Revised Sheet Metal Simulation, J.E. Akin, Rice University

Size: px

Start display at page:

Download "Revised Sheet Metal Simulation, J.E. Akin, Rice University"

Jayson Turner
5 years ago
Views:

1 Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis. It does not illustrate engineering considerations that a BS level engineer would probably follow. Here, some of the engineering aspects that were not considered in this study will be mentioned. This simulation failed to acknowledge one of the fundamental concepts in mechanical design: sharp reentrant corners in a material theoretically cause infinite stresses at that corner. This tutorial involves the bending of thin shell elements. Shell theory was developed (circa 1750) to treat thin solids that are primarily loaded in bending. Shell elements were developed about two hundred years later. There are six degrees of freedom (DOF) at each node of a shell element; three displacements and three (infinitesimal) rotations. This contrasts with a solid element which does not model bending and which has only three displacement DOF at each of its nodes. It takes five or more quadratic solid elements through the thickness of a part to accurately model bending in a thin region. The shell mesh is plotted on the middle surface of the part. The stress components in the shell can be, and should be, displayed on the top, middle (membrane), and/or bottom surfaces. As shown in the Figure 1 the middle plane carries the uniform in-plane stresses while bending adds tension stresses on one side and compressive stresses on the other. By default SolidWorks plots the selected stresses on the top surface. Other surface plots can be selected with Results Define a Stress Plot feature. The bending stiffness of a shell or plate element is proportional to the thickness cubed. Figure 1 Combining bending moments and center plane loads on a section The first major assumption, other than the part shape, is how it is supported. Figure 2 shows the part, notes that pressure acts normal to the lower surface, and that three bolt holes will support the part. Those assumptions will be followed initially. However, the three support holes are essentially parallel to the direction of the pressure load so it is more likely that only the top half of each hole will support the part. Furthermore, if a bolt is slightly loose it could loose its ability to support the part. That option should be considered in a later simulation. Page 1 of 11

Figure 2 Part, loaded surface, and support holds The pressure is applied, a fairly uniform mesh is created, and the results are computed.

deformed top surface with continuous varying values.

discrete contours in Figure 3. However, both display formats are essentially blue blobs that convey little information.

2 Figure 2 Part, loaded surface, and support holds The pressure is applied, a fairly uniform mesh is created, and the results are computed. The von Mises stress (actually distortional energy) material failure is appropriate for this steel so its value is plotted first on the deformed top surface with continuous varying values. That does not reveal much detail, so it is redrawn after turning up the ambient light, activating the maximum value, and converting to discrete contours in Figure 3. However, both display formats are essentially blue blobs that convey little information. Thus, the color bar is changed to where the top value is near the original green levels around the support holes. That change is shown in Figure 4. Figure 3 Original (left) and modified display of initial (top) von Mises stress values Page 2 of 11

Figure 4 Changing the color bar better shows the highest (top) von Mises stress level More precise engineering data are obtained by graphing this stress along the edge of the flat plate with the

3 Figure 4 Changing the color bar better shows the highest (top) von Mises stress level More precise engineering data are obtained by graphing this stress along the edge of the flat plate with the pressure load. That graph is in Figure 5, but the kink in the plot near the right end implies that the mesh is too crude in that region. Zooming in on the region where the red contours are (see Figure 6) indeed shows a very crude mesh with only about one element near the highest (top) von Mises stress level. Mesh control was used to create several small elements there (see Figure 7), and the study was re-run. The prior graph was re-drawn in Figure 9. There it is noted that the end slope has gotten much steeper. Is an even finer mesh required in that region? No! Refining the mesh again leads to even higher peak stresses. A basic principle has been overlooked. Figure 4 Kinks in a (top) stress graph suggests that the mesh is too crude Page 3 of 11

4 Figure 6 A mesh zoom verifies large elements are in the high stress region Figure 7 Revised mesh near stress concentrations Page 4 of 11

5 Figure 8 Updated (top) von Mises stress approaching and near the sharp corners The theory of Elasticity (and heat transfer, etc.) shows that if a part has a sharp reentrant corner then the stresses at the corner go to infinity! The rate that the stresses go to infinity depends on the interior angle. A crack (interior angle of 360 ) has the fastest growth rate; while a right angle corner (interior angle of 270 ) has a much slower growth rate. But, any sharp corner leads to theoretical infinite stress values and continuously refining the mesh is just a wasted effort. This is a problem with the original geometric design because the part has several right angle reentrant corners. The correction is simple; just add small fillets to the reentrant corner regions. The corners will still likely be high stress locations, but the stresses no longer go to infinity! The original flat sheet metal part with five sharp reentrant corners is shown in Figure 9, along with corrective small fillets that were added before conducting a new simulation. After the sheet is bent to its final design shape there will still likely be high stresses in the revised regions. Therefore, the part was further modified to add split lines in those regions so that mesh control can be used to force small elements throughout those regions. The split line areas are shown in Figure 10 along with the revised small elements there in the new mesh. Now the entire simulation is ready to be re-run. The corner regions stresses are still high, but are now realistic. The new contours and edge graph results are given in Figures 11 and 12, respectively. However, so far only the top surface von Mises stresses have been illustrated. The middle surface and bottom surface values need to be checked in a similar fashion. For this material the maximum shear stress (Intensity) values and the maximum tensile stress (P1) values should also be check on each of the three shell surfaces. Their middle surface values are plotted in Figures 13 and 14. Page 5 of 11

6 Figure 9 The original part with fillets added at reentrant corners (before bending) Page 6 of 11

7 Figure 10 Filleted corners, split line control regions, an mesh finer mesh Figure 11 Revised part, (top) von Mises stress distribution Page 7 of 11

8 Figure 12 von Mises (top surface) stress graph between now filleted corners Figure 13 The middle surface Intensity (twice the maximum shear stress) values Page 8 of 11

9 Figure 14 The middle surface First Principle (usually maximum tensile) Stress values Page 9 of 11

10 Figure 15 Loose left bolt deflections (bottom) are four times larger Figure 16 Loose left bolt von Mises stresses affect a much larger portion of the revised part Page 10 of 11

11 Appendix: The matrix equilibrium equations, S u = c can be partitioned in terms of the unknown nodal displacements, u u, and the known essential boundary values of the displacements (fixtures) u k : [ S uu S uk ] { u u S ku S kk u } = { c u k r } k where the resultant applied forces (from the pressure) are c u, and the unknown reaction forces at the fixtures are r k. The sub-matrices S uu and S kk are square, whereas S uk and S ku are rectangular. In a finite element formulation all of the coefficients in the S and c u matrices are known. The above matrix equations can be re-written in expanded form as: S uu u u + S uk u k = c u S ku u u + S kk u k = r k so that the unknown nodal displacements are obtained by inverting the non-singular square matrix S uu in the top partitioned rows. That is, u u = S 1 uu (c u S uk u k ). The values of the necessary reactions, r k, at the fixtures can now be determined from r k = S ku u u + S kk u k c k. Next, the displacement gradients are calculated in every element and they are combined to define the strains. Then the material stress-strain law is used to calculate the components of the stress tensor. The components of the stress tensor are then used to calculate the most common failure criteria, like the von Mises stress and the Intensity (twice the maximum shear stress). Page 11 of 11

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to