workCONT-WK07-Q-SnapFit1

W7.6Note: 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 snap fit of a clip. The model is shown in Figure W71. Both the clip and holder are assumed linear elastic and are modeled with C3D8R elements using enhanced hourglass control. Frictional contact (m = 0.01) is assumed. The edges of the clip and holder are modeled as sharp. This approximation has been used to illustrate the technique required to model oblique contact involving a sharp corner. Figure W71. Model undeformed configurationPreliminaries1. Change to the ./contact/keywords/snap_fit directory. 2. Open the input file w_snap_fit.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.Contact propertiesFrictional contact is assumed between the parts. The coefficient of friction is 0.01. Use the penalty constraint enforcement method with the default penalty stiffness. The options to define these properties are as follows:*Surface Interaction, name=Friction-0p01*Friction 0.01,*Surface Behavior, penaltyContact interactionsPredefined surfaces are available to facilitate the contact pair definitions. The surfaces are depicted in Figure W72. Note that Clip and Holder are element-based surfaces while leadingEdge is a node-based surface.HolderClipleadingEdgeFigure W72. Surface definitionsEither contact pairs or general contact may be used to define the contact interactions. Regardless of the approach taken, special care must be taken to address expected issues at the leading edge of the holder. Thus, two contact interactions are required (the first one defines contact between the two parts and the second focuses on the leading edge of the holder).The option to define the element-based contact interaction is described first. Choose either the contact pair or the general contact approach, as indicated below. If you prefer to use contact pairs:*Contact Pair, type=SURFACE TO SURFACE, interaction=Friction-0p01 Clip, Holder If you prefer to use general contact:*Contact*Contact Inclusions, ALL EXTERIOR*Contact Property Assignment , , Friction-0p01As mentioned earlier, special care has to be taken when modeling oblique contact involving a sharp corner. The recommended approach is to augment the element-based contact interaction(s) with an additional contact pair in which the nodes on the sharp corner form part of a node-based surface. The node-based surface is then used as a slave surface to enforce contact at the sharp corner. Thus, you will now define a second contact interaction to address contact at the leading edge of the holder, as described below.*Contact Pair, type=NODE TO SURFACE, interaction=Friction-0p01 leadingEdge, ClipStep definitionThe analysis consists of a single general static step. Set the initial time increment size to 1% of the total time period. The step will consider geometric nonlinearity as well as activate automatic stabilization. The default dissipated energy fraction will be chosen as a starting point but the amount of stabilization energy will be adapted throughout the step so that the maximum ratio of stabilization energy to internal energy does not exceed 5% (the default ratio). This will aid convergence when the clip loses contact with the holder (stored elastic energy will be released when contact is lost; in reality this is a dynamic event but we use viscous stabilization as a mechanism to dissipate this energy for a static analysis).The following options define the step and analysis procedure: *Step, nlgeom=YES*Static, stabilize, allsdtol=0.05 0.01, 1.Boundary conditionsYour next task is to define the boundary conditions that will act on the assembly. The position of the holder is fixed while the clip is pushed through it. Predefined sets are available to facilitate the procedure. These are depicted in Figure W73.PushFix Figure W73. Set definitionsThe options to define the boundary conditions are as follows:*Boundary Fix, 1, 3 Push, 1, 1, 6.1 Push, 2, 3OutputRequest 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_snap_fitVisualizing the analysis resultsAfter the analysis is complete, you will review the results using Abaqus/Viewer.1. Start Abaqus/Viewer and open the file w_snap_fit.odb:abaqus viewer odb=w_snap_fit.odb2. Click to plot the Mises stress, as shown in Figure W74.Figure W74. Mises stress distribution3. In the Results Tree, expand the Instances branch underneath output database file named w_snap_fit.odb. Select the clip. Click mouse button 3 and select Replace from the menu that appears to examine only the clip.4. Animate the deformation history of the clip.5. Restore the visibility of all part instances (click in the toolbar).6. Make only the holder visible and plot its undeformed model shape.7. Create an X-Y plot to examine the history of the contact pressure at the leading edge of the holder.a. In the Results Tree, double-click XYData. In the Create XYData dialog box, select ODB field output as the source and click Continue.b. In the Variables tabbed page of the XY Data from ODB Field Output dialog box, select Unique Nodal as the position and select CPRESS ASSEMBLY_LEADINEDGE/ ASSEMBLY_CLIP.c. In the Elements/Nodes tabbed page, choose Pick from viewport as the method and click Edit Selection.d. In the viewpo