On October 23rd, 2014, we updated our
By continuing to use LinkedIn’s SlideShare service, you agree to the revised terms, so please take a few minutes to review them.
Nonlinear Analysis of a Skew Plate
You have been asked to model the plate shown in Figure W12–1. It is skewed 30° to the
global 1-axis, is built-in at one end, and is constrained to move on rails parallel to the
plate axis at the other end. You are to determine the midspan deflection when the plate
carries a uniform pressure. You are to perform both linear and nonlinear static and
Figure W12–1. Sketch of the skewed plate
Defining the model geometry
Start ABAQUS/CAE in the workshops/skewPlate directory, and enter the Part
module. A default model name is assigned by ABAQUS/CAE (Model-1). However,
since the linear analysis model will later form the basis of the nonlinear analysis model,
you should rename the current model to give it a more descriptive name.
· From the main menu bar, select ModelRenameModel-1. Rename the
Create a three-dimensional, deformable body with a planar shell base feature. Name the
part Plate, and specify an approximate part size of 4.0. A suggested approach to
creating the part geometry is outlined in the following procedure:
To sketch the plate geometry:
1. In the Sketcher create a vertical line of length 0.4 m using the Create Lines:
2. Using the Create Construction: Line at an Angle tool, create a construction
line oriented 30° with respect to the horizontal through each of the line’s
3. Using the Create Isolated Point tool, create an isolated point at a horizontal
distance of 1.0 m to the right of the vertical line. Create a vertical construction line
through this point.
4. Using the Create Lines: Connected tool, draw the skewed rectangle using the
preselection points at the intersections of the construction lines to position the
The final sketch is shown in Figure W12–2.
Figure W12–2. Sketch of the plate geometry
5. In the prompt area, click Done to finish the sketch.
Defining the material and section properties and the local
The plate is made of an isotropic, linear elastic material with a Young's modulus
E = 30E9 Pa and a Poisson's ratio = 0.3. Enter the Property module, and create the
material definition; name the material Steel.
The orientation of the structure in the global coordinate system is shown in
Figure W12–1. The global Cartesian coordinate system defines the default material
directions, but the plate is skewed relative to this system. It will not be easy to interpret
the results of the simulation if you use the default material directions because the direct
stress in the material 1-direction, 11 , will contain contributions from both the axial
stress, produced by the bending of the plate, and the stress transverse to the axis of the
plate. It will be easier to interpret the results if the material directions are aligned with the
axis of the plate and the transverse direction. Therefore, a local rectangular coordinate
system is needed in which the local x’-direction lies along the axis of the plate (i.e., at
30° to the global 1-axis) and the local y’-direction is also in the plane of the plate.
To define shell section properties and local material directions:
1. Define a homogeneous shell section named PlateSection. Assign a shell
thickness of 0.8E-2 and the Steel material definition to the section. Specify
that section integration be performed before the analysis since the material is
6. Define a rectangular datum coordinate system as shown in Figure W12–3 using
the Create Datum CSYS: 2 Lines tool .
Figure W12–3. Datum coordinate system used to define local material directions
7. From the main menu bar, select AssignMaterial Orientation and select the
entire part as the region to which local material directions will be applied. In the
viewport, select the datum coordinate system created earlier. Select Axis-3 for the
direction of the approximate shell normal. No additional rotation is needed about
Tip: To verify that the local material directions have been assigned correctly, select
ToolsQuery from the main menu bar and perform a property query on the material
Once the part has been meshed and elements have been created in the model, all element
variables will be defined in this local coordinate system.
8. Assign the section definition to the plate.
Creating an assembly, defining an analysis step, and specifying
Instance the plate in the Assembly module. Before leaving the Assembly module, define
geometry sets to facilitate output request and boundary condition definitions. You will
first need to partition the plate in half to create a geometry set at the plate midspan.
Select this edge to be along the
Select this edge to
be in the local x’-y’
To partition the plate and define geometry sets:
1. Partition the plate in half using the Partition Face: Shortest Path Between 2
Points tool . Use the midpoints of the skewed edges of the plate to create the
partition shown in Figure W12–4.
Figure W12–4. Partition used to define a geometry set at the plate midspan
9. Select ToolsSetCreate to create a geometry set for the midspan named
MidSpan. Similarly, create sets for the left and right edges of the plate and name
them EndA and EndB, respectively.
