics toolbar, click  Boundaries and choose Face Load.
2
In the Settings window for Face Load, locate the Boundary Selection section.
3
From the Selection list, choose Shell.
4
Locate the Force section. Specify the FA vector as
0
x
0
y
-p
z
Add physics settings for the Beam interface.
Beam (beam)
1
In the Model Builder window, under Component 1 (comp1) click Beam (beam).
2
In the Settings window for Beam, locate the Edge Selection section.
3
Click  Clear Selection.
4
From the Selection list, choose Beam.
Cross-Section Data 1
1
In the Model Builder window, under Component 1 (comp1)>Beam (beam) click Cross-Section Data 1.
2
In the Settings window for Cross-Section Data, locate the Cross-Section Definition section.
3
From the list, choose Common sections.
4
In the hy text field, type hbl.
5
In the hz text field, type wbl.
Section Orientation 1
1
In the Model Builder window, click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
0
X
0
Y
1
Z
Cross-Section Data 2
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
In the Settings window for Cross-Section Data, locate the Edge Selection section.
3
From the Selection list, choose H-Beam.
4
Locate the Cross-Section Definition section. From the list, choose Common sections.
5
From the Section type list, choose H-profile.
6
In the hy text field, type hbh.
7
In the hz text field, type wbh.
8
In the ty text field, type tbh.
9
In the tz text field, type tbh.
Section Orientation 1
1
In the Model Builder window, expand the Cross-Section Data 2 node, then click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
1
X
0
Y
0
Z
Cross-Section Data 3
1
In the Physics toolbar, click  Edges and choose Cross-Section Data.
2
In the Settings window for Cross-Section Data, locate the Edge Selection section.
3
From the Selection list, choose ProtrudingBeam.
4
Locate the Cross-Section Definition section. From the list, choose Common sections.
5
In the hy text field, type tp.
6
In the hz text field, type wbc.
Section Orientation 1
1
In the Model Builder window, expand the Cross-Section Data 3 node, then click Section Orientation 1.
2
In the Settings window for Section Orientation, locate the Section Orientation section.
3
From the Orientation method list, choose Orientation vector.
4
Specify the V vector as
0
X
0
Y
1
Z
Point Load 1
1
In the Physics toolbar, click  Points and choose Point Load.
2
Select Point 27 only.
3
In the Settings window for Point Load, locate the Force section.
4
Specify the FP vector as
Fh
x
0
y
0
z
Point Load 2
1
In the Physics toolbar, click  Points and choose Point Load.
2
Select Point 58 only.
3
In the Settings window for Point Load, locate the Force section.
4
Specify the FP vector as
0
x
0
y
-Fc
z
5
Click the  Zoom Extents button in the Graphics toolbar.
Add the couplings between the beams and the shell.
Multiphysics
Shell-Beam Connection 1 (shbc1)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
From the Connection type list, choose Shared edges.
4
Select the Manual control of selections check box.
5
Locate the Edge Selection section. Click  Clear Selection.
6
Select Edge 2 only.
7
Locate the Connection Settings section. From the Offset definition list, choose Offset vector.
8
Specify the d0 vector as
0
X
wbl/2
Y
-(tp+hbl)/2
Z
The edge selection should be like in Figure 6.
Shell-Beam Connection 2 (shbc2)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
From the Connection type list, choose Parallel edges.
4
Locate the Edge Selection, Shell section. Select the  Activate Selection toggle button.
5
Select Edge 4 only.
6
Locate the Edge Selection, Beam section. Select the  Activate Selection toggle button.
7
Select Edge 3 only.
8
Clear the  Activate Selection toggle button.
9
Click the  Wireframe Rendering button in the Graphics toolbar.
The selection should be like in Figure 5.
10
Click the  Wireframe Rendering button in the Graphics toolbar.
Shell-Beam Connection 3 (shbc3)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
From the Connection type list, choose Shell boundaries to beam points.
4
Select the Manual control of selections check box.
5
Locate the Boundary Selection, Shell section. Select the  Activate Selection toggle button.
6
Select Boundary 1 only.
7
Locate the Point Selection, Beam section. Select the  Activate Selection toggle button.
8
Select Point 26 only.
9
Clear the  Activate Selection toggle button.
You should get the same selection as in Figure 7.
10
Locate the Connection Settings section. From the Connected region list, choose Connection criterion.
11
In the text field, type (abs(x-lp/2)<hbh/2)*(abs(y-wp/2)<wbh/2).
Shell-Beam Connection 4 (shbc4)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Global>Shell-Beam Connection.
