workCONT-WK01-Q-Seal

W1.17Note: 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.Goals Evaluate a hyperelastic material. Define contact interactions using contact pairs and general contact. Perform a large displacement analysis with Abaqus/Standard. Use Abaqus/Viewer to create a compression load-deflection curve.IntroductionIn this workshop, a compression analysis of a rubber seal is performed to determine the seals performance. The goal is to determine the seals compression load-deflection (CLD) curve, deformation and stresses. The analysis will be performed using Abaqus/Standard. Two analyses are performed: one using contact pairs and the other using general contact. As shown in Figure W11, the top outer surface of the seal is covered with a polymer layer, and the seal is compressed between two rigid surfaces (the upper one is displaced along the negative 2-direction; the lower one is fixed). During compression, the cover contacts the top rigid surface; the outer surface of the seal is in contact with the cover and the bottom rigid surface; in addition the inner surface of the seal may come into contact with itself.SealCoverRigid SurfacesfixedU2Figure W11. Seal model Seal analysis1. Change to the ./contact/keywords/seal directory. 2. Open the input file w_seal.inp, which already contains the nodes, elements, and material model data for the analysis. You will first use Abaqus/CAE functionality to evaluate the stability of the hyperelastic material model and then edit the input file to include the contact, step and boundary condition definitions. Material EvaluationIt is important to determine whether the material model of the seal will be stable during the analysis. Before completing the input file, evaluate the material definition that is used for the seal.1. Use your text editor to review the supplied workshop model contained in the file w_seal.inp. 2. The material named SANTOPRENE is used for the seal. Locate the *MATERIAL, NAME=SANTOPRENE option. It is a hyperelastic material with a first order polynomial strain energy potential. The coefficients are already specified for the analysis.3. Evaluate the material definition. Abaqus/CAE provides a convenient Evaluate option that allows you to view the behavior predicted by a hyperelastic material by performing standard tests to choose a suitable material formulation. You will use this option to view the behavior predicted by the material SANTOPRENE. a. Start a session of AQUS/CAE using the following command at the command prompt:abaqus cae In the Start Session dialog box, select Create Model Database. b. In the Model Tree, double-click the Materials container to create a material definition as specified in the input file. In the Edit Material dialog box, name the material Santoprene; from the menu bar, select MechanicalElasticityHyperelastic; in the Hyperelastic field, select the Polynomial strain energy potential and the Coefficients input source, accept a strain energy potential order of 1, and enter the values of the coefficients (defined in the input file) as shown in Figure W12. Click OK to save the material definition and exit the material editor.Figure W12. Material editorc. From the main menu bar in the Property module, select MaterialEvaluateSantoprene. d. The Evaluate Material dialog box appears. Notice that you can choose either the Coefficients or Test data source for evaluating the material. Typically the test data are used to define a material model; you can use the Evaluate option to view the predicted behavior and adjust the material definition as necessary. In this workshop you will only evaluate the stability of the material model for the given coefficients.e. In the Evaluate Material dialog box, accept all defaults and click OK. Abaqus/CAE creates and submits a job to perform the standard tests using the material Santoprene; at the same time, Abaqus/CAE switches to the Visualization module and displays the evaluation results when the job is complete. Figure W13 shows the Material Parameters and Stability Limit Information dialog box; Figure W14 shows three stress vs. strain plots from uniaxial, biaxial, and planar tests. Question W11:What do the plots indicate about the stability of the material? Based on these results, you can have confidence that your material will remain stable.Figure W13. Material parameters and stability limit information Figure W14. Material evaluation results for uniaxial, biaxial, and planar tests After evaluating the material, you can exit Abaqus/CAE and will now complete the model definition.Part 1: Analysis using contact pairs Contact interactions1. Open the input file w_seal.inp in a text editor.2. Define contact pairs as listed in Table W11. The surfaces which will be used in the contact pair definitions are shown in Figure W15. The