Next, create a single static, general step in the Step module. Name the step Apply
Pressure, and specify the following step description: Uniform pressure (20
kPa) load. Accept all the default settings for the step.
Among the output you will need are the nodal displacements and element stresses as field
data. These data will be used to create deformed shape plots and contour plots in
ABAQUS/Viewer. You will also want to write the displacements at the midspan as
history data to create X–Y plots in ABAQUS/Viewer.
To change the default output requests:
1. Edit the field output request so that only the nodal displacements and element
stresses for the whole model are written as field data to the output database
10. Edit the history output request so that only nodal displacements for the MidSpan
geometry set are written as history data to the output database file.
Prescribing boundary conditions and applied loads
As shown in Figure W12–1, the left end of the plate is completely fixed; the right end is
constrained to move on rails that are parallel to the axis of the plate. Since the latter
boundary condition direction does not coincide with the global axes, you must define a
local coordinate system that has an axis aligned with the plate. You can use the datum
coordinate system that you created earlier to define the local material directions.
To assign boundary conditions in a local coordinate system:
1. Switch to the Load module.
11. Select BCCreate, and define a Displacement/Rotation mechanical
boundary condition named Rail boundary condition in the Initial
In this example you will assign boundary conditions to sets rather than to regions selected
directly in the viewport. Thus, when prompted for the regions to which the boundary
condition will be applied, click Sets in the prompt area of the viewport.
12. From the Region Selection dialog box that appears, select set EndB. Toggle on
Highlight selections in viewport to make sure the correct set is selected. The
right edge of the plate should be highlighted. Click Continue.
13. In the Edit Boundary Condition dialog box, click Edit to specify the local
coordinate system in which the boundary condition will be applied. In the
viewport, select the datum coordinate system that was created earlier to define the
local directions. The local 1-direction is aligned with the plate axis.
14. In the Edit Boundary Condition dialog box, fix all degrees of freedom except
The right edge of the plate is now constrained to move only in the direction of the plate
axis. Once the plate has been meshed and nodes have been generated in the model, all
printed nodal output quantities associated with this region (displacements, velocities,
reaction forces, etc.) will be defined in this local coordinate system.
Complete the boundary condition definition by fixing all degrees of freedom at the left
edge of the plate (set EndA). Name this boundary condition Fix left end. Use the
default global directions for this boundary condition.
Finally, define a uniform pressure load named Pressure across the top of the shell in
the Apply Pressure step. Select both regions of the part using [Shift]+Click, and
choose the top side of the shell (Magenta) as the surface to which the pressure load will
be applied. You may need to rotate the view to more clearly distinguish the top side of the
plate. Specify a load magnitude of 2.0E4 Pa.
Creating the mesh and defining a job
Figure W12–5 shows the suggested mesh for this simulation.
Figure W12–5. Suggested mesh design for the skewed plate simulation
You must answer the following questions before selecting an element type: Is the plate
thin or thick? Are the strains small or large? The plate is quite thin, with a thickness-to-
minimum span ratio of 0.02. (The thickness is 0.8 cm, and the minimum span is 40 cm.)
While we cannot readily predict the magnitude of the strains in the structure, we think that
the strains will be small. Based on this information, choose quadratic shell elements
(S8R5) because they give accurate results for thin shells in small-strain simulations. For
further details on shell element selection, refer to Section 15.6.2 of the
ABAQUS/Standard User’s Manual.
Enter the Mesh module, and seed the part using a global element size of 0.1. From the
main menu bar, select MeshControls to specify the structured mesh technique for this
model. Create a quadrilateral mesh using quadratic, reduced-integration shell elements
with five degrees of freedom per node (S8R5).
Enter the Job module, and define a job named SkewPlate with the following
description: Linear Elastic Skew Plate. 20 kPa Load.
Save your model in a model database file named SkewPlate.cae.
Submit the job for analysis, and monitor the solution progress; correct any modeling
errors detected by the solver, and investigate the cause of any warnings.
Postprocessing the linear analysis results
Switch to the Visualization module to postprocess the analysis results. By default,
ABAQUS/Viewer plots the fast representation of the model. Plot the undeformed model
shape by selecting PlotUndeformed Shape from the main menu bar or by clicking
the tool in the toolbox.
Use the undeformed shape plot to check the model definition. Check that the element
normals for the skew-plate model were defined correctly and point in the positive
To display the element normals:
1. In the prompt area, click Undeformed Shape Options.
The Undeformed Shape Plot Options dialog box appears.
