You have been asked to find the axial stiffness of the rubber mount shown in Figure 10–39 and to identify any areas of high maximum principal stress that might limit the fatigue life of the mount. The mount is bonded at both ends to steel plates. It will experience axial loads up to 5.5 kN distributed uniformly across the plates. The cross-section geometry and dimensions are given in Figure 10–39.
You can use axisymmetric elements for this simulation since both the geometry of the structure and the loading are axisymmetric. Therefore, you only need to model a plane through the component: each element represents a complete 360° ring. You will examine the static response of the mount; therefore, you will use Abaqus/Standard for your analysis.
You do not need to model the whole section of this axisymmetric component because the problem is symmetric about a horizontal line through the center of the mount. By modeling only half of the section, you can use half as many elements and, hence, approximately half the number of degrees of freedom. This significantly reduces the run time and storage requirements for the analysis or, alternatively, allows you to use a more refined mesh.
Many problems contain some degree of symmetry. For example, mirror symmetry, cyclic symmetry, axisymmetry, or repetitive symmetry (shown in Figure 10–40) are common. More than one type of symmetry may be present in the structure or component that you want to model.
When modeling just a portion of a symmetric component, you have to add boundary conditions to make the model behave as if the whole component were being modeled. You may also have to adjust the applied loads to reflect the portion of the structure actually being modeled. Consider the portal frame in Figure 10–41.
The frame is symmetric about the vertical line shown in the figure. To maintain symmetry in the model, any nodes on the symmetry line must be constrained from translating in the 1-direction and from rotating about the 2- or 3-axes (degrees of freedom 5 and 6). Therefore, the symmetry constraints are
*BOUNDARY <node>,1 <node>,5,6
In the frame problem the load is applied along the model's symmetry plane; therefore, only half of the total value should be applied to the portion you are modeling.
In axisymmetric analyses using axisymmetric elements, such as this rubber mount example, we need model only the cross-section of the component. The element formulation automatically includes the effects of axial symmetry.
The model in this example uses the default r–z (1–2) axisymmetric coordinate system in this simulation. Its origin is placed at the level of the bottom of the plate, as shown in Figure 10–39.
The mesh in this example uses a 30 × 15 mesh of first-order, axisymmetric, hybrid solid elements (CAX4H) for the rubber mount. Only the bottom half of the mount is specified in the model, as shown in Figure 10–42.
Hybrid elements are required in this example because the material is fully incompressible. The elements are not expected to be subjected to bending, so shear locking in these fully integrated elements should not be a concern. Model the steel plates with a single layer of incompatible mode elements (CAX4I) because it is possible that the plates may bend as the rubber underneath them deforms.The node and element numbers from the input file given in “Axisymmetric mount,” Section A.10, are shown in Figure 10–43 and Figure 10–44. These will be used in the discussion of this example. If you build the model yourself, it will probably have different node and element numbers.
The steps that follow assume that you have access to the full input file for this example. This input file, mount.inp, is provided in “Blast loading on a stiffened plate,” Section A.9. Instructions on how to fetch and run the script are given in Appendix A, “Example Files.”
If you use Abaqus/CAE or another preprocessor to create the mesh for this model, try to create a node set MIDDLE containing all the nodes on the symmetry plane, and apply a pressure load of 0.50 MPa to the bottom of the plate (Figure 10–45). Check that this pressure results in a total applied load of 5.5 kN (5.5 kN = 0.50 MPa × 
). If you can't create the mesh, the Abaqus input options used to create the model can be found in “Axisymmetric mount,” Section A.10.
If you wish to create the entire model using Abaqus/CAE, refer to “Example: axisymmetric mount,” Section 10.7 of Getting Started with Abaqus: Interactive Edition.
We review the model data, including the geometry definition (nodes and elements) and the material properties.
Model description
The input file should contain a suitable description of the analysis.
