2.31 Assignment 12 (a.k.a. The Never-ending Story) Due Wed, Dec 5 at 9:30 am In sheet metal forming operations, a sheet of metal is shaped into a product by plastic deformation. Typically, the sheet is deformed by forcing it to conform to the shape of a rigid die. If the final curvature of the part is not too severe, a simple process that is often selected is the stretch-forming process. In stretch-forming, a sheet is clamped by the grips of a machine, stretched, and wrapped around the die. Because of the elastic-plastic behavior of the sheet material, the deformation imposed on the sheet when it is forced to conform to the die has both an elastic and a plastic component. The elastic part of the deformation is recovered when the sheet is unloaded. This is known as springback. In this assignment we will model a stretch forming operation of an aluminum sheet over a cylindrical die. The aluminum sheet in its undeformed configuration (the blank) is a L=20cm x W=2cm strip in 0.063” gage. The material can be modeled as elastic-perfectly plastic with elastic properties E=70GPa, ν=0.3, and a yield stress σy=300MPa. The radius of the die is Rdie=7cm. The sheet is first stretched along its length by an axial force F=3.2KN, then wrapped around the die by a θL=π/4, and finally unloaded to obtain a final part with a rounded bend of radius RU (@ the midplane), and flat edges opening up to an angle θU . 1) Pen and Paper a) Neglecting the effect of the axial force F (i.e., for F=0), estimate the bending moment M0,L necessary to force the sheet around a radius of curvature (@ the midplane) of 7cm: draw the corresponding strain profile through the thickness, and the stress profile through the thickness, indicating the actual magnitude of strain at the skins of the sheet, and the extension of the elastic core. If you do not remember how to do this, you can find help in the pdf file on elastic-plastic beam bending in the Announcement folder, and/or you can dig up your old 2.002 lab notes. (aaagh!) F F θ L F F θ U L W Rdie RL RU (1) (2) (3)b) Now think about the effect of the pre-stretching force F. What is the strain distribution through the thickness at the end of the pre-stretching step (1)? Sketch it with its numerical value. c) Now when the sheet is wrapped around the die as in (2), with the pulling force F, what happens to the sheet will be a nonlinear superposition of the situation in (a) and (b) Æ you cannot simply obtain the strain and stress profile by summing up the profiles in (a), (b). Try to come up with a reasonable sketch of the actual strain profile and the corresponding stress profile. You do not need to put in actual numbers if you cannot figure out how to obtain them. Remember that plane sections remain plane (i.e. the strain remains linear through the thickness), and that the integral of the axial stress should give you F. Do you expect the actual bending moment in the loaded bent part, MF,L,, to be higher or lower than M0,L? 2) FE model Create an FE model of the forming process. Due to symmetry of the geometry and loading conditions, you can limit your model to ¼ of the actual geometry, imposing the appropriate boundary conditions along the 1-2 and 2-3 symmetry planes. Things to keep in mind as you set up the model: PART: For the sheet metal, you want to create a 3D Deformable Shell Part using Extrusion (Approx size : 0.3). You will extrude in the depth direction, so in the sketch plane the blank profile is simply a horizontal line of length 0.1. Your life will be easier later on if you sketch your part so as to have the symmetry plane coinciding with the 2-axis and the part profile going from (0,0) to (0.1,0). Extrude the part by a depth of 0.01. For the die, you want to create a 3D Analytical Rigid Extruded Shell. Because of the symmetry boundary conditions along the 2-3 plane, you do not need to worry about “nodes falling off the edge of the die” along that plane, and you can actually limit the die to a single quadrant. In the sketch plane the profile of the cylindrical die is ¼ of a circle that you can center for now at (0,-0.07) and then reposition later when you assemble the model. Give it an extrusion depth of 0.02; note that this value is just used for visualization (ABAQUS thinks of this as an infinite cylinder in the extrusion direction). Create a reference point at the center of curvature (PartÆReference Point). 1 2 3PROPERTY : In material properties you have to input the Mechanical props for the sheet. Remember to input both the elastic (E, ν) and the plastic (σy) properties. In section property you want to create a shell homogeneous section of thickness 0.0016m (0.063”). The section properties will have to be integrated during the analysis. In the integration… option, change the number of integration points to 11 (Simpson rule), so as to better capture the elastic-plastic stress profile as the sheet goes plastic. Assign the section to the entire shell (Part-1). Now you want to assign local material orientations, so the stress output tensor rotates with the sheet. If you want the local 1 axis (σ11) along the loading direction, you first need to define a rectangular datum coordinate system: use the ToolÆDatumÆCSYSÆdefaultÆrectangular tool to create a datum coordinate system. Now you can use the AssignÆmaterial orientation tool: select the entire part, and choose the newly created CSYS. Select the Y direction (Axis-2) as the direction that defines the approximate shell normal, with 90 degrees additional rotation, and click OK to confirm the change. Use the QueryÆMaterial Orientation tool to check the material directions. ASSEMBLY : Instance the sheet and the die. With the current geometry, the two parts are coincident along the 3-axis. To start a simulation with parts in contact is a sure way to get in trouble. To avoid problems, create a small clearance between the sheet and the die by translating the die instance down by (0,-0.001,0). Use the InstanceÆTranslate tool to reposition the die. STEP : For this assignment, we are going only to model the loading sequence. (The unloading will be part of the weekly project). We will model the loading history through three loading steps: in Step 1 we will apply the pre-stretch load F. In Step 2 we will bring the sheet down to touch the die. In Step 3 we will wrap the sheet around the die. So you have to create three steps. For each step choose General Static