required option is: *CONTACT PAIR, INTERACTION=frictionless, ADJUST=0.001Cover, SealOuterCover, TopSealOuter, BottomNote that the interaction property named frictionless has already been defined in the input file. Locate the *SURFACE INTERACTION, NAME=frictionless option to review its definition. Table W11. Contact pairs Slave SurfaceMaster SurfaceCoverSealOuterCoverTopSealOuterBottomTopBottomSealOuterSealInnerCoverFigure W15. Contact surfaces 3. Define a self-contact definition for the inner surface of the seal:*CONTACT PAIR, INTERACTION=frictionlessSealInner,Question W12:In the interaction between the seal and the cover, why do we choose SealOuter as the master surface?Step definition1. Define a general static step considering geometric nonlinearity. Set the initial time increment size to 0.5% of the total time period. The following option defines the procedure:*STEP, NLGEOM=YES*STATIC0.005, 1.Boundary conditions and history output requests1. Asymmetric lateral sliding of the model is prevented by constraining the seal and the cover along their vertical symmetry axes in the X-direction. The bottom rigid surface is fixed, and a displacement of 6 units is applied to the top rigid surface along the Y-direction to compress the seal between the two surfaces. The node sets on which the boundary conditions will be defined are shown in Figure W16. The following option completes these boundary conditions: *BOUNDARYFix1, 1, 1BotRP, ENCASTRETopRP, 1, 1TopRP, 2, 2, -6.TopRP, 6, 6TopRPBotRPFix_1Figure W16: Node Sets2. The preselected default field output does not include the nominal strain NE; to visualize the nominal strain in Abaqus/Viewer, you will write additional field output to the output database file. Locate the *OUTPUT, FIELD, VARIABLE=PRESELECT option and add the following sub-option:*ELEMENT OUTPUTNE,3. Add a history output request to write the history of RF2 and U2 for the set TopRP to the output database file. The required option is:*OUTPUT, HISTORY*NODE OUTPUT, NSET=TopRPRF2, U24. 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_sealWhen the job is complete, use the following procedure to visualize the results using Abaqus/Viewer:1. Start Abaqus/Viewer and open the file w_seal.odb:abaqus viewer odb=w_seal.odb2. Plot the undeformed and the deformed model shapes. To distinguish between the different parts, color code the model based on section assignments.Tip: From the toolbar, select Sections from the color-coding pull down menu, as shown in Figure W17 (or use the Color Code Dialog tool to customize the color for each section).Figure W17. Color-coding pull down menu3. Use the Animate: Time History tool to animate the deformation history.4. Display only the seal. In the Results Tree, expand the Instances container underneath the output database file named seal.odb. Click mouse button 3 on the instance SEAL-1 and select Replace from the menu that appears.Abaqus/CAE now displays only the elements associated with the seal.5. Contour the Mises stress of the seal on the deformed shape. If necessary, use the frame selector in the context bar to select the last increment.The contour plot is shown in Figure W18.Figure W18. Mises contour plot6. Contour the minimum and maximum principal nominal strains. Elastic strains can be very high for hyperelastic materials. Because of this, the linear elastic material model is not used because it is not appropriate for elastic strains greater than approximately 5%. 7. Contour the contact pressures. Note that the mesh obscures the contours in the region of self-contact; thus, also extrude the mesh. Use display groups as indicated below to make the mesh translucent:a. Create a contour plot of the contact pressure (in the Field Output toolbar, select Primary from the list of variable types on the left side of the toolbar and CPRESS from the list of output variables in the center).b. From the main menu bar, select ViewODB Display Options. In the dialog box that appears, switch to the Sweep/Extrude tabbed page and toggle on Extrude elements. Accept the default depth and click OK.c. Use the Common Plot Options dialog box to set the deformation scale factor to 0.96 (this will further aid visualization).d. In the toolbar, click the Create Display Group tool .e. In the Create Display Group dialog box, click Save As at the bottom of the dialog box. Name the display group mesh.f. In the Create Display Group dialog box, select Surfaces as the item.g. Select SEALINNER and SEALOUTER. Click Replace and then Save As at the bottom of the dialog box. Name the display group surfaces.h. Dismiss the dialog box.i. In the toolbar, click the Display Group Manager tool .j. In the display group manager, select mesh and click Plot. k. Change the color coding back to the Visualization defaults and change the plot state to