*HEADING Axisymmetric mount analysis under axial loading S.I. Units (m, kg, N, sec)
Nodal coordinates and element connectivity
There will be at least two *ELEMENT option blocks in the input file since two different types of elements are used in the simulation. It is a good idea to check that the element types are correct and that the element sets containing the elements have descriptive names. The *ELEMENT options in your input file should look like
*ELEMENT, TYPE=CAX4I, ELSET=PLATE *ELEMENT, TYPE=CAX4H, ELSET=RUBBER
Node sets
Check that the node set MIDDLE has been created. If it has not, add it using an editor.
Property definition
Two element property definitions are required: one for the elements modeling the rubber and one for those modeling the plates. The following element property definitions should be in your model:
*SOLID SECTION, MATERIAL=RUBBER, ELSET=RUBBER *SOLID SECTION, MATERIAL=STEEL, ELSET=PLATE
Material properties: hyperelastic model for the rubber
You have been given some experimental test data, shown in Figure 10–46, for the rubber material used in the mount. Three different sets of test data—a uniaxial test, a biaxial test, and a planar (shear) test—are available. You decide to have Abaqus calculate the appropriate hyperelastic material constants from the test data. You are not sure how large the strains will be in the rubber mount, but you suspect that they will be under 2.0.
The test data for the biaxial and planar tests go well beyond this magnitude, so you decide to perform a one-element simulation of the experimental tests to confirm that the coefficients that Abaqus calculates from the test data are adequate.Use a first-order, polynomial strain energy function to model the rubber material. Indicate these choices by using the N=1 and POLYNOMIAL parameters on the *HYPERELASTIC option. Use the TEST DATA INPUT parameter to indicate that Abaqus should find the material constants from the test data you will provide. The test data are given on options that immediately follow the *HYPERELASTIC option. The data should be entered as nominal stress and the corresponding nominal strain, with negative values indicating compression. You may be able to enter the data directly using your preprocessor (for instance, if you are using Abaqus/CAE); otherwise, you will have to add it to your input file with an editor. The material definition for the rubber will look like
*MATERIAL, NAME=RUBBER *HYPERELASTIC, N=1, POLYNOMIAL, TEST DATA INPUT *UNIAXIAL TEST DATA 0.054E6, 0.0380 0.152E6, 0.1338 0.254E6, 0.2210 0.362E6, 0.3450 0.459E6, 0.4600 0.583E6, 0.6242 0.656E6, 0.8510 0.730E6, 1.4268 *BIAXIAL TEST DATA 0.089E6, 0.0200 0.255E6, 0.1400 0.503E6, 0.4200 0.958E6, 1.4900 1.703E6, 2.7500 2.413E6, 3.4500 *PLANAR TEST DATA 0.055E6, 0.0690 0.324E6, 0.2828 0.758E6, 1.3862 1.269E6, 3.0345 1.779E6, 4.0621
The input file for the single-element simulation of the three experimental tests is shown in “Test fit of hyperelastic material data,” Section A.11. The computational and experimental results for the various types of tests are compared in Figure 10–47, Figure 10–48, and Figure 10–49.
Figure 10–47 Comparison of experimental data (BIAXIAL) and Abaqus results (BIAX_COMP): biaxial tension.
Material properties: elastic properties for the steel
The steel is modeled with linear elastic properties only (
= 200 GPa, 
= 0.3) because the loads should not be large enough to cause inelastic deformations. Thus, the material option blocks for the steel are
*MATERIAL, NAME=STEEL *ELASTIC 2.0E11, 0.3
We now discuss the history data associated with this problem, including the time incrementation parameters, boundary conditions, loading, and output requests.
Including nonlinear geometry and specifying the initial increment size
When hyperelastic materials are used in a model, Abaqus assumes that it may undergo large deformations. But large deformations and other nonlinear geometric effects are included only if the NLGEOM parameter is set to YES on the *STEP option. Therefore, you must include it in this simulation or Abaqus will terminate the analysis with an input error. The *STEP option should look like
*STEP, NLGEOM=YES
The simulation will be a static analysis with a total step time of 1.0. Specify the initial time increment to be 1/100th of the total step time. The procedure option block should look like
*STATIC .01, 1.0
Boundary conditions
Specify symmetry boundary conditions on the nodes lying on the symmetry plane. In this model the symmetry conditions prevent the nodes from moving in degree of freedom 2 (axially), as shown in Figure 10–50.