2
In the Settings window for Shell-Beam Connection, locate the Connection Settings section.
3
Select the Manual control of selections check box.
4
Locate the Edge Selection, Shell section. Click  Clear Selection.
5
Select Edges 68 and 69 only.
6
Locate the Point Selection, Beam section. Select the  Activate Selection toggle button.
7
Click  Clear Selection.
8
Select Point 41 only.
9
Clear the  Activate Selection toggle button.
The edge and point selection should be the same as in Figure 8.
10
Locate the Connection Settings section. From the Connected region list, choose Distance (Manual).
11
In the rc text field, type wbc/2.
Mesh 1
Edge 1
1
In the Mesh toolbar, click  Boundary and choose Edge.
2
Select Edges 2, 3, 68, and 69 only.
Distribution 1
1
Right-click Edge 1 and choose Distribution.
2
Select Edges 2 and 3 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 30.
Size 1
1
In the Model Builder window, right-click Edge 1 and choose Size.
2
Select Edges 68 and 69 only.
3
In the Settings window for Size, locate the Element Size section.
4
Click the Custom button.
5
Locate the Element Size Parameters section. Select the Maximum element size check box.
6
In the associated text field, type wbc/2.
Free Triangular 1
1
In the Mesh toolbar, click  Boundary and choose Free Triangular.
2
Select Boundary 1 only.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Point.
4
Select Point 26 only.
5
Locate the Element Size section. Click the Custom button.
6
Locate the Element Size Parameters section. Select the Maximum element size check box.
7
In the associated text field, type hbh/10.
8
Select the Maximum element growth rate check box.
9
In the associated text field, type 1.1.
Size 2
1
In the Model Builder window, right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
4
Click  Build Selected.
Free Tetrahedral 1
In the Mesh toolbar, click  Free Tetrahedral.
Size 1
1
Right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Finer.
4
Click  Build All.
The different structural mechanics interfaces should always be solved together. Replace the default segregated solver with a fully coupled solver.
Study 1
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 node.
4
Right-click Study 1>Solver Configurations>Solution 1 (sol1)>Stationary Solver 1 and choose Fully Coupled.
5
In the Study toolbar, click  Compute.
Results
Stress (solid)
Each physics interface will provide its own default plots. Here, you will compare all the results in one plot.
Surface 1
1
In the Model Builder window, expand the Stress (solid) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose MPa.
Surface 1
1
In the Model Builder window, expand the Results>Stress (shell) node.
2
Right-click Surface 1 and choose Copy.
Surface 2
1
In the Model Builder window, right-click Stress (solid) and choose Paste Surface.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose MPa.
4
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
Line 1
1
In the Model Builder window, expand the Results>Stress (beam) node.
2
Right-click Line 1 and choose Copy.
Line 1
1
In the Model Builder window, right-click Stress (solid) and choose Paste Line.
2
In the Settings window for Line, locate the Expression section.
3
From the Unit list, choose MPa.
4
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
Definitions
View 1
1
In the Model Builder window, expand the Component 1 (comp1)>Definitions node, then click View 1.
2
In the Settings window for View, locate the View section.
3
Clear the Show grid check box.
Results
Stress
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type Stress in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Manual.
4
In the Title text area, type von Mises stress (MPa) .
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Stress toolbar, click  Plot.
Stress comparison
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Stress comparison in the Label text field.
Line Graph 1
1
Right-click Stress comparison and choose Line Graph.
2
Select Edge 7 only.
3
In the Settings window for Line Graph, locate the y-Axis Data section.
4
In the Expression text field, type solid.mises.
5
From the Unit list, choose MPa.
6
Click to expand the Legends section. Select the Show legends check box.
7
From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
Solid
Line Graph 2
1
In the Model Builder window, right-click Stress comparison and choose Line Graph.
2
Select Edge 3 only.
3
In the Settings window for Line Graph, locate the y-Axis Data section.
4
In the Expression text field, type beam.mises.
5
From the Unit list, choose MPa.
6
Click to expand the Quality section. From the Resolution list, choose No refinement.
7
Locate the Legends section. Select the Show legends check box.
8
From the Legends list, choose Manual.
9
In the table, enter the following settings:
Legends
Beam at centerline
Line Graph 3
1
Right-click Line Graph 2 and choose Duplicate.
2
In the Settings window for Line Graph, locate the Selection section.
3
Click  Clear Selection.
4
Select Edge 2 only.
5
Locate the Legends section. In the table, enter the following settings:
Legends
Beam at shell edge
6
In the Stress comparison toolbar, click  Plot.