15. Set the render style to Shaded.
16. Click the Normals tab.
17. Toggle on Show normals.
18. Click OK to apply the settings and to close the dialog box.
The default view is isometric. You can change the view using the options in the view
menu or the view tools (such as ) from the toolbar.
To change the view:
1. From the main menu bar, select ViewSpecify.
The Specify View dialog box appears.
19. From the list of available methods, select Viewpoint.
20. Enter the X-, Y- and Z-coordinates of the viewpoint vector as -0.2, -1, 0.8
and the coordinates of the up vector as 0, 0, 1.
21. Click OK.
22. From the main menu bar, select ViewParallel to turn perspective off.
ABAQUS/Viewer displays your model in the specified view, as shown in Figure W12–6.
Figure W12–6. Shell element normals in skewed plate model
Symbol plots display the specified variable as a vector originating from the node or
element integration points. You can produce symbol plots of most tensor- and vector-
valued variables. The exceptions are mainly nonmechanical output variables and element
results stored at nodes, such as nodal forces. The relative sizes of the arrows indicate the
relative magnitude of the results, and the vectors are oriented along the global direction of
the results. You can plot results for the resultant of variables such as displacement (U),
reaction force (RF), etc.; or you can plot individual components of these variables.
To generate a symbol plot of the displacement:
1. From the main menu bar, select ResultField Output.
The Field Output dialog box appears; by default, the Primary Variable tab is selected.
23. From the list of output variables, select U.
24. Click OK.
The Select Plot Mode dialog box appears.
25. Choose Symbol, and click OK.
ABAQUS/Viewer displays a symbol plot of the displacements in the 3-direction on the
deformed model shape.
26. To modify the attributes of the symbol plot, click Symbol Options in the
The Symbol Plot Options dialog box appears; by default, the Basic tab is selected.
27. To plot the symbols on the undeformed model shape, click the Shape tab and
toggle on Undeformed shape.
28. Click OK to apply the settings and to close the dialog box.
A symbol plot on the undeformed model shape appears, as shown in
Figure W12–7. Symbol plot of displacement
ABAQUS/Viewer also lets you visualize the element material directions. This feature is
particularly helpful, allowing you to ensure the correctness of the material directions.
Material directions are associated with element integration points. Consequently, to view
material directions the current field output variable must be an element-based variable.
To plot the material directions:
1. From the main menu bar, select ResultField Output.
The Field Output dialog box appears; by default, the Primary Variable tab is selected.
29. From the list of output variables, select S.
30. Click OK.
The current primary field output variable changes to stress at integration points.
2. From the main menu bar, select PlotMaterial Orientations; or click the
tool in the toolbox.
The material orientation directions are plotted on the deformed shape. By default, the
triads that represent the material orientation directions are plotted without arrowheads.
31. To display the triads with arrowheads, click Material Orientation Options in
the prompt area.
The Material Orientation Plot Options dialog box appears.
32. Click the Color & Style tab; then click the Triad tab.
33. Set the Arrowhead option to use filled arrowheads in the triad.
34. Click OK to apply the settings and to close the dialog box.
35. From the main menu bar, select ViewViews Toolbox; or click the tool in
The Views toolbox appears.
36. Use the predefined views available in the toolbox to display the plate as shown in
Figure W12–8. In this figure, perspective is turned off.
In Figure W12–8 nondefault material direction colors have been used: the material 1-
direction is colored red, and the material 2-direction is colored blue.
Figure W12–8. Plot of material orientation directions in the plate
Adding geometric nonlinearity
Now perform the simulation considering geometrically nonlinear effects. From the main
menu bar, select ModelCopy, and copy the model named linear to a new model
named nonlinear. The changes required for this model are described next.
Enter the Step module. From the main menu bar, select StepEditApply Pressure
to edit the step definition. In the Basic tabbed page of the Edit Step dialog box, toggle
on Nlgeom to include geometric nonlinearity effects and set the time period for the step
to 1.0. In the Incrementation tabbed page, set the initial increment size to 0.1. The
default maximum number of increments is 100; ABAQUS may use fewer increments
than this upper limit, but it will stop the analysis if it needs more.