Symmetry conditions that constrain motion in the global 2-direction can be applied using the YSYMM type boundary condition, or you can simply constrain the 2-direction. In this case the *BOUNDARY option block has the following format:*BOUNDARY MIDDLE, 2, 2, 0.0
No boundary constraints are needed in the radial direction (global 1-direction) because the axisymmetric nature of the model does not allow the structure to move as a rigid body in the radial direction. Abaqus will allow nodes to move in the radial direction, even those initially on the axis of symmetry (i.e., those with a radial coordinate of 0.0), if no boundary conditions are applied to their radial displacements (degree of freedom 1). Since you want to let the mount deform radially in this analysis, do not apply any boundary conditions; again, Abaqus will prevent rigid body motions automatically.
Loading
The mount must carry a maximum axial load of 5.5 kN, spread uniformly over the steel plates. A distributed load is, therefore, applied to the bottom of the steel plate. The magnitude of the pressure is given by
If you generated the pressure loading using a preprocessor, a *DLOAD option block with many data lines may be present in the input file.
*DLOAD 1, P1, 0.50E6 2, P1, 0.50E6 ... 29, P1, 0.50E6 30, P1, 0.50E6
For the element and node numbering discussed here, the pressure is applied to face 1 of all the elements in element set PLATE. This allows us to use a much more compact format for the data lines of the *DLOAD option block.
*DLOAD PLATE, P1, 0.50E6
Output requests
Write the preselected variables and nominal strains as field output to the output database file. In addition, write the displacement of one of the nodes on the bottom of the steel plate to the output database file so that the stiffness of the mount can be calculated. You will need to create a node set containing the node. The output option blocks in your model should be similar to the following:
*NSET, NSET=OUT 1, *OUTPUT, FIELD, VARIABLE=PRESELECT *ELEMENT OUTPUT NE, *OUTPUT, HISTORY *NODE OUTPUT, NSET=OUT U,Ensure that the end of the step definition is clearly marked with an *END STEP option.
Store your input options in a file called mount.inp. The input options for the model discussed in the above sections can be found in “Axisymmetric mount,” Section A.10. Since the nonlinear nature of the simulation means that it may take some time to complete, use the following command to run the analysis in the background:
abaqus job=mount
When the job has completed, check the data file, mount.dat, for errors. If there are any, correct the input file and rerun the analysis. If necessary, compare your input with that shown in “Axisymmetric mount,” Section A.10.
We briefly review the results associated with the polynomial fit of the test data.
The hyperelastic material parameters
In this simulation you specified that the material is incompressible (
=0). The incompressibility is assumed since no volumetric test data were provided. To simulate compressible behavior, you must provide volumetric test data in addition to the other test data. You also specified that Abaqus should use a first-order, polynomial strain energy function. This form of the hyperelasticity model is known as the Mooney-Rivlin material model.
The hyperelastic material coefficients—
, 
, and —that Abaqus calculates from the material test data are given in the data file, mount.dat, provided that you used the *PREPRINT, MODEL=YES option in the model data section of the input file. The material test data are also written in the file so that you can ensure that Abaqus used the correct data, as shown below.
