This simulation of the shearing of a lap joint illustrates the use of general contact in Abaqus/Standard.
The model consists of two overlapping aluminum plates that are connected with a titanium rivet. The left end of the bottom plate is fixed, and the force is applied to the right end of the top plate to shear the joint. Figure 12–27 shows the basic arrangement of the components. Because of symmetry, only half of the joint is modeled to reduce computational cost. Frictional contact is assumed.
Select the element type before designing the mesh. The mesh used for the plates should consist of C3D8I elements; the rivet should be meshed with C3D8R and C3D6 elements (a representative mesh is shown in Figure 12–28).
The steps that follow assume that you have access to the full input file for this example. This input file, lap_joint.inp, is provided in “Shearing of a lap joint,” Section A.14. Instructions on how to fetch and run the script are given in Appendix A, “Example Files.” If you wish to create the entire model using Abaqus/CAE, please refer to “Abaqus/Standard 3D example: shearing of a lap joint,” Section 12.8 of Getting Started with Abaqus: Interactive Edition.
We first review the model definition, including the node and element definitions, and section and material properties.
Model description
The input file starts with a relevant description of the simulation and model in the *HEADING option.
*HEADING Shearing of a lap joint SI units (N, kg, mm, s)
Nodal coordinates and element connectivity
Check that the preprocessor used the correct element type for the plates and rivet. Provide meaningful element set names, such as PLATE and RIVET, for the elements. The *ELEMENT options in this model follow:
*ELEMENT, TYPE=C3D8I, ELSET=PLATE ... *ELEMENT, TYPE=C3D8R, ELSET=RIVET ... *ELEMENT, TYPE=C3D6, ELSET=RIVET ...
The model definition also specifies the creation of node sets so that parts of the model can be constrained and moved easily. These sets are located at the following locations: at the bottom-left corner of the bottom plate (set CORNER), the left face of the bottom plate (set FIX), the right face of the top plate (set PULL), and the symmetry plane (set SYMM).
*NSET, NSET=CORNER ... *NSET, NSET=FIX ... *NSET, NSET=PULL ... *NSET, NSET=SYMM ...The first of these sets will be used to prevent rigid body motion in the 3-direction; the next two will be used to fix the end of one plate and pull the end of the other, respectively; the last one will be used to impose symmetry conditions.
Section and material properties
The plates are made from aluminum (elastic modulus of 71.7 × 103 MPa, 
= 0.33). Its stress-strain behavior is shown in Figure 12–29.
The rivet is made from titanium (elastic modulus of 112 × 103 MPa, = 0.34). Its stress-strain behavior is shown in Figure 12–30.
The following input options are needed to define the material properties:
*SOLID SECTION, MATERIAL=ALUMINUM, ELSET=PLATES *MATERIAL, NAME=ALUMINUM *ELASTIC 71700., 0.33 *PLASTIC 350.00, 0. 368.71, 0.001 376.50, 0.002 391.98, 0.005 403.15, 0.008 412.36, 0.011 422.87, 0.015 444.17, 0.025 461.50, 0.035 507.90, 0.070 581.50, 0.150 649.17, 0.250 704.22, 0.350 728.78, 0.400 751.85, 0.450 773.68, 0.500 794.44, 0.550 814.28, 0.600 *SOLID SECTION, MATERIAL=TITANIUM, ELSET=RIVET *MATERIAL, NAME=TITANIUM *ELASTIC 112000., 0.34 *PLASTIC 907.00, 0. 934.86, 0.001 944.28, 0.002 961.77, 0.005 973.73, 0.008 983.28, 0.011 993.89, 0.015 1014.7, 0.025 1023.3, 0.030 1051.1, 0.050 1099.8, 0.100 1129.0, 0.140 1164.9, 0.200 1190.2, 0.250 1212.8, 0.300
The contact definitions for the model are discussed here.
Defining contact
Contact will be used to enforce the interactions between the plates and the rivet. The friction coefficient between all parts is assumed to be 0.05.
This problem could use either contact pairs or the general contact algorithm. We will use general contact in this problem to demonstrate the simplicity of the contact definition.
The contact property is defined using the *SURFACE INTERACTION option; a friction coefficient of 0.05 is specified.