You may wish to change the description of the step to reflect that it is now a nonlinear
In a linear analysis ABAQUS solves the equilibrium equations once and calculates the
results for this one solution. A nonlinear analysis can produce much more output because
results can be requested at the end of each converged increment. If you do not select the
output requests carefully, the output files become very large, potentially filling the disk
space on your computer. If selected carefully, data can be saved frequently during the
simulation without using excessive disk space.
1. From the main menu bar, select OutputField Output RequestsManager
to open the Field Output Requests Manager.
37. On the right side of the dialog box, click Edit to open the field output editor.
38. Remove the field output requests defined for the linear analysis model, and specify
the default field output requests by selecting Preselected defaults under
This preselected set of output variables is the most commonly used set of field variables
for a general static procedure.
39. To reduce the size of the output database file, write field output every second
increment. Note that if you were simply interested in the final results, you could
select The last increment.
40. The history output request for the displacements of the nodes at the midspan can
be kept from the previous analysis.
Running and monitoring the job
In the Job module, create a job named NlSkewPlate and give it the description
Nonlinear Elastic Skew Plate. Remember to save your model database file.
Submit the job for analysis, and monitor the solution progress. If any errors are
encountered, correct them; if any warning messages are issued, investigate their source
and take corrective action as necessary.
The Job Monitor is particularly useful in nonlinear analyses. It gives a brief summary of
the automatic time incrementation used in the analysis for each increment. The
information is written as soon as the increment is completed, so you can monitor the
analysis as it is running. This facility is useful in large, complex problems. The
information given in the Job Monitor is the same as that given in the status file
Comparing the linear and nonlinear analysis results
When the job has completed, enter the Visualization module and plot the deformed model
shape. The final deformed shape is shown in Figure W12–9.
Figure W12–9. Final deformed shape
Next, create an X–Y plot of the displacement history of a midspan node. Use the node
indicated in Figure W12–10.
Figure W12–10. Midspan node
1. In the Labels tabbed page of the Undeformed Shape Plot Options dialog
box, toggle on Show node labels and click Apply to identify the node’s label.
41. From the main menu bar, select ResultHistory Output.
42. Select the output variable U3 for the midspan node, and click Save As. Give the
curve the name nl-20kPa.
43. From the main menu bar, select FileOpen and open the ODB file for the linear
skew plate job.
44. Repeat steps 2 and 3 above to create a curve named lin-20kPa based on the
linear analysis results.
45. From the main menu bar, select ToolsXY DataManager to open the XY
46. In the dialog box, select both curves and click Plot.
The nonlinear effects are relatively mild at this load level, as shown in Figure W12–11.
Figure W12–11. Midspan displacement history (pressure = 20kPa)
Query the plot to identify the value of the midspan displacement at the end of each
47. From the main menu bar, select ToolsQuery.
48. In the Query dialog box, select Probe values and click OK.
49. Drag the mouse across the curve to obtain the values of the midspan
displacements under full loading (this state corresponds to a time equal to 1.0).
50. Enter the vertical displacement (U3) of the midspan node from each analysis in
Load (Pa) Linear (m) NLGEOM (m)
Table W12–1. Midspan displacements
Triple the load in both the linear and nonlinear analysis models, and rerun each of the
1. Switch to the Load module and for each model do the following:
A. From the main menu bar, select LoadEditPressure.
B. In the Edit Load dialog box, enter a value of 6.0E4 for the pressure.
51. Switch to the Job module, and resubmit each analysis job.
Create and plot displacement history curves from each analysis as described earlier; name
the curves lin-60kPa and nl-60kPa. Probe the X–Y plot, and enter the vertical
displacement (U3) of the midspan node from each analysis in Table W12–1. The
nonlinear effects under the larger load are clearly evident, as shown in Figure W12–12.
Figure W12–12. Midspan displacement history (pressure = 60kPa)
How does tripling the load affect the midspan displacement in each analysis?
Optional modifications to the model
If time permits, perform the analyses that are described next.
1. Adding material nonlinearity
You will specify the post-yield behavior of the material using the Mises (or classical)
metal plasticity model. Note that ABAQUS requires the use of true stress and logarithmic
plastic strain when defining plasticity data. The data for this problem are shown in Figure
W12–13 and are plotted using this strain measure.
Figure W12–13. Stress versus strain curve
Hint: The total stain tot at any point on the curve is equal to the sum of the elastic strain
el and plastic strain pl . The elastic strain at any point on the curve can be evaluated from
Young’s modulus and the true stress .true
= Use the following relationship to
determine the plastic strains:
.pl tot el tot E = - = -
The changes to the nonlinear model are described next.