M A T E R I A L D E S C R I P T I O N
MATERIAL NAME: RUBBER
HYPERELASTIC MATERIAL PROPERTIES
UNIAXIAL TEST DATA
NOMINAL STRAIN NOMINAL STRESS(TEST) NOMINAL STRESS(ABAQUS)
3.8000E-02 5.4000E+04 3.9605E+04
0.1338 1.5200E+05 1.2803E+05
0.2210 2.5400E+05 1.9764E+05
0.3450 3.6200E+05 2.8404E+05
0.4600 4.5900E+05 3.5477E+05
0.6242 5.8300E+05 4.4505E+05
0.8510 6.5600E+05 5.5627E+05
1.427 7.3000E+05 8.0275E+05
HYPERELASTIC MATERIAL PROPERTIES
BIAXIAL TEST DATA
NOMINAL STRAIN NOMINAL STRESS(TEST) NOMINAL STRESS(ABAQUS)
2.0000E-02 8.9000E+04 4.1264E+04
0.1400 2.5500E+05 2.2551E+05
0.4200 5.0300E+05 4.6078E+05
1.490 9.5800E+05 1.0063E+06
2.750 1.7030E+06 1.7767E+06
3.450 2.4130E+06 2.3301E+06
HYPERELASTIC MATERIAL PROPERTIES
PLANAR TEST DATA
NOMINAL STRAIN NOMINAL STRESS(TEST) NOMINAL STRESS(ABAQUS)
6.9000E-02 5.5000E+04 9.0339E+04
0.2828 3.2400E+05 2.9189E+05
1.386 7.5800E+05 8.3431E+05
3.034 1.2690E+06 1.4500E+06
4.062 1.7790E+06 1.8235E+06
HYPERELASTICITY - MOONEY-RIVLIN STRAIN ENERGY
D1 C10 C01
0.00000000 176050.524 4332.63031 If there were any problems with the stability of the hyperelastic material model, warning messages would be given before the material parameters. The material model is stable at all strains with these material test data and this strain energy function. However, if you specified that a second-order (N=2), polynomial strain energy function be used, you would see the following warnings in the data file:
*HYPERELASTIC, N=2, POLYNOMIAL, TEST DATA INPUT
***WARNING: UNSTABLE HYPERELASTIC MATERIAL
FOR UNIAXIAL TENSION WITH A NOMINAL STRAIN LARGER THAN 6.9700
FOR UNIAXIAL COMPRESSION WITH A NOMINAL STRAIN LESS THAN -0.9795
FOR BIAXIAL TENSION WITH A NOMINAL STRAIN LARGER THAN 5.9800
FOR BIAXIAL COMPRESSION WITH A NOMINAL STRAIN LESS THAN -0.6458
FOR PLANE TENSION WITH A NOMINAL STRAIN LARGER THAN 7.0400
FOR PLANE COMPRESSION WITH A NOMINAL STRAIN LESS THAN -0.8756
POLYNOMIAL STRAIN ENERGY FUNCTION WITH N = 2
D1 C10 C01
D2 C20 C11 C02
0.0000E+00 0.1934E+06 -148.2
0.0000E+00 -805.7 180.0 -3.967If you only had the uniaxial test data available for this problem, you would find that the Mooney-Rivlin material model Abaqus creates would have unstable material behavior above certain strain magnitudes.
Use Abaqus/Viewer to look at the analysis results by issuing the following command at the operating system prompt:
abaqus viewer odb=mount
Calculating the stiffness of the mount
Determine the stiffness of the mount by creating an X–Y plot of the displacement of the steel plate as a function of the applied load. You will first create a plot of the vertical displacement of the node on the steel plate for which you wrote data to the output database file. Data were written for the node in set OUT in this model.
To create a history curve of vertical displacement and swap the X- and Y-axes:
In the Results Tree, expand the History Output container underneath the output database named mount.odb.
Locate and select the vertical displacement U2 at the node in set OUT.
Click mouse button 3, and select Save As from the menu that appears to save the X–Y data.
The Save XY Data As dialog box appears.
In the Save XY Data As dialog box, name the curve SWAPPED and select swap(XY) as the save operation; click OK.
The plot of time-displacement appears in the viewport.
You now have a curve of time-displacement. What you need is a curve showing force-displacement. This is easy to create because in this simulation the force applied to the mount is directly proportional to the total time in the analysis. All you have to do to plot a force-displacement curve is multiply the curve SWAPPED by the magnitude of the load (5.5 kN).
To multiply a curve by a constant value:
In the Results Tree, double-click XYData.
The Create XY Data dialog box appears.
