workCONT-WK02-Q-LapJoint1

W2.10Note: This workshop provides instructions in terms of the Abaqus Keywords interface. If you wish to use the Abaqus GUI interface instead, please see the “Interactive” version of these instructions. Please complete either the Keywords or Interactive version of this workshop.IntroductionThis workshop simulates the shearing of a lap joint. A lap joint describes a technique for joining two pieces of material by overlapping them. In the model shown in Figure W21, two aluminum plates are overlapped; a titanium rivet penetrates the two plates, thus connecting them together. The rivet is modeled with C3D8R elements; the plates with C3D8I elements. Because of symmetry, only half of the joint is modeled to reduce computational cost. Frictional contact is assumed. Figure W21. The lap joint assembly model (undeformed configuration, top; deformed configuration, bottom)Preliminaries1. Change to the ./contact/keywords/lap_joint directory. 2. Open the input file w_lap_joint.inp, which already contains the nodes, elements, and material model data for the analysis. You will edit the input file to include the contact, step and boundary condition definitions.Part 1: Analysis using contact pairsThis problem could use either the contact pairs or the general contact algorithm. We will consider both approaches, beginning with the contact pair algorithm.Contact propertiesFrictional contact is assumed between all mating parts. The coefficient of friction is 0.05. Use the penalty constraint enforcement method for both the normal and tangential behaviors. For the normal behavior, scale the penalty stiffness to 10% of the default value. The options to define these properties are as follows:*Surface Interaction, name=fric*Friction 0.05,*Surface Behavior, penalty , , 0.1Contact pairsPredefined surfaces are available to facilitate the contact pair definitions. The surfaces are depicted in Figure W22 through Figure W24.bot-plate-1top-plate-1hole-plate-1 Figure W22. Surface definitions on top plate (plate-1)bot-plate-2top-plate-2hole-plate-2Figure W23. Surface definitions on bottom plate (plate-2)shank-rivettop-rivetbot-rivet Figure W24. Surface definitions on rivetSince the rivet is more finely meshed than the plates, any contact pair involving the rivet should use the rivet surface as the slave surface. The surfaces will be adjusted to ensure initial contact.Five contact pairs are required to define the contact interactions. They will be defined between the surfaces listed in Table W21.Table W21. Contact pairs Slave SurfaceMaster Surfacetop-plate-2bot-plate-1shank-rivethole-plate-1top-rivettop-plate-1shank-rivethole-plate-2bot-rivetbot-plate-2The options to define the contact pairs are as follows:*Contact Pair, interaction=fric, type=SURFACE TO SURFACE, adjust=0.01 top-plate-2, bot-plate-1 shank-rivet, hole-plate-1 top-rivet, top-plate-1 shank-rivet, hole-plate-2 bot-rivet, bot-plate-2 Step definitionThe analysis consists of a single general static step. The step will consider geometrically nonlinear effects. The initial time increment size of the step will be set to 5% of the total time period.The following options define the step and analysis procedure: *STEP, NLGEOM=YES*STATIC0.05, 1.Boundary conditionsYour next task will be to define the boundary conditions that will act on the assembly. One end of the assembly is fixed while the other is pulled along the length of the plates (X-direction). Also, a single node is fixed in the vertical (Z-) direction to prevent rigid body motion and the nodes on the symmetry plane are fixed in the direction normal to the plane (Y-direction). Predefined sets are available to facilitate the procedure. These sets are depicted in Figure W25.cornersymmpullfixFigure W25. Set definitionsThe options to define the boundary conditions are as follows:*Boundary fix, 1, 1 pull, 1, 1, 2.5corner, 3, 3 symm, 2, 2OutputRequest predefined field and history output. The options to define the output requests are as follows:*Output, field, variable=PRESELECT*Output, history, variable=PRESELECT Save all the changes and close the input file. Running the job and visualizing the results:Run the analysis using the following command:abaqus job=w_lap_jointVisualizing the analysis resultsAfter the analysis is complete, you will review the results using Abaqus/Viewer.1. Start Abaqus/Viewer and open the file w_lap_joint.odb:abaqus viewer odb=w_lap_joint.odb2. Click to plot the Mises stress, as shown in Figure W26.Figure W26. Mises stress distribution3. In the Results Tree, expand the Instances branch underneath output database file named w_lap_joint.odb. Select the rivet. Click mouse button 3 and select Replace from the menu that appears to examine only the rivet. Contour the shear stress components to better understand the stress state in the rivet.4. Restore the visibility of all part instances (click in the toolbar).5. Plot the contact pressures (use the Field Output toolbar to change the selected output variable to CPRESS; alternatively select ResultField Output to make the change). Since it is difficult to see the contact pressures when the entire model is displayed, make only the top plate visible:a. In the toolbar, click the Replace tool .b. In the prompt area, choose Part instances as the selection method.c. Click on the top plate in the viewport.6. Create a path plot to examine the variation of the contact pressure around the bolt hole of the top plate.a. In the Results Tree, double-click Paths. In the Create Path dialog box, select Edge list as the type and click Continue.b. In the Edit Edge List Path dialog box, select PLATE-1 as the part instance and click Add After.c. In the prompt area, select by shortest distance as the selection method.d. In the viewport select the edge and node indicated in Figure W27 to define the path.Select this element edge to startEnd node Figure W27 Path on bolt holee. In the Results Tree, double-click XYData. Select Path in the Create XY Data dialog box and click Continue.f. 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.g. Make sure that Field output variable is set to CPRESS and click Plot to view the path plot. Click Save As to save the plot as plate-1.The plot appears as shown in Figure W28.Figure W28 CPRESS distribution around the bolt hole in top plate.OptionalDefine a path around the bolt hole of the bottom plate. Use this path to plot and save the CPRESS variation around the bolt hole of the bottom plate. Plot both curves simultaneously (expand the XYData container, select both curves, and click mouse button 3; from the menu that appears, select Plot). The plot appears as shown in Figure W29.Figure W29 CPRESS distribution around the bolt hole in both plates.Part 2: Analysis using general contactWe will now use general contact to solve the lap joint problem.1. Copy the input file named w_lap_joint.inp to one named w_lap_joint_gc.inp. Edit this input file as described below.2. Locate the contact pairs defined earlier and delete them.3. Create a general contact interaction using the default all-inclusive element-based surface and apply the frictional contact property globally. The following options define the interaction:*CONTACT*CONTACT INCLUSIONS, ALL EXTERIOR*CONTACT PROPERTY ASSIGNMENT, , FRIC4. Save all the changes and close the input file. 5. Run the analysis using the following command:abaqus job=w_lap_joint_gc6. When the job is complete, use the following procedure to visualize the results using Abaqus/Viewer.7. Compare the results with those obtained earlier using contact pairs. A comparison of the stress state in the lap joint