1. Enter the Property module; and, if necessary, select the nonlinear model. From
the main menu bar, select MaterialEditSteel.
52. Select MechanicalPlasticityPlastic to invoke the classical metal
plasticity model. Enter data corresponding points A and B on the stress-strain
curve shown in Figure W12–13.
Slope = E
Tip: You can use the message area of ABAQUS/CAE as a simple calculator. For
example, to compute the plastic strain at B, enter 0.02-(3e7/3e10) in the message
area and hit [Enter]. The value of the plastic strain is printed in the message area.
1. From the main menu bar, select SectionEditPlateSection.
53. In the Edit Section dialog box, toggle on During analysis to indicate that
section integration will be performed during the analysis. This is required since the
material is no longer linear elastic.
Enter the Load module. Change the magnitude of the applied pressure load to 1.E4 Pa.
1. In the Job module, create a job named PlSkewPlate and enter the following job
description: Elastic-Plastic Skew Plate. Remember to save your
model database file.
54. Submit the job for analysis, and monitor the solution progress. Correct any
modeling errors, and investigate the source of any warning messages.
To postprocess the results, contour the S11 stress component in the plate:
1. From the main menu bar, select PlotContours.
55. From the main menu bar, select ResultField Output.
56. In the Field Output dialog box, select S11 as the stress component.
The contour plot appears as shown in Figure W12–14.
Figure W12–14. Contour plot of S11
Create and plot of the displacement history of the midspan displacement node. The plot
appears as shown in Figure W12–15.
Figure W12–15. Midspan displacement history (elastic-plastic analysis)
2. Dynamic analysis
You will now investigate the response of the structure to a sudden loading. This requires
the simulation of a dynamic event. You will use the explicit dynamics solver in this
Copy the nonlinear model to a model named dynamic and make the following changes
to the dynamic model.
1. Enter the Property module. From the main menu bar, select
57. Select GeneralDensity to define the material density. Enter a density value of
Step definition and output requests
1. Enter the Step module. From the main menu bar, select StepDeleteApply
pressure to delete the general static step.
Note this will delete all step-dependent objects such as loads and output requests. These
must be redefined.
58. From the main menu bar, select StepCreate to create a Dynamic, Explicit
step. Name the step Apply pressure. In the Edit Step dialog box, enter the
following description for the step: Dynamic analysis and prescribe a time
period of 1.0 second.
59. Create a new history output. Request that displacements for the set MidSpan be
written to the output database (.odb) file as history data.
1. Enter the Load module. From the main menu bar, select LoadCreate to create
a pressure load in the Apply pressure step.
60. Name the load Pressure. Select both regions of the part using [Shift]+Click,
and choose the top side of the shell (Magenta) as the surfaces to which the
pressure load will be applied. You may need to rotate the view to more clearly
distinguish the top side of the plate. Specify a load magnitude of 1.0E4 Pa.
In a dynamic analysis, the load is applied instantaneously by default. Thus, while the
static models simulated the response of the plate to gradually applied load, this model
simulates the response of the plate to a suddenly applied load.
1. Enter the Mesh module. From the main menu bar, select MeshElement Type
to modify the element type of all regions in the model.
61. In the Element Type dialog box, select Explicit as the element library, Shell as
the element family, and Linear as the geometric order. Among the available
element controls, choose Finite membrane strains and the Relax stiffness
hourglass control. The selected element type is S4R.
1. In the Job module, create a job named DynSkewPlate and enter the following
job description: Dynamic Skew Plate. Remember to save your model
62. Submit the job for analysis, and monitor the solution progress. Correct any
modeling errors, and investigate the source of any warning messages.
Plot the time history of the vertical displacement of the midspan and the model energies
ALLKE, ALLIE, and ALLAE. The results are shown in Figure W12–16 and Figure W12–
17, respectively. The early transient response is depicted in these figures. The
displacements show progressively smaller oscillations about a steady state. In fact, if the
time period of the analysis is increased and the simulation is rerun, these oscillations
disappear completely and the displacement solution converges to a steady-state solution.
Note that the steady-state behavior is different from the static behavior due to the path-
and history-dependent effects induced by the plasticity material model.
Figure W12–16. Midspan displacement history (dynamic analysis)
Figure W12–17. Model energy history (dynamic analysis)