Select Operate on XY data, and click Continue.
The Operate on XY Data dialog box appears.
In the XY Data field, double-click SWAPPED.
The expression "SWAPPED" appears in the text field at the top of the dialog box. Your cursor should be at the end of the text field.
Multiply the data object in the text field by the magnitude of the applied load by entering *5500.
Save the multiplied data object by clicking Save As at the bottom of the dialog box.
The Save XY Data As dialog box appears.
In the Name text field, type FORCEDEF; and click OK to close the dialog box.
To view the force-displacement plot, click Plot Expression at the bottom of the Operate on XY Data dialog box.
You have now created a curve with the force-deflection characteristic of the mount (the axis labels do not reflect this since you did not change the actual variable plotted). To get the stiffness, you need to differentiate the curve FORCEDEF. You can do this by using the differentiate( ) operator in the Operate on XY Data dialog box.
To obtain the stiffness:
In the Operate on XY Data dialog box, clear the current expression.
From the Operators listed, click differentiate(X).
differentiate( ) appears in the text field at the top of the dialog box.
In the XY Data field, double-click FORCEDEF.
The expression differentiate( "FORCEDEF" ) appears in the text field.
Save the differentiated data object by clicking Save As at the bottom of the dialog box.
The Save XY Data As dialog box appears.
In the Name text field, type STIFF; and click OK to close the dialog box.
To plot the stiffness-displacement curve, click Plot Expression at the bottom of the Operate on XY Data dialog box.
Click Cancel to close the dialog box.
Open the Axis Options dialog box, and switch to the Title tabbed page.
Customize the axis titles so they appear as shown in Figure 10–51.
Click Dismiss to close the Axis Options dialog box.
To define the stiffness curve directly:
In the Results Tree, double-click XYData.
The Create XY Data dialog box appears.
Select Operate on XY data, and click Continue.
The Operate on XY Data dialog box appears.
From the Operators listed, click differentiate(X).
differentiate( ) appears in the text field at the top of the dialog box.
In the XY Data field, double-click SWAPPED.
The expression differentiate( "SWAPPED" ) appears in the text field.
Place the cursor in the text field directly after the "SWAPPED" data object, and type *5500 to multiply the swapped data by the constant total force value.
differentiate( "SWAPPED"*5500 ) appears in the text field.
Save the differentiated data object by clicking Save As at the bottom of the dialog box.
The Save XY Data As dialog box appears.
In the Name text field, type STIFFNESS; and click OK to close the dialog box.
Click Cancel to close the Operate on XY Data dialog box.
Customize the X- and Y-axis labels as they appear in Figure 10–51 if you have not already done so.
In the Results Tree, click mouse button 3 on STIFFNESS underneath the XYData container and select Plot from the menu that appears to view the plot in Figure 10–51 that shows the variation of the mount's axial stiffness as the mount deforms.
Model shape plots
You will now plot the undeformed and deformed model shapes of the mount. The latter plot will allow you to evaluate the quality of the deformed mesh and to assess the need for mesh refinement.
To plot the undeformed and deformed model shapes:
From the main menu bar, select Plot
Undeformed Shape; or use the 
tool in the Visualization module toolbox to plot the undeformed model shape (see Figure 10–52).
Select PlotDeformed Shape, or use the 
tool to plot the deformed model shape of the mount (see Figure 10–53).
If the figure obscures the plot title, you can move the plot by clicking the 
tool and holding down mouse button 1 to pan the deformed shape to the desired location. Alternatively, you can turn the plot title off (ViewportViewport Annotation Options).
The plate has been pushed up, causing the rubber to bulge at the sides. Zoom in on the bottom left corner of the mesh using the 
tool from the View Manipulation toolbar. Click mouse button 1, and hold it down to define the first corner of the new view; move the mouse to create a box enclosing the viewing area that you want (Figure 10–54); and release the mouse button. Alternatively, you can zoom and pan the plot by selecting ViewSpecify from the main menu bar.
You should have a plot similar to the one shown in Figure 10–54.