*SURFACE INTERACTION, NAME=FRIC *FRICTION 0.05,
Use the *CONTACT option to define a general contact interaction. Use the ALL EXTERIOR parameter on the *CONTACT INCLUSIONS option to specify self-contact for the unnamed, all-inclusive surface defined automatically by Abaqus/Standard. The *CONTACT PROPERTY ASSIGNMENT option is used to assign the contact property named FRIC to the general contact interaction.
*CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT PROPERTY ASSIGNMENT , , FRIC
Step definition and boundary conditions
Create a single static, general step and include the effects of geometric nonlinearity. Set the initial time increment to 0.05 and the total time to 1.0. Accept the default output requests.
One end of the assembly is fixed while the other is pulled along the length of the plates (1-direction). In addition, a single node is fixed in the vertical (3-) direction to prevent rigid body motion and the nodes on the symmetry plane are fixed in the direction normal to the plane (2-direction). The boundary conditions are summarized in Table 12–1.
Table 12–1 Summary of boundary conditions.
| Geometry Set | BCs |
|---|---|
| fix | U1 = 0.0 |
| pull | U1 = 2.5 |
| symm | U2 = 0.0 |
| corner | U3 = 0.0 |
The complete step definition required for the model appears below:
*STEP, NLGEOM=YES *STATIC 0.05, 1. *BOUNDARY FIX, 1, 1 PULL, 1, 1, 2.5 SYMM, 2, 2 CORNER, 3, 3 *OUTPUT, FIELD, VARIABLE=PRESELECT *OUTPUT, HISTORY, VARIABLE=PRESELECT *END STEP
Save the input in the file lap_joint.inp (see “Shearing of a lap joint,” Section A.14). Run the simulation using the following command:
abaqus job=lap_jointCheck the status and message files while the job is running to see how it is progressing.
Status file
This analysis should take approximately 13 increments to complete. The contents of the status file are shown below:
SUMMARY OF JOB INFORMATION:
STEP INC ATT SEVERE EQUIL TOTAL TOTAL STEP INC OF DOF IF
DISCON ITERS ITERS TIME/ TIME/LPF TIME/LPF MONITOR RIKS
ITERS FREQ
1 1 1 11 2 13 0.0500 0.0500 0.05000
1 2 1 3 2 5 0.100 0.100 0.05000
1 3 1 4 2 6 0.175 0.175 0.07500
1 4 1 3 2 5 0.288 0.288 0.1125
1 5 1 4 5 9 0.456 0.456 0.1688
1 6 1U 6 0 6 0.456 0.456 0.1688
1 6 2 3 3 6 0.498 0.498 0.04219
1 7 1 2 6 8 0.541 0.541 0.04219
1 8 1 1 4 5 0.583 0.583 0.04219
1 9 1 0 4 4 0.625 0.625 0.04219
1 10 1 1 2 3 0.688 0.688 0.06328
1 11 1 1 3 4 0.783 0.783 0.09492
1 12 1 2 2 4 0.926 0.926 0.1424
1 13 1 1 2 3 1.00 1.00 0.07441
In Abaqus/Viewer, examine the deformation of the assembly.
Deformed model shape and contour plots
The basic results of this simulation are the deformation of the joint and the stresses caused by the shearing process. Plot the deformed model shape and the Mises stress, as shown in Figure 12–31 and Figure 12–32, respectively.
Contact pressures
You will now plot the contact pressures in the lap joint.
Since it is difficult to see contact pressures when the entire model is displayed, use the Display Groups toolbar to display only the top plate in the viewport.
Create a path plot to examine the variation of the contact pressure around the bolt hole of the top plate.
To create a path plot:
In the Results Tree, double-click Paths. In the Create Path dialog box, select Edge list as the type and click Continue.
In the Edit Edge List Path dialog box, select the instance corresponding to the top plate and click Add After.
In the prompt area, select by shortest distance as the selection method.
In the viewport, select the edge at the left end of the bolt hole as the starting edge of the path and the node at the right end of the bolt hole as the end node of the path, as shown in Figure 12–33.
Click Done in the prompt area to indicate that you have finished making selections for the path. Click OK to save the path definition and to close the Edit Edge List Path dialog box.
In the Results Tree, double-click XYData. Select Path in the Create XY Data dialog box, and click Continue.
In the Y Values frame of the XY Data from Path dialog box, click Step/Frame. In the Step/Frame dialog box, select the last frame of the step. Click OK to close the Step/Frame dialog box.
Make sure that the field output variable is set to CPRESS, and click Plot to view the path plot. Click Save As to save the plot.
The path plot appears as shown in Figure 12–34.
