Question 8.CS.7: FEA Analysis of a Trailer Hitch Problem A trailer hitch suba...
FEA Analysis of a Trailer Hitch
Problem A trailer hitch subassembly and dimensions of its bracket are shown in Figure 8-38. Loads are applied as shown in Figure 8-39. Analyze this assembly with FEA and determine its stresses.
Given The tongue weight of 998 N acts downward, and the pull force of 4905 N acts horizontally. All material is steel.
Assumptions The frame to which the hitch is bolted is significantly stiffer than the hitch assembly. Bolts are snug-tight with no preload.
See Figures 8-38 to 8-41.
1 The geometry of the part requires a 3-D FEA model if information on stress concentration around the holes is needed. Figure 8-40a shows the part meshed with 8-node, linear hexahedral “brick” elements. Note the finer mesh pattern around the holes. This mesh was refined until the stresses converged to values that changed only slightly with successively finer meshes as was done in Example 8-1.
2 Figure 8-40b shows the boundary constraints applied. The holes at points A and B have the same type of “kinematic constraints” applied as were used in prior examples to simulate a pin or round fastener (here a bolt) in a hole. A node is placed in the center of the hole at the back surface where the bracket touches the frame (not shown) to which it is clamped. Rigid elements attach this central node to all the nodes on the inside surface of the hole. The central nodes at A and B are fixed in x, y, and z.
3 The area at the bottom of the back surface labeled C in Figure 8-40 has all the surface nodes of the bottom two rows of elements fixed in x to represent contact with the frame and prevent rigid-body rotation about the z axis. Note that a superior way to do this would be to provide contact constraints to all the nodes on the back surface that touch the frame. This would account for a possible load reversal that could tend to separate the bottom rows of nodes from the frame. Using contact constraints would then require a nonlinear FEA analysis that would significantly increase computation time. The approach used here allows a linear FEA calculation. (Note that because this part is symmetric about the midplane and is loaded in that plane, a 2-D analysis of the part without any holes would also give good—but less complete—information and would have much shorter run time.)
4 Another node is placed at point D, 40-mm above the top surface on the axis of the hole that accepts the hitch ball. This node is connected with rigid elements to the nodes on the inner surface of the 26-mm-dia hole. Forces are applied to this offset node to represent their application at the center of the hitch ball. This approach makes the implicit assumption that the ball is much stiffer than the bracket (i.e, essentially rigid). If we had been concerned about stresses and deflections in the ball, we could have included it in the model at the expense of model generation and computation time.
5 Figure 8-41 shows the distribution of von Mises stresses throughout the bracket, which range from 11 to 274 MPa. Note the stress concentrations around the holes. Point A at the tangent between the outside radius and the back surface that is clamped to the frame has a maximum principal stress of 75 MPa. This correlates well with the value of 72.8 MPa calculated at the same point with classical cantilever-beam theory in the solution of Problem 4-4e (p. 228) as reported in Appendix D (p. 1007). Note that there are points with higher stresses than this within the part, typically at locations of stress concentration around holes.