display the deformed shape of the seal (click in the toolbox). l. Open the Common Plot Options dialog box and do the following: In the Basic tabbed page of the dialog box, select the Filled render style, and make only Feature edges visible. Change the fill color to light grey (under the Color & Style tabbed page of the dialog box). Activate the Translucency option (under the Other tabbed page of the dialog box); set the translucency level to 0.15. m. In the display group manager, click Lock (next to mesh) in the Display Group Instance field to freeze the mesh display.n. In the display group manager, select surfaces and click Add. Lock the surface display. The plot appears as shown in Figure W19.Figure W19. CPRESS contour plot8. Animate the contour plot (click in the toolbox).9. Display the reaction force history at the reference node of the top rigid surface: In the Results Tree, expand the History Output container underneath the output database file named w_seal.odb and double-click Reaction force: RF2 PI: TOP-1 Node 3 in NSET TOPRP to display the reaction force history at the reference node of the top rigid surface.10. You will now create the CLD curve.a. In the History Output container, click mouse button 3 on Reaction force: RF2 PI: TOP-1 Node 3 in NSET TOPRP and select Save As from the menu that appears. Save the data as Force. b. Click mouse button 3 on Spatial displacement: U2 PI: TOP-1 Node 3 in NSET TOPRP and select Save As from the menu that appears. Save the data as Disp. c. In the Results Tree, double-click XYData. d. In the Create XY Data dialog box that appears, select the Operate on XY data source and click Continue. The Operate on XY Data dialog box appears.e. From the Operators listed in the Operate on XY Data dialog box, select combine(X, X) and then abs(A). Note that the abs(A) operator is used to obtain the absolute values. f. In the XY Data field, double-click the curve Disp. The current expression reads combine(abs(Disp). g. Move the cursor before the far-right bracket, enter a comma, and then select the operator abs(A). h. In the XY Data field, double-click the curve Force. The final expression reads combine(abs(Disp), abs(Force) ). i. Click Plot Expression to plot this expression. j. Save this plot as CLD.11. Customize the plot as follows:a. Double-click anywhere on the chart to open the Chart Options dialog box. In the Grid Display tabbed page, toggle on the major X- and Y- grid lines. Set the line color to blue and the line style to dashed. Change the fill color using the following RGB values: red: 175; green: 250; blue: 185. In the Grid Area tabbed page, select Square as the size and drag the slider to 80. From the list of auto-alignments, choose the one that places the chart in the center of the viewportb. Double-click the legend to open the Chart Legend Options dialog box. In the Contents tabbed page, click to increase the legend text font size to 10. In the Area tabbed page, toggle on Inset. Toggle on Fill to flood the legend with a white background. In the viewport, drag the legend over the chart.c. Double-click either axis to open the Axis Options dialog box. In the X Axis region of the dialog box, select the displacement axis. In the Scale tabbed page, place 4 major tick marks on the X-axis at (use the By count method). In the Title tabbed page, change the X-axis title to Displacement (inch). In the Y Axis region of the dialog box, select the force axis. In the Scale tabbed page, specify that the Y-axis should extend from 0 (the Y-axis minimum) to 250 (the Y-axis maximum). Increase the number of Y-axis minor tick marks per increment to 4. In the Title tabbed page, change the Y-axis title to Force (lbf). In the Axes tabbed page, change the font size for both axes to 10.d. Expand the list of plot option icons in the toolbox:e. Examine the remaining options. Add the following plot title: CLD Diagram. Double-click the plot title to open the Plot Title Options dialog box. In the Title tabbed page, click to change the legend text style to bold. In the Area tabbed page, toggle on Inset. In the viewport, drag the plot title above the chart.f. Click in the toolbox to open the Curve Options dialog box. Change the legend text to Top Surface Ref Point and toggle on Show symbol. Set the color for both the line and symbols to red. Use large filled circles for the symbols. Reposition the legend as necessary.The final plot appears as shown in Figure W110.Figure W110. Compression load deflection diagram Question W5-3: What does the inverted peak near 4 inches of deflection represent?Part 2: Analysis using general contact1. Copy the input file named w_seal.inp to one named w_seal_gc.inp. Edit this input file as described below.2. Edit the step definition to invoke the unsymmetric solver (the unsymmetric solver is generall