Some elements in this corner of the model are becoming badly distorted because the mesh design in this area was inadequate for the type of deformation that occurs there. Although the shape of the elements is fine at the start of the analysis, they become badly distorted as the rubber bulges outward, especially the element in the corner. If the loading were increased further, the element distortion may become so excessive that the analysis may abort. “Mesh design for large distortions,” Section 10.8, discusses how to improve the mesh design for this problem.
The keystoning pattern exhibited by the distorted elements in the bottom right-hand corner of the model indicates that they are locking. A contour plot of the hydrostatic pressure stress in these elements (without averaging across elements sharing common nodes) shows rapid variation in the pressure stress between adjacent elements. This indicates that these elements are suffering from volumetric locking, which was discussed earlier in “Selecting elements for elastic-plastic problems,” Section 10.3, in the context of plastic incompressibility. Volumetric locking arises in this problem from overconstraint. The steel is very stiff compared to the rubber. Thus, along the bond line the rubber elements cannot deform laterally. Since these elements must also satisfy incompressibility requirements, they are highly constrained and locking occurs. Analysis techniques that address volumetric locking are discussed in “Techniques for reducing volumetric locking,” Section 10.9.
Contouring the maximum principal stress
Plot the maximum in-plane principal stress in the model. Follow the procedure given below to create a filled contour plot on the actual deformed shape of the mount with the plot title suppressed.
To contour the maximum principal stress:
By default, Abaqus/Viewer displays S, Mises as the primary field output variable. In the Field Output toolbar, select Max. Principal as the invariant.
Abaqus/Viewer automatically changes the current plot state to display a contour plot of the maximum in-plane principal stresses on the deformed model shape.
Open the Contour Plot Options dialog box.
Drag the uniform contour intervals slider to 8.
Click OK to view the contour plot and to close the dialog box.
Create a display group showing only the elements in the rubber mount.
In the Results Tree, expand the Materials container underneath the output database file named Mount.odb.
Click mouse button 3 on RUBBER, and select Replace from the menu that appears to replace the current display with the selected elements.
The viewport display changes and displays only the rubber mount elements, as shown in Figure 10–55.
The maximum principal stress in the model, reported in the contour legend, is 136 kPa. Although the mesh in this model is fairly refined and, thus, the extrapolation error should be minimal, you may want to use the query tool 
to determine the more accurate integration point values of the maximum principal stress.
When you look at the integration point values, you will discover that the peak value of maximum principal stress occurs in one of the distorted elements in the bottom right-hand part of the model. This value is likely to be unreliable because of the levels of element distortion and volumetric locking. If this value is ignored, there is an area near the plane of symmetry where the maximum principal stress is around 88.2 kPa.
The easiest way to check the range of the principal strains in the model is to display the maximum and minimum values in the contour legend.
To check the principal nominal strain magnitude:
From the main menu bar, select ViewportViewport Annotation Options.
The Viewport Annotation Options dialog box appears.
Click the Legend tab, and toggle on Show min/max values.
Click OK.
The maximum and minimum values appear at the bottom of the contour legend in the viewport.
In the Field Output toolbar, select Primary as the variable type if it is not already selected.
Abaqus/Viewer automatically changes the current plot state to display a contour plot of the maximum in-plane principal stresses on the deformed model shape.
From the list of output variables, select NE.
From the list of invariants in the Field Output toolbar, select Max. Principal if it is not already selected.
The contour plot changes to display values for maximum principal nominal strain. Note the value of the maximum principal nominal strain from the contour legend.
From the list of invariants, select Min. Principal.
The contour plot changes to display values for minimum principal nominal strain. Note the value of the minimum principal nominal strain from the contour legend.
The maximum and minimum principal nominal strain values indicate that the maximum tensile nominal strain in the model is about 100% and the maximum compressive nominal strain is about 56%. Because the nominal strains in the model remained within the range where the Abaqus hyperelasticity model has a good fit to the material data, you can be fairly confident that the response predicted by the mount is reasonable from a material modeling viewpoint.
